Docstoc

Logic Creator Schematic Capture Symbol Creator PartSymbol

Document Sample
Logic Creator Schematic Capture Symbol Creator PartSymbol Powered By Docstoc
					     Logic Creator: Schematic Capture
    Symbol Creator: Part/Symbol Editor
Board Creator: Printed Circuit Board Editor
    View Creator: Photo Plotter Viewer
                   and
   Route Creator: PCB Automatic Router




Microsoft Windows 95/98, NT & Windows 2000
Advanced Microcomputer Systems, Inc.
       1377 South Andrew Avenue,
        Pompano Beach, FL 33069

   Web Site: www.advancedmsinc.com
   E-mail: info@advancedmsinc.com
  CIRCUIT CREATOR™ INDEX
Chapter 1 Welcome to The World of Circuit Creator
Chapter 2 Logic Creator Basics
Chapter 3 Logic Creator Schematic Tutorial
Chapter 4 Printing The Schematic and it Reports
Chapter 5 Hierarchical and Flat Design
Chapter 6 Logic Creator Referance Section
Chapter 7 How To Section for Logic Creator
Chapter 8 Symbol Creator Basics
Chapter 9 Creating a Part and Its Symbol
Chapter 10 Part And Symbol Reference Section
Chapter 11 Board Creator Basics
Chapter 12 Creating A Printed Circuit BoardChapter
Chapter 13 Board Creator Reference
Chapter 14 Creating A Thd Footprint (Through Hole Device)
Chapter 15 Creating A Smd Footprint (Surface Mount Device)
Chapter 16 Creating Gerber Photo Plotter File
Chapter 17 How to Section for Board Crator
Chapter 18 Using the Automatic Router
Chapter 19 View Creator General Help
CIRCUIT CREATOR "Hot-Keys"
Frequently Asked Questions
                                                                               1



Chapter 1
Welcome to the World of Circuit Creator
From Sketches to Schematics
   When a company decides on the creation of a new product, the design of the
   electronic circuitry is naturally assigned to the engineering department. The
   electronic engineering group(s) will design the different circuits and draw
   rough sketches on paper. These sketches will become the source of information
   for the engineer or technician who will create a schematic diagram using a
   CAD program like Logic Creator. These sketches are usually incomplete and
   the technician may have to look up parts in data books for pin numbering and
   pin names for example. Familiarity with data books and parts catalogs will
   greatly help in the process of drafting the schematic. If you are not very
   familiar do not worry because you will see several detailed examples through
   this book.

Manual Drafting or Computer Aided Drafting?
   Electronic schematics show how electronic parts are interconnected in order to
   accomplish the goals of the design. The schematic will become the source of
   information, which other programs like Board Creator will need to operate on.
   The schematic will also be used in the documentation associated with the
   product. A copy of the schematic(s) will appear in the Technical Manual of the
   product for after sales service. Engineering and manufacturing requirements
   may also be shown on schematics.

   Until recently, design engineers and draftsmen drew schematics by hand. This
   method was quite effective, but it was slow, tedious, and revisions to the
   schematic drawings were difficult to make. Changes often forced the
   redrawing of the schematics from scratch. Unfortunately, this allowed new
   errors to enter into the design. The productivity of the draftsperson was very
   low because of these reasons.
2

    The next major advancement in schematic technology was the invention of
    computer aided drafting (CAD) systems. These systems made the drawing of
    the schematics faster, easier, and modifying the original could make revisions
    to the drawings. However, the first CAD systems were very expensive because
    they could run only on mainframe computers. The cost of that CAD software
    was often more than $100,000. They also required highly trained people to
    operate the equipment, and the drawings were still just drawings. They
    contained no internal information about the design represented by the
    drawings.

    Next came the introduction of systems, which could draw schematics and also
    recognize the information represented by the schematics. Although these
    systems worked reasonably well, they were still expensive, required highly
    trained operators, and required the purchase of equipment, which was
    dedicated to this one application. With the invention of the personal computer
    and the dedication of some clever programmers and designers, electronic
    schematics can now be created, edited, and processed effectively on a personal
    computer or engineering work-station.

    The Logic Creator schematic environment represents the state-of-the-art for
    electronic schematics on a personal computer. It may be used to draw and
    revise schematic drawings, check the drawings for errors, generate engineering
    and manufacturing reports such as a parts list, a net list, and a bill of material.
    It also produces hard-copy prints of the schematics, and can generate (in
    computer form) the data required to layout and update a PC board.

What schematic diagrams are?
    As was previously mentioned, schematic diagrams are drawings of electronic
    designs, which show the symbols of the parts used in the design and the how
    they are logically interconnected.

    If you look at a typical schematic diagram, you will see three types of
    information: symbols of parts, connection lines, and annotation (a fancy word
    for notes). Do not let anyone kid you; all schematics are made up of these
    simple elements. So how do we create a schematic diagram? You place
    symbols of the parts on the sheet, draw lines to wire the symbols together, and
                                                                                      3

     add any special notes that apply to that particular sheet of logic. Sounds easy?
     The schematic capture process is simple. This does not imply that the design of
     an electronic circuit is simple. A good designer is a highly trained and skilled
     individual. The actual design of a circuit initially resides in the brain of the
     designer. Logic Creator allows that information to flow from the designer's
     imagination onto a schematic drawing. The designer is now allowed to
     concentrate on designing, and relieved of the burden of manually drawing the
     schematics.

     On a typical schematic, the part symbols will account for about 90 percent of
     the drawing effort when drawn by hand. In the Logic Creator system, the
     symbols representing the electronic parts, along with additional packaging and
     electronic data, are supplied in the form of parts libraries. If required, the user
     may add new or custom parts. Since the part symbols are pre-drawn for you in
     the library, you can add a part to your schematic with just a few keystrokes or a
     click of the mouse. Most of what you see on a typical schematic is actually
     pre-drawn for you. This is a tremendous advance in productivity and accuracy.
     Create a part/symbol right once, and use it over and over.

Hardware and Software Requirements for Circuit
Creator CAD System
     The Circuit Creator CAD system runs on IBM or compatible personal
     computers. Make sure that you have the following minimum hardware and
     software facilities in your computer system before loading the software:

A)   Hardware:
     1.   Pentium Microprocessor
     2.   15 M Bytes of free hard drive space.
     3.   16 M Bytes of RAM
     4.   Color VGA monitor
     5.   Mouse
     6.   104 Standard Key board
4

B)   Software:
     1. Microsoft Win95/98, 2000, 2000 XP Operating system

     If your system has the above minimum requirements then lets proceed with the
     installation of Circuit Creator.

Installation of the Circuit Creator system
Installation Of Software
A)   CD-ROM Installation
     If you received this software on a CD-ROM you can simply put the CD into
     your drive and the installation should start automatically. If it doesn't then run
     setup.exe off the CD.

B)   Downloaded from Web
     If you downloaded the demo from the web then run the file
     "cktcrt_demo.exe".

     In both cases the installation program with ask the name of the directory where
     you wish to install the demo. You can use the default (CKTCRT) or give it any
     name you wish. The same goes the for name of the Program (Start Menu)
     Group.



                Figure 1-1: Windows 98 Start Menu Tiltle Bar

     To start any of the programs go to Circuit Creator program group (on the Start
     Menu) and click on the appropriate Circuit Creator icon.

     If you have any problems using the Start Menu, consult your Microsoft WIN
     95/98 Users Manual.
                                                                              5

From this point on we will start the interactive tutorial sessions. In other
words, I will be explaining a function of the program and then I will ask you to
perform the same function with detailed step-by-step instructions. These
instructions will be enclosed in a special text box like the one below:




            Figure 1-2: Circuit Creator Program Folder

As you become familiar with the system the text boxes will become less
frequent. They will still be used when an important feature is explained. Inside
the Circuit Creator program group there are six icons.

The four main modules of Circuit Creator are Logic Creator, Symbol Creator,
Board Creator, and Route Creator. Logic Creator is the schematic drafting
module. It enables you to create or modify schematic diagrams. Symbol
Creator is the symbol and part module. It enables you to create or edit symbols
of electronic devices. Board Creator is the printed circuit board and footprint
module. It enables you to create the printed circuit board artwork or create
footprints for new electronic devices. Route Creator is the automatic router
module. It enables you to automatically route the printed circuit board instead
of doing it manually.

The other two icons, Gerber-View and Photo Plotter Setup are utilities of
Circuit Creator. To start any one of the three programs you simply double click
anywhere on its icon. I know how anxious you are to start using this amazing
6

    software but don't do it just yet. Be patient until you are instructed to do so.
    Read on for some important information that follows.


Circuit Creator System: Overviwe
    This section gives you an overview of the entire Circuit Creator system. A
    brief description of each of the major components, and how they interact with
    each other is presented.

Logic Creator: Schematic System




                          Figure 1-3: Logic Creator

    The Logic Creator schematic system is a high-end electronic schematic entry
    system. It is used to create and/or update electronic designs. It also is used to
    directly print schematics, generate electronic reports of designs, and to
    generate a data file that is used by the Board Creator PC board layout system to
    create the initial PC board for a design, or to update an existing design.
                                                                                 7

Board Creator: PC Board Layout System




                         Figure 1-4: Board Creator

    The Board Creator system is used to layout PC board designs. This system is
    used to create, edit, and maintain the layout masks for PC board designs, print
    the masks to printers, plotters, and photo-plotters, maintain the component
    footprint symbols, schedule routes for the auto-router, and to print net lists,
    part lists, and other PC board specific reports. Also, the program can check a
    PC board layout for agreement with physical design rules. Such things as
    clearances of lines to pads, lines to lines, lines to vias, as well as numerous
    other checks are performed.
8

Route Creator: Auto-Router




                        Figure 1-5: Route Creator

     The Route Creator program is used to automatically route the electrical
     connections of a PC board. The auto-router uses a method of artificial
     intelligence to automatically route the paths of electrical connections. The
     auto-router will preserve any nets that you wish to pre-route manually. Also,
     the auto-router allows for being interrupted, manually editing the board with
     the editor, and continuing the automatic routing.
                                                                                9

View Creator: Gerber Viewer




                         Figure 1-7: Gerber Viewer

     The View Creator program may be used to preview Gerber photo-plotter files
     on the computer screen, prior to actually printing the files.

Circuit Creator Program Specification
     The following is a summary of the specifications for the Circuit Creator
     system.

Systems wise Feautres
     •   Runs on IBM PC, IBM PS/2 and compatible computers with WIN 95/98
         2000 Operating System.
     •   State-of-the-art, object-oriented user interface with pull-down menus and
         pop-up dialog boxes. Dynamic point, click and drag editing.
     •   On-line and context-sensitive help.
     •   Automatic "check-pointing" of the work in progress. Protects against loss
         of work in the event of a power failure. Time between check-points is
         controlled by configuration.
     •   Complete user manuals with tutorials for all the major subsystems.
     •   Video support for EGA, VGA, and Super-VGA and many other display
         devices supported by WIN95/98 2000 System..
10

     •   Hard copy support for PostScript, Epson, Hewlett-Packard, IBM, Gerber,
         and many other printers/plotters supported by WIN95/98 2000 System..
     •   Parameters such as the default path for drawings, memory usage, default
         width of lines, display colors, etc. may all be configured.

Schematic Entry
     •   A complete electronic schematic working environment in a single program.
     •   True hierarchical designs. Each hierarchy level has independent net naming
         and pseudo-part reuse capability.
     •   Fully compatible with the Board Creator printed circuit board system.
     •   Up to 32 E-size sheets of logic in a single design, even more through the
         use of hierarchical designs.
     •   Comes with standard part and symbol libraries. Over 25,000 part/symbol
         combinations and can be expanded by the user.
     •   Symbols may be dynamically mirrored and/or rotated. A single symbol
         definition may be displayed in any of sixteen different orientations. No
         need to make separate symbol definitions for different views.
     •   DeMorgan equivalents and more. A single part may be represented by
         many different symbols. Rotation and mirroring of part symbols from a
         single definition. Symbols are based on true geometric definition, not a
         raster image.
     •   Automatic re-routing of connections when objects are moved. Not just "air-
         lines", but true schematic routing via use of "smart-lines".
     •   Bezier curves for true curved lines, not just arc segments.
     •   Electronic/printed design reports of parts-list, net-list, loading, design
         verification, etc.
     •   Direct design error checking. Errors are pointed out directly on the
         schematic with an explanation of exactly what the problem is.
     •   "Double-click" to update any object on the schematic.
     •   Supports hierarchical drawings and full hierarchical net naming
         conventions (inheritance).
                                                                                11

PC Board Layout
    •   A complete electronic printed circuit board layout working environment in
        a single program.
    •   Fully compatible with the Logic Creator schematic system. Imports other
        Schematic and PCB files.
    •   Boards up to 32 x 32 inches, 255 layers.
    •   Comes with a complete set of standard foot-print part symbols, including
        surface-mount devices.
    •   Foot-print symbols may be dynamically rotated and/or mirrored to the back
        of the board. No need to make separate symbol definitions for different
        orientations or board sides.
    •   "Double-click" to update any object on the board.
    •   Support for blind and buried vias.
    •   Support for power and ground planes.
    •   "Copper pour" command for filling unused areas of a board with
        conductor, such as power or ground. Can be selected and removed as a
        single unit, or edited as individual lines.
    •   Direct design and clearance error checking. Errors are pointed out directly
        on the screen. Checks that all points which should be connected are
        actually connected to each other. Checks for nets improperly connected
        (shorts). Checks for pad-to-pad, pad-to-via, pad-to-line, via-to-line, and
        line-to-line clearances. Component, solder side, and inner layers may have
        different clearance rules.
    •   Lines 0.001 to 0.255 inches wide.
    •   Up to 50 different pad shapes and sizes per board. users may define their
        own pad shapes. Different layers of the same pad may have different
        shapes.
    •   Text in 16 combinations of rotation and mirroring. Eight degrees of
        boldness.
    •   Bezier curves for true curved lines, not just arc segments.
    •   Arcs and circles.
    •   Built-in report generator for net-list, part-list, drill-hole, etc.
12

     •   Built-in hard copy output allows queuing of up to ten plots.
     •   "Rat's nest" prompting to aid in optimal component placement and manual
         routing of nets.
     •   User specified layout grid.
     •   Users may work in mils, inches, or millimeters, and switch at any time.
     •   Can create/update an Circuit Creator board from the following net/pin list
         formats: Circuit Creator, Schema, Orcad, Futurenet, Pcad.
     •   Can create a net/pin list from an Circuit Creator board in the following
         formats: Circuit Creator, Schema, Orcad, Futurenet, Pcad, Applicon Bravo,
         Applicon Leap, Computervision, Calay, Cadnetix, Scicards, Spice, Telesis,
         Vectron, Multiwire, and Excellon drill list.

PC Board Auto-Router
     •   Fully compatible with the Board Creator printed circuit board system.
     •   Routes multi-layer boards, two layers at a time.
     •   Routes boards with different line widths, such as wide lines for power and
         ground, and normal lines for other nets.
     •   Router respects nets pre-routed (manually) by the user.
     •   Router may be interrupted, board edited with Board Creator, and restarted
         to finish the routing.
     •   User selectable routing parameters for line width and clearances.
     •   User selectable routing strategies.
     •   Visual display of the routing progress.
     •   Full support for routing blind/buried vias.
     •   Routing schedule may be generated automatically with Board Creator, by
         hand, or any combination of the two.
     •   Routing schedule may specify routing to a specific layer. This is required
         to route to edge connectors and SMD devices.
     •   Uses a proprietary, state-of-the-art, artificial intelligence algorithm to route
         the nets. Routing completion rates are matched only by mainframe and
                                                                                 13

        high-end work-stations routers costing much more and requiring very
        expensive equipment.

Customer Support
    •   Free Email and Fax support during normal business hours.
    •   If you sign up for our yearly update service, you will receive all scheduled
        program revisions as they become available.
    •   If you decide not to sign-up for the yearly update service, you can always
        get the latest revision of any Circuit Creator program for a small update
        fee.


How Circuit Creator Interfaces with the User
    All the programs in the Circuit Creator family share a common windows
    graphical user interface (GUI). Once you learn a few simple principles, you
    can efficiently use any of the programs in the entire system. This interface is
    designed to be consistent throughout all commands and operations. To avoid a
    confusing amount of redundant information, the procedure required for the
    user to interact with this interface is described here once.

    1. Move the mouse pointer so that the tip of the arrow is anywhere within
       the icon.
    2. Double click the left mouse button. What you have now in front of you
       is the opening screen of Logic Creator should look like figure 1.8
14




                Figure 1-8: Logic Creator Opening Screen

Using the Keyboard
     The keyboard is the most direct way of communicating with the program.
     Simply typing keys on the keyboard does this. The following notation is used
     to indicate keyboard-typing sequences.

     •   "XYZ" indicates to type the characters X, Y, and Z.
     •   ENTER indicates to press the key on the keyboard labeled ENTER.
     •   ESC indicates to press the key labeled ESC.
     •   X indicates to press the X key.
     •   ALT+X indicates to hold down the ALT key and press the X key.
                                                                                   15

Using the Mouse
   The mouse is the most efficient way of communicating with this program. The
   mouse is used to select commands and to indicate position.

   •   Pressing and releasing a mouse button is referred to as clicking that button.
   •   Clicking the left mouse button is the same as pressing the ENTER key on
       the keyboard.
   •   Clicking the right mouse button is the same as pressing the ESC key.
   •   The arrow that moves on the screen when the mouse is moved indicates the
       position of the mouse. Moving the mouse pointer changes the current
       position. For most programs, the coordinate of this position is shown in the
       upper-right corner of the title bar window.

   Now, let's start Logic Creator and apply some of this information.

   Let’s take a tour of the opening screen of Logic Creator. Starting from the top,
   the first line obviously displays the title of the program currently running under
   windows, which in this case is Logic Creator. This line is called the Title bar.
   As soon as we create or load an existing file in Logic Creator, the file name
   will be displayed to the right of the Logic Creator on the title bar. On the left
   corner of the title bar the little square with the horizontal line in the middle is
   called the Control-menu box. By clicking on this you can resize, move,
   maximize, close windows, and switch to other programs. There are two buttons
   on the right hand side of the Title bar. The one with the down arrow is called
   the minimize button, and the other one is called the maximize button. You can
   use the mouse to click the maximize button so that Logic Creator fills the
   entire screen, or click the minimize button to reduce Logic Creator to an icon.
   When you reduce the program still runs in the background, you have not exited
   the program yet. To resume or maximize, simply double click the Logic
   Creator icon, which should be located on the bottom left corner of the screen.
   On the right side of the screen we have the vertical scroll bar and on the
   bottom side we have the horizontal scroll bar. These two bars with their arrows
   and the little boxes allow you to move the schematic into the viewing area
   when the entire schematic does not fit in the window. Now let's practice some
   of these movements around the screen. Follow the instruction below carefully.
16

     In case you make a mistake and you get to unfamiliar territory try pressing the
     escape <Esc> on the top left corner of your keyboard or the right mouse
     button. They both perform the same function.

     They move you back to the previous stage in the program. The large blue are
     on your screen is called the edit window. That's where all your schematics will
     be created. It will also change appearance as soon as you create a file.

     1. Click on the Control box to pull down the control menu. Take look at
        the available options.
     2. Move the mouse pointer outside the pull menu and click anywhere in
        order to roll-up the menu.
     3. Click on the maximize button to make Logic Creator fill the entire
        screen


Pull-down Menus
     The second line of the screen is called the Menu bar. By clicking anywhere on
     the menu title you pull down its options or commands. Then you click the one
     you wish to execute. Pull-down menus are lists of commands that appear to
     pull-down from the words that appear in the title-bar.

     •   To pull-down a menu, hold down the ALT key and type the character that
         is underlined in the title of the menu. With the mouse click on the menu
         title with the left mouse button.
     •   While a pull-down menu is displayed the,         and     keys may be used to
         move to the next menu to the right or left of the one displayed. To select a
         command from a menu, move the position indicator with the arrow keys
         (NumLock must be off). Press Enter, or click with the left mouse button, to
         make a selection. This is referred to as executing or starting a command.
     •   To make a quick selection with the mouse, position the pointer on the
         menu title and press the left mouse button, but do not release it yet. While
         the button is still down, move the pointer to the desired menu item and
         release the button to make the selection.
                                                                             17

•   If a menu item has a key indicated in the right margin, then this command
    has a hot key. The hot key may be used to execute the command without
    selecting it directly from the menu. For example, in the Logic Creator
    program, the DRAW/WIRE command indicates a hot key of W. The wire
    command may be executed by just typing W when no menu or dialog-box
    is displayed.
•   If a menu item appears fuzzy or grayed-out, this indicates that this
    command cannot presently be executed.
•   To close a menu without making a selection, press the ESC key or move
    the mouse pointer completely out of the menu and click (or release) the left
    mouse button.

1. Click on the FILE menu, to pull it down. Then use the up and down
   arrow keys to move the highlight from one command to the next.
2. Click anywhere outside the file menu to close it or press the escape
   button.
3. Repeat steps 1 and 2 for all the menus of the menu bar.

OK! I am sure you are ready for some practice by now. Go ahead and follow
the instructions of the text box below.
18




      Figure 1-9: Shows the File menu pulled down in Logic Creator.

     The horizontal area under the menu bar is called the tool bar. It consists of
     many buttons with different icons on them as shown in the figure below.




                           Figure 1.10: The Tool Bar

     Each icon represents the function of the button or tool. There is a button for the
     most frequently used commands. For example the right most button is the Print
     tool. By pressing it the print dialog box appears. In other or words you do not
     have to pull down the File menu and then click on the Print command. A click
                                                                                19

   of the Print tool does all of this for you. Read carefully the function of each
   tool in figure 1.9. You may have to refer to this figure later on when you start
   creating schematics with Logic Creator.

Dialog-Boxes
   Dialog-boxes are forms that pop-up on the screen in response to commands
   that need additional information from you. They display various field names
   and the values. A dialog-box allows these values to be changed. Dialog-boxes
   are very efficient because a single dialog-box may allow the setting of several
   values common to a specific topic.

   The dashed rectangle outlining a field or button name is called the focus
   indicator. Use the TAB, BACK TAB, arrow keys, or the mouse pointer to
   move the focus indicator to the desired field.

   •   Moving the focus to the button and pressing ENTER presses a button. With
       the mouse, just point at the button and click the left mouse button. You
       may also press a button by holding the ALT key down and typing the
       underlined letter in its name.
   •   Most dialog boxes have an OK and a CANCEL button. When all the values
       shown in a dialog-box are set as desired, press the OK button to accept the
       values and close the dialog-box. All changes made in a dialog-box are
       temporary until the OK button is pressed. Pressing the CANCEL button
       will exit the dialog-box and ignore any changes that were made to the
       values while the box was displayed.
   •   The HOME key may be used to set the focus to the OK button. The END
       key will set the focus to the CANCEL button.
   •   If the focus is not already on the CANCEL button, ESC will set the focus
       to the CANCEL button. If the focus is already on the CANCEL button,
       ESC will close the dialog-box (same as CANCEL).
20




                 Figure 1-11: The Select Object Dialog Box

     •   To directly select a dialog-box field, hold down the ALT key and press the
         key for the letter that is underlined in the field label.
     •   To enter a value for a text or number field, move to the desired field and
         begin typing the new value. Press ENTERS when you are finished entering
         the value. Pressing ENTER while the focus is on a text or number field will
         allow you to edit the current value. The INS key may be used to toggle
         between insert and replace mode.
     •   Radio button fields (circles) are used to select one-of-several, while check
         boxes (squares) are used to enable or disable a specific selection. For these
         types of fields, move the focus indicator to the desired field and ENTER or
         click the left mouse button to make the selection.
     •   List box fields are used to select an item from a list of items, similar to a
         menu. Use the , , HOME, END keys, or the mouse pointer to position
         to the desired item. ENTER or click the left mouse button to make the
         selection.
     •   Pop-up menus are also used to select a value from a list of items.
                                                                                21

Context Sensitive Help (F1)
    Context sensitive help is a very powerful feature of Circuit Creator. It allows
    you to receive specific help on the screen about the command you are about to
    use. What you have to do is activate the command or menu you need help on
    and then press F1. The help window will open with all the available
    information for the command right in front of you. You can use the scroll bar
    to move around the help window. The help window has it own menu bar,
    which you can use like the Logic Creator menu bar. To properly exit from help
    pull down the help control menu and click on Close or pull down the FILE
    menu and click on EXIT.




                   Figure 1-12: The Help Dialogue Box

    Please use the context sensitive help whenever you need help. It is easy,
    instant, and right there in front of you. Lets practice now
22


            1.  Click on the File menu to pull it down.
            2.  Select the Print command
            3.  Press F1
            4.  Read the information in the help window.
            5.  When done, pull down the File menu and then click on Exit..
            6.  Let's see how you can receive help on the View menu.
            7.  Close any pulled down menus by clicking anywhere on the work-
                area.
            8. Click on the View menu to pull it down.
            9. Click on any command you wish to activate it.
            10. Press F1. Now you are in the help window. Read the information.
            11. Click on the File menu and then select Exit.


Cursor Commands
     Most of the programs use an edit cursor. This is the little "+" that appears in
     the edit window. It is used to indicate the current position for editing within
     this window. The coordinate value of the position is always shown in the
     upper-right corner to the title-bar window. Please note that this cursor is not
     always the same as the mouse pointer. The edit cursor applies only to the edit
     window. The mouse pointer may be moved all over the screen.

     The easiest way to move the cursor is with the mouse. The cursor will follow
     the mouse as it is moved.

     The arrow keys may also be used to move the cursor in steps of one tenth of an
     inch about the screen. This is the default unit step in Logic Creator.

                           Move right one cursor unit
                           Move up one cursor unit
                           Move left one cursor unit
                           Move down one cursor unit
                                                                       23

Holding the SHIFT key down and pressing one of these arrow keys will cause
the cursor to move one inch, or ten units at a time.
24
                                                                                 25



Chapter 2
Logic Creator Basics
Introduction to Logic Creator
    This Chapter will introduce you to Logic Creator, the schematic editor of the
    Circuit Creator CAD system. You receive a guided tour of Logic Creator,
    examine all its menus and commands, and learn what is their purpose. You will
    also learn how to navigate through the different screens, and how to get out
    safely return to the opening screen from any other screen.

Launching Logic Creator
    You launch Logic Creator from the Windows Start Menu. Look for the Circuit
    Creator Start Menu Group and then click on Logic Creator to launch it.

    To familiarize you with Logic Creator we have a schematic that was created at
    AMS Inc., and was shipped with your disks. We will load this sample
    schematic and learn how to navigate around the screen. Before we proceed
    though let's review how to select commands from the pull-down menus and
    pop-up dialog-boxes.

    If you are using a mouse, you may pull-down a menu by moving the pointer to
    the menu name in the title-bar and pressing the left mouse button and releasing
    it. The menu will appear when the button is released. To select a menu item,
    move the pointer to the desired item and press the left mouse button and
    release it. The selection is made when the button is released. For quicker menu
    selections, move the pointer to the title and press the left mouse button and do
    not release the button yet. Now, move the pointer to the desired menu item
    and release the button to make the selection.

    If you are using the keyboard a pull-down menu may be displayed
    (pulled-down) by holding the ALT key down pressing the key indicated by the
26

     underlined character in its name on the title-bar. Upper or lower case may be
     used.
     When a pull-down menu is displayed, the and arrow keys may be used to
     move to the next menu to the right or left. The NUMLOCK key must be off.
     Use the and arrow keys to move the menu selector up and down. Move to
     the FILE/OPEN command and select it by pressing the ENTER key.

     After selecting the FILE/OPEN command, a dialog-box will appear which is
     prompting for the name of a schematic file.

     At this point, we can type the file name of a schematic file, or select one from
     the list that is displayed. Double click on the file named "DEMO.SCH" or click
     once and then press the OK button to open it. Here is a summary of what you
     need to do:




                  Figure 2-1: The FILE/OPEN Dialog Box

     1. Launch LOGIC CREATOR by double clicking its icon.
     2. Click on File to pull down its menu.
     3. Click on Open.
                                                                                27

   4. Click on DEMO.SCH to open it up (see fig.2-1).
   5. You should have now in front of you the screen of figure 2-2.

   When a dialog-box is displayed, clicking the left mouse button on the OK
   button, or pressing the ALT-O key combination will immediately accept the
   values in the dialog-box. Clicking on the CANCEL button, or pressing the
   ESC key will immediately cancel the dialog box. Any changes made to the
   values shown in a dialog-box do not actually take effect until the OK button is
   pressed. If the cancel button is pressed, the changes made to values in the
   dialog-box are ignored.

   For a file-selection or part-selection dialog-box, pressing ENTER twice while
   on the same name in the list implies that this is the name you want to accept
   immediately.

   Context sensitive help is always available by highlighting the command you
   need help on and then pressing F1.

Screen Presentation
   The screen is divided into several windows, as shown in the figure 2-2. Each
   window contains a specific type of information.

   The top area of the screen is the title-bar. This line displays the name of the
   program, the file currently being edited and the current cursor's location.

   Just down from the top is the menu or action-bar. This bar displays the title of
   each of the pull-down menus assigned to it.

   Under the menu bar you see the tool bar, which consists of several little
   buttons with different icons on them. These buttons allow us to execute several
   of the most commonly used commands sequences at the click of a button. This
   increases our productivity considerably.
28

     The bottom area of the screen is the command status window. This line
     displays the current command that is active, and additional values and sub-
     commands that are of particular interest for this command.
     The center area of the screen is the editing window. It is used to display the
     schematic that is currently being edited. Also, dialog-boxes may pop-up in this
     area from time-to-time.

     The editing window is bordered on the top and left with rulers to assist in the
     location and positioning of items.

     Editing window is bordered on the right and bottom with slide-bars. The slide
     bars are used in conjunction with a mouse to change the view of the edit
     window. The view may also be set by keyboard and menu commands.




               Figure 2-2: DEMO.SCH displayed on screen

Navigating Around the Screen
     What you see in figure 2-2 is only the top left corner of the schematic because
     not all of it can fit on the screen. Think of your screen as a window that you
                                                                              29

look through to see the schematic. Right now you are the one to one (1:1) of
magnification. We can ZOOM OUT and look at the schematic from a distance.
This will allow us to see more of the schematic but we loose in clarity and
detail. The easiest way to zoom out is to click on the button with the
magnifying glass having the minus (-) sign inside. It is located under the
VIEW menu.

Go ahead and do that. The whole schematic is still not contained in the screen.
You can ZOOM OUT again by pressing the same button once more. Now you
can see the whole schematic but no parts are discernable. Viewing at this level
is useful when you are planning the placement of the components when you
start a new schematic. It is also useful for checking the overall appearance and
symmetry of your schematic after you finish drafting it. To zoom back to the
previous level click on the button with the magnifying lens the plus (+) sign.

You can zoom in and out using the keyboard too. Here is how. Pull-down the
VIEW menu now move down and select the ZOOM OUT command. The
display will be redrawn at a smaller scale. You will notice that the ZOOM
OUT menu item has CTRL+PGDN listed in the right margin next to it. This
indicates that this command has a hot-key. This key combination may be used
when the menu is not displayed to directly execute this command. Let's try it.
Now, hold the CTRL key down and press the PGDN key to zoom-in. Once you
are more familiar with the program, using hot-keys will improve your
productivity, especially if you do not have a mouse. Zoom back to the original
scale by pressing the CTRL+PGUP key twice.

The current coordinate of the cursor is displayed in inches in the upper-right
corner of the screen. Use the cursor keys to move the cursor to coordinate
(2.000,1.000). Follow the track of the cursor on the screen, and watch the
value in the upper-right corner change. Notice that the active cursor (the little
cross) is not always the same as the mouse pointer position. When you press
the arrow keys the cursor moves 0.1" at a time. This is its smallest step.

Holding the SHIFT key down and using the cursor keys will move the cursor
one inch at a time. Hold the SHIFT key down and use the ← and ↑ arrows to
30

     move quickly to coordinate (0.000,0.000), the upper-left corner of the sheet.
     Did you notice that the cursor now moves in one-inch (1.0") steps?

     The display may be panned using the keyboard by bumping into one of the edit
     window edges. Let's pan right. Move the cursor with the SHIFT → key until it
     bumps the right edge of the window. The portion of the schematic that was out
     of view to the right of the screen is now displayed.

     With a mouse, the view may be panned by using the vertical slide-bar at the
     right, or the horizontal slide bar at the bottom. Display the upper-left corner of
     the sheet at normal scale by pressing Ctrl + Home.

Reference Grid
     The lines, normally green, that you see on the screen represent a reference grid.
     This grid is used to assist the user in drawing a schematic and lining up
     objects. It is not part of the schematic itself, and is not printed on hard-copy
     output. From the VIEW menu, select the GRID command. This dialog-box is
     used to control the display of the reference grid, and the step size of the cursor
     movements. Select the check-box entry for DISPLAY so the X check mark is
     off. Now, select OK. Notices that the grid lines no longer appear in the display;
     however, the cursor-motion grid is still active.

     A single Logic Creator design file may have several sheets of drawings. This
     demo drawing has two active sheets. From the VIEW menu, select the SHEET
     command. Now, from the list, select sheet number two by double clicking on
     it. Sheet two is now shown on the display. ZOOM OUT two times in order to
     see what's on the sheet. Move your mouse pointer in the middle of the
     schematic and press CTRL + PageUP to zoom in that spot. Do this twice. At
     this point, the magnification level is one to one.

     When starting a new schematic it may be more helpful at the beginning to use
     grid spacing of 0.1" (100 mil), because all component input and output pins
     will coincide with a grid line. The reason for this is Symbol Creator. When a
     part is created in Symbol Cretor, all its inputs and outputs are automatically
     positioned on multiples of 100-mil spacing. For example you will find a pin on
     position 1.2", or 3.7", or 7.5", but not at locations like 1.25", or 3.75". This is
                                                                                  31

   also the smallest grid spacing possible. Go ahead and experiment with different
   grid sizes and see the effect on the screen. The hot Key for GRID is G!

The Select Command
   The select command is the default Logic Creator command. That is, when no
   other command is active, the select command is active by default.

   The select command is used when you want to make changes. It is used to
   point out which objects you want to change. Before an object can be changed,
   it must first be selected. Once selected, an object may be deleted, moved,
   stretched, or updated.

   For example, if you want to delete a part from a schematic, first select the part
   you want to delete and then press the Del key. If you want to move an object
   on a schematic to a new location, first select the object, then grab it with mouse
   and move it to the new location.

   To select an item, or group of items, first pick the Select command from the
   Edit menu, or just Esc the current command to start it by default.

   To select a single object, move the cursor on top of the object you want to
   select and press the Enter key twice. With the mouse, just point at the object
   and click the left mouse button. When an object is selected, it will appear on
   the schematic in the configured select color.

   To select more than one object, move the cursor to one corner of the area that
   bounds the objects and Enter. Now, move to the other corner and Enter again
   to select all the objects within this area. With the mouse, hold down the left
   button and move the mouse to stretch-out the desired area. Release the button
   to select the objects.

   Use the O key, or click on the status line with the left mouse button, to pop-up
   the select options dialog-box. This dialog-box allows you to control which
   objects will be selected, and which objects will not be selected.
32

     When touching is active, any objects touching the selection area will be
     selected. When bound-by is active, only the objects completely bound by the
     selection rectangle will be selected. When component is active, selecting a part
     symbol will also select any other objects that connect to this symbol. This
     makes it easy to drag a symbol, along with the lines and net names that connect
     to it. When flat is active, only the symbol is selected.

     Each individual object type that appears on a schematic may be enabled or
     disabled for selection.

     To unselect, make a new selection, select in an area on the screen where there
     are no objects, or pick the Edit/Unselect command.

     Once an object is selected, the following operations may be applied:

     •   CUT, COPY, ERASE, UPDATE - Refer to the specific command.
     •   MOVE/DRAG - Press ENTER while the cursor is within the select area
         indicator, and then use the arrow keys to move/stretch the selected objects.
         ENTER again to place the objects (stop moving). With the mouse, press
         the left mouse button down and drag the objects to the new location.
         Release the mouse button to place the objects.
     •   STRETCH - Selecting only the portion of the object that you want to
         move may stretch Lines, wires, and buses. For example, if you only select
         one tip of a line, then the end of the line will stretch as it is moved. The
         other end of the line will remain anchored. This technique may be used to
         quickly reshape wires and bus lines.

     As you can see, the select command is a very convenient and powerful
     command that works in combination with other commands. All editing
     changes are done through the use of the select command.

Unselect (Z)
     Use this command to unselect all objects on a schematic.
                                                                                33

    You may also unselect all objects by selecting in an area of the schematic that
    has no objects.

    Practice using the select command and its options in the Demo schematic you
    have on the screen. Do not worry about any changes you may make. Make sure
    that when you exit Logic Creator you don't save any of the changes you have
    made.

How to Exit Logic Creator
    From the File Menu select Exit. A dialog box will pop up asking if you want to
    save the changes in the current design. Click on NO and you are back in the
    windows program manager.
34
                                                                                   35



Chapter 3
Logic Creator: Schematic Tutorial
Introduction
The next three chapters present tutorials for the Logic Creator schematic entry
program, Board Creator PC board layout program, and the Route Creator program.
These tutorials will give you actual hands-on experience using the Circuit Creator
system. The tutorials will lead you through the creation of a simple schematic and its
PC board layout.

Notation
       The following notation is used throughout the tutorials.




                Figure 3-1: Notation in Logic Creator Schematic

       The notation "XXX" indicates that the characters shown between the quotes are
       to be typed. For example, "XYZ" indicates that the characters X, Y, and Z are
       to be typed. Do not type the quotes.
36

     The notation, XXX, indicates this single key, key combination,
     menu/command, or dialog-box button should be pressed. For example,
     ENTER means press the enter key while G indicates the G key is to be
     pressed. FILE/OPEN means to select the OPEN command from the FILE
     menu. OK means to select the OK button in a dialog-box. Unless otherwise
     noted, either upper or lower case may be used.

     The notation, (xxx,yyy), indicates a coordinate. For example, (10.0,15.250)
     indicates the horizontal position is 10 inches and the vertical position is 15.250
     inches.

     The tutorial steps are listed in terms of the keyboard. If your system has a
     mouse, feel free to use it. The left button of the mouse is equivalent to the
     ENTER key, while the right button is equivalent to the ESC key.

     Initially, great detail is given. As we proceed through each of the tutorials, and
     you learn the basics; less detail will be given. If you will be using a plotter
     connected to a serial port.
     This tutorial leads you, step by step, through the creation of a simple
     schematic. If you have not yet installed the evaluation software, refer to
     Chapter 5 for instructions.

Starting Logic Creator
     To run the Logic Creator program, double click on the Circuit Creator program
     group (if it has been minimized) and then double click on the Logic Creator
     icon.


Loading a Schematic
     To get a feel for the system, we will first load a sample schematic file. We will
     then learn how to navigate about the schematic on the display.
                                                                             37




       Figure 3-2: Loading Schematic file in Logic Creator

First, an explanation of how to select commands from the pull-down menus
and dialog-boxes will be given.

If you are using the keyboard, a pull-down menu may be displayed (pulled-
down) by holding the ALT key down pressing the key indicated by the
underlined character in its name on the title-bar. Upper or lower case may be
used.

When a pull-down menu is displayed, the and arrow keys may be used to
move to the next menu to the right or left. The NUMLCK key must be off. Use
the and arrow keys to move the menu selector up and down. Move to the
FILE/OPEN command and select it by pressing the ENTER key.

If you are using a mouse, you may pull-down a menu by moving the pointer to
the menu name in the title-bar and pressing the left mouse button and releasing
it. The menu will appear when the button is released. To select a menu item,
move the pointer to the desired item and press the left mouse button and
release it. The selection is made when the button is released. For quicker menu
selections, move the pointer to the title and press the left mouse button and do
not release the button yet. Now, move the pointer to the desired menu item and
release the button to make the selection.
38

File Selection Dialog Box
     After selecting the FILE/OPEN command, a dialog-box will appear which is
     prompting for the name of a schematic file. At this point, we can type the file
     name of a schematic file, or select one from the list that is displayed. Use the
     arrow keys to move the selector to the file in the list named "DEMO.SCH" and
     press ENTER. This will copy the file name from the list into the file field of
     the dialog-box. Now press ENTER again to directly accept this name, or press
     the Home key to move the selector to the OK button, then press ENTER.

     When a dialog-box is displayed, clicking the left mouse button on the OK
     button, or pressing the ALT-O key combination will immediately accept the
     values in the dialog-box. Pressing the HOME key will move the selector to the
     OK button.

     Clicking on the Cancel button, or pressing the ALT-C combination will
     immediately cancel the dialog-box. Pressing the END key or the ESC key will
     move the selector to the cancel button. Once the selector is on the cancel
     button, pressing ESC again will cancel the dialog-box. Any changes made to
     the values shown in a dialog-box do not actually take effect until the OK
     button is pressed. If the CANCEL button is pressed, the changes made to
     values in the dialog-box are ignored.

     For a file-selection or part-selection dialog-box, pressing ENTER twice while
     on the same name in the list implies that this is the name you want to accept
     immediately.

Getting Help
     Press the F1 key to pop-up a window of help information. Notice that the help
     information is specific to the current command being performed. The UP and
     DOWN buttons may be used to page the help text up and down in the window.
     You may also use the NEXT, PREV, or GENERAL buttons to view other
     help topics.

     Now, select the EXIT button to close the help window. Help is always
     available with the F1 key.
                                                                                   39

Moving Around A Schematic
    We will now learn how to change the view of a schematic displayed on the
    screen. Pull-down the View menu. Now, move down and select the Zoom Out
    command. The display will be redrawn at a smaller scale. You will notice that
    the ZOOM OUT menu item has CTRL+PGDN listed in the right margin next
    to it. This indicates that this command has a hot key. This key combination
    may be used when the menu is not displayed to directly execute this command.
    Let's try it. Now, hold the Ctrl key down and press the PGDN key to zoom-in.
    Once you are more familiar with the program, using hot-keys will improve
    your productivity, especially if you do not have a mouse.

    Zoom back to the original scale by pressing the CTRL+PGUP key twice.

    The current coordinate of the cursor is displayed in inches in the upper-right
    corner of the screen. Use the cursor keys to move the cursor to coordinate
    (2.000,1.000). Follow the track of the cursor on the screen, and watch the value
    in the upper-right corner change. Notice that the active cursor (the little cross)
    is not always the same as the mouse pointer position.

    Holding the SHIFT key down and using the cursor keys will move the cursor
    one inch at a time. Hold the SHIFT key down and use the       and arrows to
    move quickly to coordinate (0.000,0.000), the upper-left corner of the sheet.

    The display may be panned using the keyboard by bumping into one of the edit
    window edges. Let's pan right. Move the cursor with the SHIFT     key until it
    bumps the right edge of the window. The portion of the schematic that was out
    of view to the right of the screen is now displayed.

    With a mouse, the view may be panned by using the vertical slide-bar at the
    right, or the horizontal slide bar at the bottom.
    Display the upper-left corner of the sheet at normal scale by pressing
    CTRL+HOME.

Reference Grid
    The lines, normally green, that you see on the screen represent a reference grid.
    This grid is used to assist the user in drawing a schematic and lining up
40

     objects. It is not part of the schematic itself, and is not printed on hard-copy
     output. From the VIEW menu, select the GRID command. This dialog-box is
     used to control the display of the reference grid, and the step size of the cursor
     movements. Select the check-box entry for DISPLAY so the X check mark is
     off. Now, select OK. Notice that the grid lines no longer appears in the display;
     however, the cursor-motion grid is still active.

     A single Logic Creator design file may have up to thirty-two sheets of
     drawings. This demo drawing has two active sheets. From the VIEW menu,
     select the SHEET command. Now, from the list, select sheet number two.
     Sheet two should now be shown on the display.

     This completes a summary of how to start LOGIC CREATOR, make menu
     selections, set the parameters in a dialog-box, load an existing schematic, view
     the schematic, and control the reference grid. Use the G hot key and turn the
     grid back on.

Creating A New Schematic




                  Figure 3-3: Schematic Format Dialog-Box

     Our assignment is to create the schematic drawing for a small board design
     entirely from scratch. Once created, it will be checked for errors, with
                                                                               41

assistance from the program, and various reports about the design will be
generated. This circuit is intentionally simple and small; however, it
demonstrates the basic steps by which any circuit, regardless of size, is created.
A rough, hand-drawn sketch of the circuit is given in the figure that follows.
This is the way actual schematics normally start out, although an experienced
designer may use Logic Creator to directly enter designs without the use of
sketches.




             Figure 3-4: Rough Sketch Of Schematic

From our rough sketch, we have all the information we need to begin entering
our schematic. From the FILE menu, select the NEW command. If you have
made any changes to the sample schematic we have been viewing, you will be
prompted whether or not you want to save these changes. If prompted, type N
for no.

We are presented with the FORMAT dialog-box. For the overall title, enter
"Tutorial Demo Lesson"; for the title of sheet number 1, enter "Detector
Circuit". The default settings for the remainder of the parameters will do.
Anyway, we can use the EDIT/FORMAT command later if we want to change
42

     any of these values. Select the OK button to accept the settings. We now have
     a blank sheet, sheet number one, to work on.

Placing The Parts
     We are now ready to place the parts of our circuit on this sheet. Pull-down the
     LIBRARY menu and select the IC's library entry. We will first place the four-
     input NAND gates on the sheet. From the list of parts that is displayed, locate
     and select the 7420 part name. The outline of this part is now attached to our
     cursor. Move the cursor to coordinate (2.0,1.5). ENTER to place the symbol
     at this point. This particular part has two gates in it. Notice that the pin
     numbers for the gate corresponding to the 1st section of this part have been
     placed. Also, the reference number has automatically been filled in as U1-A.




                  Figure 3-5: Parts Placed on Schematic

     Now, while we still have the symbol for this part on our cursor, let's add the
     other gate. Move the cursor to (2.0,2.8) and ENTER. Notice that this gate has
     pin numbers corresponding to the 2nd gate in the part, and the reference
     number is U1-B.
                                                                             43

Now we will add the flip-flops. From the library menu, select the IC's library.
This time, locate and select the 7474 part. Move to (4.4,1.4) and ENTER to
place the first flip-flop. This part has been labeled as U2-A. Now, move to
(4.4,3.3) and place the other half of the flip-flop. Isn't this much easier than
drawing the parts every time?

Now, we will add the 330 ohm resistors to the schematic. Select the
RESISTORS library from the library menu. Select the resistor part R330.
Place one resistor at coordinate (6.2,2.0) and a second one at (6.2,3.9). They
will be labeled as R1 and R2.

Now, we will add the light-emitting diodes to the schematic. In this case, we
will intentionally make a mistake, and recover from it. Select the part LED-
RED from the MISC library. Place the first LED at (7.4,2.0) and the second
one at (7.4,3.9). Press the ESC key to end the part placement command. Look
at the orientation of the LEDs on the screen. You will notice that the cathode
end of the LED is on the incorrect (right) side. This is not what we want! If we
had noticed this while the part was on the cursor, we could have used the F9 or
F10 keys to set the desired mirroring and orientation of the symbol. Since our
diodes are already placed, we will update them with new values.

Move the cursor to any point within the area of one of the diodes and press
ENTER twice. This will select the diode, which is now displayed in the select
color (usually red). Once selected, an item may be moved, deleted, or its
parameter settings changed. Press U to select the UPDATE command. This
command may also be selected by pressing the ENTER key again, without
moving the cursor.

Change the value for MIRROR from NONE to RIGHT-LEFT. This is done
by moving the selector to this field and pressing ENTER. Select the right-to-
left from the pop-up menu and select the OK button. Notice that the diode pin
numbers and symbol shape have flipped ends. This method may also be used
to change the rotation of the part symbol, change the reference value, and to
select alternate part symbols.
44

     Now, using the technique just learned, change the mirror parameter for the
     other diode so that it looks like this one.

     Next, we will complete the placement of our part symbols by adding the
     connector. From the library menu, use the MISC library to select the CONN-
     12 connector part. Place the connector at location (0.4,1.8).

Wiring The Circuit
     Since all of our parts are placed, we are now ready to wire them together. First,
     let's wire the connection from U1 pin 6 to U2 pin 3. From the DRAW menu,
     select the WIRE command, or just type W. Move the cursor to (3.4,2.1).
     ENTER to begin the wire line. Move to (4.4,2.1) and ENTER to draw a
     segment of the wire. Press ESC to stop drawing this net's wires.

     Now, let's make a similar connection from U1 pin 8 to U2 pin 11. Move to
     (3.4,3.4) and ENTER to start the net line. Move to (3.5,3.4), ENTER; to
     (3.5,4.0), ENTER; to (4.4,4.0), ENTER, and ESC.

     Got the hang of it? In actual practice, the wiring process is even easier because
     you are drawing the lines by looking at the points that need connecting on the
     screen instead of working from a list of points as we are doing here. If you add
     a wire in the wrong place, simply press the F2 key to undo it, and then draw
     the right wire.

     Now, connect the following points with wires. Remember to use ESC to stop
     drawing one net before starting the next net wire.

            U2-6, R1-1     (6.0,2.3) to (6.2,2.3).
            D1-2, R1-2     (7.2,2.3) to (7.4,2.3).
            U2-8, R2-1     (6.0,4.2) to (6.2,4.2).
            D2-2, R2-2     (7.2,4.2) to (7.4,4.2).
            D1-1, D2-1     (8.4,2.3) to (8.6,2.3) to (8.6,4.2) to (8.3,4.2).

     Now, move the cursor to (8.6,4.2). At this point, we want to add a connect dot
     and continue the net. ENTER to start the line. Now, without moving the
     cursor, ENTER again. This will add a connect dot. From this point, move to
                                                                                 45

    (8.5,5.1) and ENTER. Continue this net line to (3.8,5.1), ENTER; then to
    (3.8,3.8), ENTER, and into U2 pin 12 at (4.4,3.8). Now ESC and move back
    to (3.8,3.8). Add a connect dot here, and continue the net to (3.8,1.9) and end
    at U2 pin 2 (4.4,1.9). Move to (3.8,5.1) and add a connect dot. Continue the net
    to (1.6,5.1), to (1.6,4.1), and into pin 10 of the connector at (1.0,4.1).

    By referring to the rough sketch of our circuit, see if you can complete the
    wiring of this circuit.

Adding Net Names
    Now, we will add the net names for the nets, which have names. Select the
    NET NAME command from the DRAW menu. Move to location (2.1,5.1) and
    ENTER. In the dialog-box, set the net name to "+5V" and the location to
    ABOVE. Select OK to complete the adding of the net name.

    Pin 12 of the connector is the ground net. We will show this by using the
    ground symbol. First, use the DRAW/WIRE command to extend the net line
    from connector pin 12 to (1.2,4.5) and down to (1.2,5.0). Now, select the
    DRAW/NET NAME command again. Move to location (1.2,5.0) and ENTER.
    This time, select the button in the dialog-box labeled GND. Internally, and on
    reports, the name of this net will be referred to as GND; however, on the
    schematic, the graphic symbol for standard ground is shown. This same
    technique may be used to show analog-ground and chassis-ground. Select OK
    to complete the command.

Unused Pins
    The unused pins of all components on the schematic should be labeled with a
    net name of "NC" (no connect). Move to location (1.0,4.3) and add a net name
    of "NC" with a position value of RIGHT. Notice how the arrow, for a RIGHT
    type net name label is automatically displayed for you.

    Add "NC" net names for the following locations:

           U2-4 (Top)
           U2-5 (Right)
           U2-10 (Top)
46

            U2-9 (Right)

Text/Lines
     Now, we will complete our schematic by adding some notational text. Select
     the DRAW/TEXT command. Move to (4.4,0.6) and ENTER. Set the text
     string to "Notes:" and select OK. In the same manner, move to location
     (4.4,0.8) and ENTER "1. Layout on a 4 x 4 inch board.", and at (4.4,1.0)
     ENTER "2. Power and ground planes required.". Now, move to (0.7,0.8) and
     ENTER. Enter "Detector Circuit" for the text, but this time select BOLD and
     set the text size to 0.188.

     Now, select the DRAW/LINE command and, just like the wires were drawn,
     draw a box around the text that was just added.

     Please note the difference between wires and lines. Wires are used to
     electrically connect components together, lines are for graphic effect only.

Saving The Schematic
     This completes the tutorial schematic. Let's save it to disk. Select the
     FILE/SAVE AS command. Enter "mydesign" for the name and select OK. The
     evaluation version of the program will not actually save the drawing.
                                                                           47




                    Figure 3-6: Saving Schematic file

Checking The Design
    To check our layout work, select the Design Check command from the
    REPORTS menu. If you have followed all the instructions carefully, you
    should get a report of "No errors detected." Otherwise, the errors will be
    pointed out to you on the screen.
48

     If no errors were detected, just to show you how the error reporting works,
     move to location (6.1,1.9) and select the "NC" net name label. Press the Del
     key to delete the label. Run the check again. This time an error should be
     detected at this location. You can use the F2 key, UNDO, to repair your
     schematic.

     If errors were detected, see if you can correct them, then run the check again.

Generating Reports
     Now that we have checked the design for errors, let's generate the formal
     reports for this design. From the REPORTS menu, select the FORMAL
     command. Check the Pin-List, Net-List, and Bill of Material reports. Select
     OK to start making the reports. The reports are written to files on the disk. The
     pin list report will be in "Mydesign.pin", the net list will be in "Mydesign.net",
     and the bill of materials will be in "Mydesign.bom". The files are in ASCII
     format, and may be printed on your.

Exiting The Program
     We are finished with this schematic for now. Select EXIT command on the
     FILE menu or just type Alt + X to exit the program.

Summary Of Schematic Entry
     Let us emphasize that the entry of the tutorial schematic may seem a little
     tedious. This is because we have stepped you through each of the steps at a
     very detailed level. In actual practice, you are choosing your own locations for
     parts, paths for the nets, and the order in which you wish to layout the circuit.
     You will have a much greater sense of freedom. Just follow the principles you
     have learned here and it will flow very smoothly. At this point, you may want
     to re-start the program and "just play around" for a while.
     Our assignment is to create the schematic drawing for a small board design
     entirely from scratch. Once created, we will ask Logic Creator to check our
     schematic for wiring errors. If there are any Logic Creator will pin point them
     to us so that we can fix them. We will also produce a bill of material report,
     which will list all the parts used in our design and their cost. As you will find
     out the cost of the components more likely will be incorrect because it changes
     daily. Other reports like the printed circuit board update file, and a net list file
                                                                         49

will be generated and printed. Then we will analyze these files and explain
how they are used.

This circuit is intentionally simple and small; however, it demonstrates the
basic steps by which any circuit, regardless of size, is created. A rough,
hand-drawn sketch of the circuit is given in the figure 3-6. This is the way
actual schematics normally start out, although an experienced designer may
use Logic Creator to directly enter designs without the use of sketches.

From our rough sketch, we have all the information we need to begin entering
our schematic.




              Figure 3-6: Sketch of Detector Circuit.

1.   Launch Logic Creator from the Circuit Creator program group.
2.   Click in the File menu.
3.   Select New, and the dialog box of figure 3-2 pops up.
4.   Click the title box and enter " Tutorial Demo Chapter". This is the
     title of this project.
50

     5. Complete the sheet number 1 title as "Detector Circuit". Type your
        name in the "Drawn by:" box.
     6. Do not change anything else.
     7. If you have any questions about an item in the dialog box, ask for help
        using F1 or clicking the Help button
     8. When finished click OK




                     Figure 3-7: The Format Dialog Box

     The default size of the sheet is B: 17"x11". Two A size sheets 8.5"x11" put
     side by side along the long side make up a B size sheet. Two B size sheets
     placed next to each other along their long side make up a C size sheet with
     dimensions of 34"x17". Similarly you can find out the dimensions of the D and
     E size sheets. Do not change the sheet size setting. When it's time to print the
     print menu automatically resizes the sheet to print on the size paper your
     printer can handle, usually size A. Do not change the symbol used for the sheet
     either, leave it as is (fmt_b.sym).

     1. Pull-down the Library menu.
                                                                                  51

    2. Select the 7400 library. If a library mentioned in this tutorial does not
       appear on the menu, then use the Library/Add Part command to
       directly select the library.
    3. From the list of the displayed parts select the 7420 part.
    4. The outline of the part is displayed and is attached to the cursor.
    5. Move the cursor using the mouse and/or keyboard to the coordinate
       (2.0,1.5). For fine control use the keyboard's arrow keys.
    6. Click the left mouse key or press ENTER to place the symbol of the
       7420 part at this point.

Placing Parts on the work sheet
    We are now ready to place the parts of our circuit on this sheet.

    This particular part has two gates in it. These two gates are called sections in
    Logic Creator. The 7420 integrated circuit package is one electronic part with
    two identical sections, four input NAND gates. What you have just placed on
    the schematic is the symbol for one of the two gates inside the 7420 part.
    Notice that the pin numbers for the gate corresponding to the 1st section of this
    part have been placed. Also, the reference designator number has automatically
    been filled in as U1-A. All electronic components have unique reference
    designators. The reference designator for resistors is R, for capacitors C, for
    diodes D, for transistors Q, and for integrated circuits U. Please search the
    program's help file for ANSI Standard, it lists all the electronic and electrical
    device reference designators in accordance with the standards of the American
    National Standards Institute (ANSI). Please refer to it when you are creating a
    new part that needs a new reference designator.

    Now, while we still have the symbol for this part on our cursor, let's add the
    other gate.

    1. Move the cursor to (2.0,2.8) and press ENTER to place it.
    2. Press ESC or click the right mouse button to stop the place command.
52

     Notice that LOGIC CREATOR numbered the pins of this gate according to the
     standard numbering of the second gate of the 7420 part, and the reference
     number is U1-B. Look up the pin numbering of the 7420 in a data book.

     Now we will add the flip-flops.

     1. From the library menu, select the 7400 library.
     2. Locate and select the 7474 part.
     3. Move to coordinate (4.4,1.4) and press ENTER to place the first flip-
        flop.
     4. Move to (4.4,3.3) and place the other second flip flop which is the
        second section of the 7474 part.

     Isn't this much easier than drawing the parts by hand, one at a time, every
     time?

     Now, we will add the 330 Ohm resistors to the schematic.

     Notice that they are automatically labeled as R1 and R2. Notice also that the
     resistors have numbers on their leads like IC's on their pins. These numbers
     identify the two leads of the resistors. Later Logic Creator will use this
     information to create a list or database of all the leads of all the components
     and how they are interconnected. This list is called net list. We will talk about
     this later in greater detail.

     Now, we will add the light-emitting diodes to the schematic. In this case, we
     will intentionally make a mistake, and recover from it.

     1.   Click on LIBRARY, and select the MISC library.
     2.   Find the LED-RED and select it.
     3.   Place the first led at (7.4,2.0) and the second at (7.4,3.9).
     4.   Press the ESC key to end the command.
                                                                         53

Look at the orientation of the LEDs on the screen. You will notice that the
cathode end of the LED is on the incorrect (right) side. This is not what we
want! If we had noticed this while the part was on the cursor, we could have
used the F9 or F10 keys to set the desired mirroring and orientation of the
symbol. Since our diodes are already placed, we will update them with new
values.

1. Move the cursor to any point within the area of the diode we want to
   mirror and double click the left mouse button. The UPDATE dialog
   box shown figure 3-4 pops up.
2. Click on the MIRROR box and change its contents from NONE to
   RIGHT-LEFT.
3. Click OK, and the symbol will be mirrored about its Y-axis.

Notice that the diode symbol has been mirrored about the part's Y (vertical)
axis, and what was right now is left, and what was left now is right. Now,
using the technique just learned, change the mirror parameter for the other
diode so that it looks like this one.




              Figure 3-8: The UPDATE Dialog Box
54


     Now you should have in front of you a sheet with all the components but no
     interconnecting wires, see figure 3-9.

     We will now complete the placement of our part symbols by adding the
     connector.

     1.   Click on the LIBRARY menu.
     2.   Click on the MISC library.
     3.   Select the CONN-12 part.
     4.   Place it at location (0.4,1.8) by pressing ENTER
     5.   Click the right mouse button or the ESC key to end the command.




               Figure 3-9: Part Placement of Detector Circuit
                                                                                  55

Wiring the parts together
    Since all of our parts are placed, we are now ready to wire them together. First,
    let's wire the connection from U1 pin 6 to U2 pin 3. One important point falls
    here. Make sure your wires do not overlap the component leads because Logic
    Creator does not consider this a connection. It is considered an error. You will
    not be notified of this error until later when we will perform a CHECK of the
    schematic. When you are not sure if your wires and component leads touch or
    overlap, simply ZOOM-IN the area where you are making the connection, or
    inspecting a connection. Since components and wires are drawn with different
    colors it will be easy to spot any overlapping.

    1. Click on the DRAW menu.
    2. Select the WIRE command, or just type W, the commands hot key.
    3. Move the cursor to (3.4,2.1), and click the left mouse button to begin
       the wire line.
    4. Move to (4.4,2.1) and click to draw a segment of wire.
    5. Click the right mouse button to stop the command.

    Now, let's make a similar connection from U1 pin 8 to U2 pin 11. Move to
    (3.4,3.4) and ENTER to start the net line. Move to (3.5, 3.4) ENTER to (3.5,
    4.0) ENTER to (4.4, 4.0) ENTER. and ESC.

    Got the hang of it? In actual practice, the wiring process is even easier because
    you are drawing the lines by looking at the points that need connecting on the
    screen instead of working from a list of points as we are doing here. If you add
    a wire in the wrong place, simply press the F2 key to undo it, and then draw
    the correct wire.

    Now, connect the following points with wires. Remember to use ESC to stop
    drawing one net before starting the next net wire.

           U2-6, R1-1     (6.0, 2.3) to (6.2, 2.3).
           D1-2, R1-2     (7.2, 2.3) to (7.4, 2.3).
           U2-8, R2-1     (6.0, 4.2) to (6.2, 4.2).
56

            D2-2, R2-2     (7.2, 4.2) to (7.4, 4.2).
            D1-2, D2-1     (8.4, 2.3) to (8.6, 2.3) to (8.6, 4.2) to (8.3, 4.2).

     Now, move the cursor to (8.6, 4.2). At this point, we want to add a connect
     dot and continue the net. ENTER to start the line. Now, without moving the
     cursor, ENTER again. This will add a connect dot. From this point, move to
     (8.5, 5.1) and ENTER. Continue this net line to (3.8, 5.1), ENTER; then to
     (3.8, 3.8), ENTER, and into U2 pin 12 at (4.4, 3.8) Now ESC and move back
     to (3.8, 3.8). Add a connect dot here, and continue the net to (3.8, 1.9) and
     end at U2 pin 2 (4.4, 1.9). Move to (3.8, 5.1) and add a connect dot. Continue
     the net to (1.6, 5.1), to (1.6, 4.1), and into pin 10 of the connector at (1.0,
     4.1).

     By referring to the rough sketch of our circuit, see if you can complete the
     wiring of this circuit.

Placing Net Names on the schematic
     Nets allow us to electrically connect several points together without showing
     the wires on the screen. This helps minimizing the clatter on the screen and the
     schematic. It would make sense to assign nets to all ground and power pins of
     integrated circuits for example. Other examples of common use of net names
     are for the clock signal in digital circuits, or the bus lines of a computer
     system, which connect to multiple integrated circuits. Let's add net names to
     our schematic.
                                                                           57




             Figure 3-10: The NETNAME Dialog Box

Select the NET NAME command from the DRAW menu. Move to location
(2.1,5.1) and Enter. In the dialog-box, set the net name to "+5V" and the
location to ABOVE. Select OK to complete the adding of the net name. Pin 11
of the connector is the ground net. We will show this by using the ground
symbol. First, use the DRAW/WIRE command to extend the net line from
connector pin 11 to (1.2,4.5) and down to (1.2,5.0). Now, select the
DRAW/NET NAME command again. Move to location (1.2,5.0) and
ENTER. This time, select the button in the dialog-box labeled GND.
Internally, and on reports, the name of this net will be referred to as "GND";
however, on the schematic, the graphic symbol for earth ground is shown.
Select OK to complete the command.

Unused Pins
The unused pins of all components on the schematic should be labeled with a
net name of NC (Not connected). Remember that the schematic diagram will
be the source of information from which Board Creator will operate on. Every
pin of the schematic has to be identified and connect to a net. Fortunately
Logic Creator has the feature that allows us to automatically check for any
mistakes. We will perform those checks after we finish creating the schematic.
58

     Move to location (1.0,4.3) and add a net name of "NC" with a position value of
     RIGHT. Notice how the arrow, for a right type net name label is automatically
     display for you.

     Add "NC" net names for the following locations:
           U2-4 (top)
           U2-5 (right)
           U2-10 (top)
           U2-8 (right)

Text/Lines
     Now, we will complete our schematic by adding some notational text. Select
     the DRAW/TEXT command. Move to (4.4,0.6) and ENTER. Set the text
     string to "Notes:" and select OK. In the same manner, move to location
     (4.4,0.8) and enter "1. Layout on a 4 x 4 inch board.", and at (4.4,1.0) enter
     "2. Power and ground planes required.". Now, move to (0.7,0.8) and ENTER.
     Enter "Detector Circuit" for the text, but this time select BOLD and set the text
     size to 0.188.

     Now, select the DRAW/LINE command and, just like the wires were drawn,
     draw a box around the text that was just added.
     Please note the difference between wires and lines. Wires are used to
     electrically connect components together; lines are for graphic effect only.

Symmetry and Balance of a Schematic
     Now that you finished your schematic zoom out and take a look at it from a
     distance. How does it look? Is it centered around the sheet, is it symmetrical or
     balanced? If you followed the instructions given your schematic should be
     located on the top left corner of the sheet. It is obviously not symmetrically
     placed on the sheet. There is nothing to worry about, because the SELECT
     command will allow us to select and move the entire schematic. Here is how
     you do it
                                                                          59




The above figures show the ZOOM OUT schematic before and after the move

  1. Press the right mouse button or the ESC key as many times needed to
     cancel the current command.
  2. You are now in the Select command, which is the default command in
     Logic Creator.
  3. Move the cursor somewhere on the sheet that there are no parts and
     click the left mouse button.
  4. The bottom line of the screen, the status window displays:
  5. ENTER: Start Select Touching Area, ESC: Cancel, O: Options Click
     on the status window or press O and the Select Object dialog box pops
     up.
  6. From the Area section select Bound By, from the Mode section select
     Flat, and from the Object section click the ALL button.
  7. Click OK to save the settings and close the dialog box.
  8. Being ZOOM OUT so that you can see the entire sheet, move the
     cursor to above the top left corner of the schematic.
  9. Press the left mouse button, and while holding it pressed drag the
     mouse towards the bottom right corner of the schematic. A rectangle is
     drawn on the screen showing the selected area. Make sure the entire
     schematic is included in the rectangle. All the selected items appear in
     red now.
60

     10. Move the cursor inside the rectangle. Its background now changes to a
         different color. Place your cursor approximately in the middle of the
         highlighted area.
     11. Press and hold down the left mouse button. Now your cursor is
         anchored to the middle of the selected area. Then drag the cursor to
         the center of the sheet and release the left mouse button.
     12. The entire schematic will be redrawn for you in a matter of seconds.
         Try doing this by hand, using pens, triangles and drafting boards!


Checking our schematic for errors
     To check our work, select the Design Check command from the REPORTS
     menu. If you have followed all the instructions carefully, you should get a
     report of "No errors detected". Otherwise, the errors will be pointed out to you
     on the screen.

     If no errors were detected, just to show you how the error reporting works,
     move to location (6.1,1.9) and select the "NC" net name label (point to it and
     click the left mouse button, or press ENTER twice). Press the DEL key to
     delete the label. Run the check again. This time an error will be detected at this
     location. You can use the F2 key, UNDO, to repair your schematic.

     If errors were detected, see if you can correct them, then run the check again
     until there are no errors.

Formal/Export
     This command is used to create different reports like the Bill of Material
     (BOM), Net List (NET), Update List (UPD) and Pin List (PIN). Choose
     FORMAL/EXPORT command from the REPORTS menu. Select all of the
     options from Formal/Export Reports dialog box and choose OK. All the
     reports will be created in the same directory where your schematic was loaded.
     The file named mydesign.bom can be viewed by Notepad or WordPad and also
     can be printed using the same software.
                                                                              61

Saving your schematic
   This completes the tutorial. Let's save it to disk. Select the FILE/SAVE AS
   command. Enter "mydesign" for the name and select OK. This will save the
   drawing into file "mydesign.sch". If you would like to save your design on a
   diskette, click on the drives box and then select your disk drive (more likely
   A), and then click OK.
62
                                                                                  63



Chapter 4
Printing the Schematic and it Reports
   From the File menu select Print, and the following dialog box will appear. The
   sheet you were last in is highlighted. You can print this one or any one of the
   eight sheets. The sheet will be automatically scaled down to A size:8.5"x11",
   to fit the current printer size. You can click in the "Pause each page" box if you
   feed your printer a page at a time. Select the sheet you want to print and then
   press OK. Your schematic will start printing and Logic Creator will pop-up a
   dialog box informing you of what is happening and at the same time allowing
   you to cancel printing if you have to.




                     Figure 4.1: The Print Dialog Box
64

     The "Output to file" box allows you to save your schematic as a binary file on
     a diskette. This feature is very handy especially when your system has a poor
     old dot-matrix printer connected to it and you would like to print on a laser
     printer which is connected on an other computer which does not have LOGIC
     CREATOR on its hard drive. What you need to do is the following:

     1.   Set your computer up with the laser printers driver first.
     2.   Invoke the Print dialog box like in figure 4-1
     3.   Click the "Output to file" box
     4.   Save your file on a floppy disk
     5.   Go to the computer with the laser printer and print the file.

     When a schematic is printed in a file, the extension "PRN" is automatically
     attached to it. So the file you are looking for has the same name as your
     schematic but with the extension "PRN".

Generating Manufacturing Reports
     Now that we have checked the design for errors, let's generate the formal
     reports for this design. From the REPORTS menu, select the FORMAL
     command. Check the PC Board Update List, Bill Of Material, Net-List, and
     Pin-List reports. Select OK to start making the reports. The reports are written
     to files on the disk. The pin list report will be in "mydesign.pin", the net list
     will be in "mydesign.net", the bill of materials will be in "mydesign.bom", and
     the pcb update list will be in "mydesign.upd". All of these files will are saved
     in the CKTCRT directory unless you have changed the path. These files are in
     ASCII format, and may be printed on your printer with the standard DOS print
     command. They can also be printed from windows as explained below.

Printing the Reports
     The default file extension of Notepad is "txt". To select and view the net list
     for example, click in the "File name" box and change the file extension to "net"
     to enable us to access the net list, "mydesign.net". Now click on the open
     folder next to "C:\" to select the subdirectory where the net list is. Double click
                                                                                 65

on the subdirectory "CKTCRT". The mydesign.net file should appear in the
file box. Double click on it to open it.
The file should look similar to the one below. Glance through it for now and
notice its headings, subheadings and the information it contains. At the end of
the net list you will find a detail analysis of the net list.

                               Your name here
       -- Net List Report ----------------------------- Page: 1 --

       File: C:\Cktcrt\mydesign.sch
       Title:
       Program: Logic Creator
       Date: 5/31/2000 10:22

       * = Pin for pseudo-part

       Net-Name          Reference-Pin Pin-Type              Location(F-S,X,Y)
       ----------------------------------------------------------------
       +5V
                W1-10                      Inout
       (MYDESIGN.SCH-1,1100,5900)
                D2-1                       InOut
       (MYDESIGN.SCH-1,9600,5600)
                D1-1                       InOut
       (MYDESIGN.SCH-1,9600,3700)
                U2-2                       In
       (MYDESIGN.SCH-1,4800,3300)
                U2-12                      In
       (MYDESIGN.SCH-1,4800,5200)
                U2-14                      Power             (Assigned)
                U1-14                      Power             (Assigned)

LC#1
            D1-2              InOut
       (MYDESIGN.SCH-1,8600,3700)
66

                  R2-2              InOut
             (MYDESIGN.SCH-1,8000,3700)

     LC#10
                  W1-5              InOut
             (MYDESIGN.SCH-1,1100,4900)
                  U1-9              In
             (MYDESIGN.SCH-1,1800,4900)

     LC#11
                  W1-1              InOut
             (MYDESIGN.SCH-1,1100,4100)
                  U1-1              In
             (MYDESIGN.SCH-1,1800,3200)

     LC#12
                  W1-4              InOut
             (MYDESIGN.SCH-1,1100,4700)
                  U1-5              In
             (MYDESIGN.SCH-1,1800,3800)

     LC#13
                  W1-3              InOut
             (MYDESIGN.SCH-1,1100,4500)
                  U1-4              In
             (MYDESIGN.SCH-1,1800,3600)
     LC#14
                  W1-2              InOut
             (MYDESIGN.SCH-1,1100,4300)
                  U1-2              In
             (MYDESIGN.SCH-1,1800,3400)

     LC#2
                  R2-1              InOut
             (MYDESIGN.SCH-1,7000,3700)
                                                                                       67

             U2-6              Out
        (MYDESIGN.SCH-1,6400,3700)

LC#3
             U2-3              In
        (MYDESIGN.SCH-1,4800,3500)
             U1-6              Out
        (MYDESIGN.SCH-1,3200,3500)

LC#4
             U2-11             In
        (MYDESIGN.SCH-1,4800,5400)
             U1-8              Out
        (MYDESIGN.SCH-1,3200,5200)


                        Your name here
-- Net List Report ----------------------------------- Page: 2 --

        Net-Name          Reference-Pin Pin-Type              Location(F-S,X,Y)
        ----------------------------------------------------------------------------
LC#5
             R1-1              InOut
        (MYDESIGN.SCH-1,7000,5600)
             U2-8              Out
        (MYDESIGN.SCH-1,6400,5600)

LC#6
             D2-2              InOut
        (MYDESIGN.SCH-1,8600,5600)
             R1-2              InOut
        (MYDESIGN.SCH-1,8000,5600)

LC#7
             W1-8              InOut
        (MYDESIGN.SCH-1,1100,5500)
68

                 U1-13             In
            (MYDESIGN.SCH-1,1800,5500)

     LC#8
                 W1-7              InOut
            (MYDESIGN.SCH-1,1100,5300)
                 U1-12             In
            (MYDESIGN.SCH-1,1800,5300)

     LC#9
                 W1-6              InOut
            (MYDESIGN.SCH-1,1100,5100)
                 U1-10             In
            (MYDESIGN.SCH-1,1800,5100)

     GND
                 W1-12             InOut
            (MYDESIGN.SCH-1,1100,6300)
                 U2-7              Power   (Assigned)
                 U1-7              Power   (Assigned)

     RESET
                 W1-9              InOut
            (MYDESIGN.SCH-1,1100,5700)
                 U2-1              In
            (MYDESIGN.SCH-1,5600,4200)
                 U2-13             In
            (MYDESIGN.SCH-1,5600,6100)

            Total nets: 17
            Total errors/warnings: 0
            End of Report
                                                                                  69

Interpreting the Netlist Report
    Let's define what a net and netlist is before we continue. A net is a point in a
    circuit where more than two leads or pins of components connect together. A
    netlist of a circuit is a list of all the component interconnections. This
    interconnectivity list is what Board Creator will need later on to create copper
    traces that will connect the parts together on a printed circuit board. Netlists
    are also the primary source of information for circuit simulators.

    Logic Creator uses the net names the user had assigned, for example +5V,
    GND and RESET were the three nets we assigned in the mydesign.sch. The
    remaining nets are labeled with the prefix LC# and a number after it. For
    example the first net Logic Creator assigns will be LC#1, the second LC#2.
    The program then continues assigning nets in ascending order until all the nets
    of the circuit are named. See figure -4 with all nets marked on it.

    Now looking back at the netlist report carefully we see that Logic Creator has
    used the net names +5V, GND, and RESET, that we assigned on the
    schematic. For the remaining nets automatically assigned net names beginning
    with LC#1, LC#2, and so forth. This report consist of four columns, the net
    name, the reference pin, pin type, and location.

    The reference pin column lists all the pins of the components that connect to
    this net. Look at LC#1. The lead no.2 of diode D1 (D1-2), and the lead no.2 of
    resistor R1 (R1-2) connect together at this net. Go ahead and verify the
    reference pins listed under the LC#2 net. The second column is the part
    reference number and the pin of the part connecting to this net. The third
    column is the type of the pin. In other words, if the pin is an input, output, or
    power pin. This information is extracted from the symbol definition of the part.
    The pin type is also examined during the Design Check, and warnings or errors
    may be generated. The purpose of a warning is to make you go back to the
    schematic and double check because something may be wrong. A common
    warning is generated when an output of an integrated circuit is directly
    connected to power. For example the output of an AND gate connected
    directly to +5V or GND. The warning message is "Net has both output and
    power type pins". Logic Creator warns you about the error. It will not explain
    to you why this connection will cause a problem in the operation of the circuit.
70

     What you need to do is to make sure you did not enter the schematic wrongly
     by checking carefully the engineer's sketch. If the mistake was on the sketch
     then consult with the designer and resolve it.

     Now let's take a look at the pin list. Again browse through it noticing the
     different headings and subheadings. At the end of it you will find a detailed
     analysis of what this list is about.

                                    Your name here
            -- Pin List Report -------------------- Page: 1 --

            File: c:\CKTCRT\mydesign.sch
            Title:
            Program: LOGIC CREATOR
            Date: 5/31/2000 10:22

            Reference: D1, Part: LED-RED
            Light Emitting Diode, Red
            Pin Net           Type              Location(F-S,X,Y)
            ---------------------------------------
            1: +5V            InOut             (MYDESIGN.SCH-1,9600,3700)
            2: LC#1           InOut             (MYDESIGN.SCH-1,8600,3700)

            Reference: D2, Part: LED-RED
            Light Emitting Diode, Red
            Pin Net           Type              Location(F-S,X,Y)
            -------------------------------------------------------
            1: +5V            InOut             (MYDESIGN.SCH-1,9600,5600)
            2: LC#6           InOut             (MYDESIGN.SCH-1,8600,5600)

            Reference: R1, Part: R330
            330 Ohm Resistor
            Pin Net          Type              Location(F-S,X,Y)
            ----------------------------------------------------
            1: LC#5          InOut              (MYDESIGN.SCH-1,7000,5600)
            2: LC#6          InOut              (MYDESIGN.SCH-1,8000,5600)
                                                                 71

Reference: R2, Part: R330
330 Ohm Resistor
Pin Net           Type              Location(F-S,X,Y)
------------------------------------------------------
1: LC#2           Inout             (MYDESIGN.SCH-1,7000,3700)
2: LC#1           InOut             (MYDESIGN.SCH-1,8000,3700)

Reference: U1, Part: 7420
Dual 4-Input Nand Gates
Pin Net           Type              Location(F-S,X,Y)
-------------------------------------------------------
1: LC#11          In                (MYDESIGN.SCH-1,1800,3200)
2: LC#14          In                (MYDESIGN.SCH-1,1800,3400)
3: --unused--
4: LC#13          In                (MYDESIGN.SCH-1,1800,3600)
5: LC#12          In                (MYDESIGN.SCH-1,1800,3800)
6: LC#3           Out               (MYDESIGN.SCH-1,3200,3500)
7: GND            Power             (Assigned)
8: LC#4           Out               (MYDESIGN.SCH-1,3200,5200)
9: LC#10          In                (MYDESIGN.SCH-1,1800,4900)
10: LC#9          In                (MYDESIGN.SCH-1,1800,5100)
11: --unused--
12: LC#8          In                (MYDESIGN.SCH-1,1800,5300)
13: LC#7          In                (MYDESIGN.SCH-1,1800,5500)
14: +5V           Power             (Assigned)


                       Your name here
-- Pin List Report -------------------- Page: 2 --

Reference: U2, Part: 7474
Dual D-Type Flip-Flop
Pin Net           Type              Location(F-S,X,Y)
----------------------------------------------
1: RESET          In                (MYDESIGN.SCH-1,5600,4200)
2: +5V            In                (MYDESIGN.SCH-1,4800,3300)
72

     3: LC#3       In             (MYDESIGN.SCH-1,4800,3500)
     4: NC         In             (MYDESIGN.SCH-1,5600,2800)
     5: NC         Out            (MYDESIGN.SCH-1,6400,3300)
     6: LC#2       Out            (MYDESIGN.SCH-1,6400,3700)
     7: GND        Power          (Assigned)
     8: LC#5       Out            (MYDESIGN.SCH-1,6400,5600)
     9: NC         Out            (MYDESIGN.SCH-1,6400,5200)
     10: NC        In             (MYDESIGN.SCH-1,5600,4700)
     11: LC#4      In             (MYDESIGN.SCH-1,4800,5400)
     12: +5V       In             (MYDESIGN.SCH-1,4800,5200)
     13: RESET     In             (MYDESIGN.SCH-1,5600,6100)
     14: +5V       Power          (Assigned)

     Reference: W1, Part: CONN-12
     12 Pin Connector
     Pin Net           Type               Location(F-S,X,Y)
     --------------------------------------------------
     1: LC#11          InOut             (MYDESIGN.SCH-1,1100,4100)
     2: LC#14          InOut             (MYDESIGN.SCH-1,1100,4300)
     3: LC#13          InOut             (MYDESIGN.SCH-1,1100,4500)
     4: LC#12          InOut             (MYDESIGN.SCH-1,1100,4700)
     5: LC#10          InOut             (MYDESIGN.SCH-1,1100,4900)
     6: LC#9           InOut             (MYDESIGN.SCH-1,1100,5100)
     7: LC#8           InOut             (MYDESIGN.SCH-1,1100,5300)
     8: LC#7           InOut             (MYDESIGN.SCH-1,1100,5500)
     9: RESET          InOut             (MYDESIGN.SCH-1,1100,5700)
     10: +5V           InOut             (MYDESIGN.SCH-1,1100,5900)
     11: NC            InOut             (MYDESIGN.SCH-1,1100,6100)
     12: GND           InOut             (MYDESIGN.SCH-1,1100,6300)

     Total real parts: 7
     Unused real pins: 2
     Total real pins: 48
     End of Report
                                                                                   73

Interpreting the Pinlist Report
    The pin list contains in essence the same information as the netlist but arranged
    differently.

    It lists the components in sub headings. Each sub heading has the part
    reference designator, in the schematic, the part name, and the part description.
    this information is extracted from the part definition table (More on this in the
    next Chapter). Under each subheading there are four columns: Pin, Net, Type,
    and Location. The first column is a pin of this part and the remaining columns
    are its characteristics. Study the "mydesign.pin" file carefully.

    The following report is the update list of mydesign.sch. Browse through it and
    take notice of the different headings and its contents. At the end of the list you
    will find again a detailed analysis of this report.

           Board Creator update list
           UPDATE_LIST
           PART CONN-12 W1 CONN12
           PAD W1 1 LC#11
           PAD W1 2 LC#14
           PAD W1 3 LC#13
           PAD W1 4 LC#12
           PAD W1 5 LC#10
           PAD W1 6 LC#9
           PAD W1 7 LC#8
           PAD W1 8 LC#7
           PAD W1 9 RESET
           PAD W1 10 +5V
           PAD W1 11 NC
           PAD W1 12 GND
           PART LED-RED D2 DISC-2
           PAD D2 1 +5V
           PAD D2 2 LC#6
           PART LED-RED D1 DISC-2
           PAD D1 1 +5V
           PAD D1 2 LC#1
74

     PART R330 R2 DISC-2
     PAD R2 1 LC#2
     PAD R2 2 LC#1
     PART R330 R1 DISC-2
     PAD R1 1 LC#5
     PAD R1 2 LC#6
     PART 7474 U2 DIP-14
     PAD U2 1 RESET
     PAD U2 2 +5V
     PAD U2 3 LC#3
     PAD U2 4 NC
     PAD U2 5 NC
     PAD U2 6 LC#2
     PAD U2 7 GND
     PAD U2 8 LC#5
     PAD U2 9 NC
     PAD U2 10 NC
     PAD U2 11 LC#4
     PAD U2 12 +5V
     PAD U2 13 RESET
     PAD U2 14 +5V
     PART 7420 U1 DIP-14
     PAD U1 1 LC#11
     PAD U1 2 LC#14
     PAD U1 3 NC
     PAD U1 4 LC#13
     PAD U1 5 LC#12
     PAD U1 6 LC#3
     PAD U1 7 GND
     PAD U1 8 LC#4
     PAD U1 9 LC#10
     PAD U1 10 LC#9
     PAD U1 11 NC
     PAD U1 12 LC#8
     PAD U1 13 LC#7
     PAD U1 14 +5V
                                                                                             75

            END_UPDATE_LIST

Interpreting the Update List
    The Update list has a sub heading for every part. Under the sub heading a line
    follows for every pin of the part that will need a pad so that it can be soldered
    to the printed circuit board. On the same line the reference designator of the
    part, the pin number and its net name are listed. This is the file Board Creator
    will use to produce the printed circuit board..
    The next report is the bill of material. This report is easier to understand. Take
    a quick look at it, and move on to the end of it for an explanation of the report
    and its use.

                          Your name here
    -- Bill of Material Report ---------------------------------- Page: 1 --

    File: C:\CKTCRT\ mydesign.sch
    Title:
    Program: Logic Creator
    Date: 5/31/2000 10:22

    * = Pseudo-part

    Count Part-Name Corporate-No. Unit-Cost                        Description
    --------------------------------------------------------------------------------------------
    1        7420              002-00020-001              0.00 Dual 4-Input Nand Gates
    1        7474              003-00074-001              0.00 Dual D-Type Flip-Flop
    1        CONN-12           007-000012-002             0.05 12 Pin Connector
    2        LED-RED           007-000001-001             0.05 Light Emitting Diode,Red
    2        R330              004-00330-000              0.05 330 Ohm Resistor

    Total real parts: 7
    Total pseudo parts: 0
            Total part cost: $0.25
76

                                       Your name here
            -- Bill of Material Report ---------------------------------- Page: 2 --
            Part              Used-by
            --------------------------------
            7420              U1
            7474              U2
            CONN-12           W1
            LED-RED           D1 D2
            R330              R1 R2
            End of Report

Interpretation of the Bill of Material (BOM)
     This report produces a list of the standard components we need to purchase in
     order to build the circuit. It consists of five columns. The lists the total of part
     packages needed. The part-name list the part name from the part definition
     table. The corporate-no is a number that your company may assign to the part
     for inventory purposes. Unit-cost is the purchase value per package.
     Description is the description given to the part when originally created. All of
     these fields can be modified in the Part:Edit table of Symbol Creator.

     At the end of the first part of the BOM report the totals of real parts, pseudo
     parts, and the total cost is printed.

     The second part of the BOM report, lists all the part names and the
     corresponding reference designator. This portion of the report will be useful in
     uncovering wasteful use of multiple sections of IC's. For example, if four
     inverters are needed in a circuit, one 7404 package is enough, to fulfill this
     need. In many occasions though because of mistakes and corrections during
     the drafting process, the BOM may show 2 or more packages. What you need
     to do in a case like this is to go back to the schematic, and update the reference
     designator and/or section of the integrated circuit in question. You can easily
     do this by double clicking the symbol of the part. When finished always
     perform again a Design Check and then produce the reports again. Then check
     the reports to see if your corrections took effect!
                                                                                  77

Additional Training
    The tutorial you have just completed is designed to familiarize you with the
    basic steps in using Logic Creator to create a schematic. To become a more
    advanced user of Logic Creator, and to use its features to your best advantage,
    the following self-training procedure is suggested.

    Start the Logic Creator program and use the FILE/NEW command to create a
    new schematic (any size). Go through each of the commands on the menus,
    one at a time. For each command, display the help information with the F1
    key. Study the options for each command and practice each of these operations
    on the board. It is not necessary to construct a real or complete schematic. Just
    use the schematic sheet as a scratch area to practice the commands. For
    example, practice the DRAW/TEXT command by placing text of various sizes,
    boldness, etc. on the sheet. Move a text string. Move a whole area of text
    strings. Update a text string. Delete a text string. Do this for each command
    and you will quickly become a power user of Logic Creator.

    In the tutorial just completed, you were instructed how to perform each step in
    the construction of a simple schematic. Therefore, there was little or no
    opportunity to make changes to the schematic during the tutorial. In the real
    world, you will need to make changes, move things around, and correct
    mistakes. Changes are made with the SELECT command. In fact, it is the
    default command. Just press ESC to exit the current command, and you are
    running the SELECT command.

    Before any object on a board can be changed, it must first be selected. For a
    detailed description of the SELECT command, and how it is used to move,
    drag, stretch, and update objects, refer to the EDIT/SELECT command in the
    next chapter. Please practice using the select command. It will be used often.

Multi-level Hierarchy Design
    An alternative method of the hierarchy design is a multi-level hierarchy design.
    For example, if there were four schematic files in the hierarchy design, you
    could place the hierarchy part that represents the second schematic anywhere
    on the first schematic. On the second schematic, place the hierarchy part that
78

     represents the third schematic and so on (up to thirty-two levels). When
     generating reports using this method, you would open or load the first
     schematic that is at the top of this hierarchy chain.

     Selecting the hierarchy part on the first schematic and using the Hierarchy
     Push command would allow you to view/edit the second schematic. From the
     second schematic, you could select the hierarchy part that represents the third
     schematic and do another Hierarchy Push and so on. To return to the first
     schematic, you will need to pop as many times as you have pushed. Note:
     Selecting the Hierarchy Pop command while at the top of the hierarchy chain
     will simply un-load the current schematic. If any changes were made to this
     schematic, you will be prompted to save the changes.
                                                                                    79



Chapter 5
Hierarchical and Flat Designs
Logic Creator Libraries




                        Figure 5-1: The Library Menu

    The library menu as shown in figure 2-1 has three commands: Freshen, Add
    Part by Name, and Add Part by Library. The remaining entries are the
    “configured” libraries. In other words the libraries that are immediately
    available to the current schematic. These libraries are searched and are
    accessible instantly when the Freshen or Add Part by Name command are
    used. When a part is in a non configured library the Add Part by Library
    command is used. It takes much longer to access a part in a non configured
    library.

    Circuit Creator comes with many libraries all together containing more than
    25,000 standard industry parts. Going back to figure 5-1, which is the Library
    menu. The configured libraries can be a maximum of 10. If a configured
    library is a symbol only library then it does not show on the menu. Notice that
    their is only one symbol library. The Symbol.lbs library, which is the last one
    in the previous list. It is the library containing the symbols of all the different
80

     74 series sub-families of digital ICs. All the other libraries have the extension
     “LBP” which indicates that the part and symbol definition is in the same
     library. The Symbol.lbs library should always be configured because in
     addition to the digital symbols it also contains the symbols for the different
     sheet sizes available in Logic Creator.




                Figure 5-2: Configured Libraries Dialog Box

     Now the question is how do you configure the libraries you want?

     The answer is: from the File/Preferance/Libraries dialog box. So, click on File,
     then Preferences and then Libraries. The dialog box shown in figure 6-2
     appears. This dialog box has three areas that need to be filled for each library.
     The first one is Type. In this area you select part if the library contains both
     parts and symbols. These are the libraries with the extension “LBP”. The
     second area is the Menu name. Here you type in the text that you want to
     appear in the library menu of figure 5-1. It does not need to be the same as the
     library file name. The third area is the Path. Here you need to enter the correct
     path to guide Logic Creator in its search for the library and part. When you
     first install Circuit Creator all the libraries are under the CKTCRT directory. In
     the example of figure 5-2 the libraries were moved into a new sub directory
                                                                                            81

       called LIBRARY. Every library has to be preceded with the path C:\CKTCRT\
       and then the library name. The library name has to be typed exactly as shown
       in the earlier library list. If on your computer no changes were made after
       installing Circuit Creator the path should be C:\CKTCRT\ and then the library
       file.
       The next logical question is: Which 10 libraries out of the 86 should I
       configure for a specific project that I will start next? The answer is that you
       need to examine what parts your project requires and configure the libraries
       containing them. For example if your project does not use any digital parts you
       should not configure any one of the 74 series libraries. Also from the
       configured libraries start with the most frequently used library on the very top.

       Then follow with the less frequently used libraries. The reason is: when Logic
       Creator is searching for a part it starts with the library at the top first. If it is not
       found then continues to the next one and so forth. Therefore the program will
       be faster when the most frequently used parts are on the “surface”.

       A final word of caution. It is very frequent during the design process to change
       the definition of a part or its symbol. Then as a consequence is to go back and
       change all the schematics that use the modified parts. This is done by loading
       the schematic in Logic Creator and then executing the Freshen command. For
       the Freshen command to be effective though, the libraries containing the
       modified parts and symbols must be configured. If not, then nothing will
       happen and the annoying error message will appear: “part or symbol can not be
       found”.

Brief Description of the Most Commonly Used
Libraries
Caps.Lbp
      Contains most of the standard capacitors from 0.0001pf to 4,700µf.

Device.Lbp
       Contains generic devices and symbols for items such as headers, batteries, bnc
       connectors, buzzers, edge connectors, inductors, bjt transistors, fets, mosfets,
82

       and many other discrete devices.

Descrete.Lbp
      Contains discrete small signal transistors.

Inductor.Lbp
      Contains standard inductors from 0.1µh to 9mh.

Misc.Lbp
      Contains a little bit of everything. Diodes, crystals, DB connectors, switches,
      transformers, etc.

Powerdev.Lbp
      Contains power transistors.

Resistor.Lbp
       Contains resistors, potentiometers, and resistor networks ranging from oΩ to
       2.2MΩ.

Rf.Lbp
      Contains parts and symbols like antennas, coaxial accessories, vacuum tubes,
      rf switches, etc.

74.Lbp
      Contains almost all the standard 74 series TTL devices.

80’s.Lbp
       Contains most of the Intel 8XXXX series devices such as 80186, 80286,
       80386, 80486, and peripherals like the 8255, 8289 etc.

Analog1.Lbp
      Contains 1,723 linear Ics from National, Analog Devices, RCA, etc.

Analog2.Lbp
      Contains 1,723 linear parts from Motorola, Signetics, Burr Brown, TI, NEC,
      etc.
                                                                       83


Motorola.Lbp
      Contains 4,250 parts. Anything from diodes, transistors, linear Ics,
      communication Ics, etc.
84
                                                                                    85



Chapter 6
Logic Creator Reference Section
This is a reference section. It lists all Logic Creator menus and their commands. A
brief explanation follows each command and how it is generally used.

Read through this section to familiarize your self with all the Logic Creator
commands. Please refer to it while you create new schematics to answer your
questions. This section along with context sensitive help should be able to resolve all
your questions.

Logic Creator Commands
       The following information is a list of all the Logic Creator menus and their
       associated commands. They are listed here for you as a reference. Go ahead
       and study each one of them so you will have an idea of what functions are
       available in Logic Creator. You are not expected to remember all of these
       commands and how to use them. You will be aware of them though and you
       will also know where to go and find the answers when you need to later on. Do
       not forget that the same information is available using context sensitive help
       (F1) or under HELP menu.

File Menu
       The file menu provides commands for loading and storing schematics,
       printing, printer set-up, displaying program version information, exiting the
       program, and for executing Dos commands. You normally start and end an
       Logic Creator session by using commands on this menu.
86




                            Figure 6-1: File Menu

Open (Ctrl + O)
     Use this command to load an existing schematic file for editing, viewing, or
     printing. Upon loading a file, the program will automatically display sheet one
     of the schematic in the edit window.




                          Figure 6-2: File/Open Dialog-box
                                                                                   87

     Select the file to be loaded from the dialog-box that appears. If the name of the
     schematic that you want to load is in the list-box, you may press Enter twice or
     double click with the mouse to directly make the selection.

     All Logic Creator schematic files must have the extension ".SCH".

New (Ctrl + N)
     Use this command to create a new schematic. If a schematic is already loaded
     and changes have been made, you will be allowed to save it before making the
     new schematic.




                           Figure 6-3: File/New Dialog-box

     Fill in appropriate values in the format dialog-box that appears, and press OK
     to start the new design.

Save (Ctrl + S)
     Use this command to immediately store a schematic to its file. Any previous
     version of this file is backed-up first (renamed with an extension of ".Bak").
88

Save As (Ctrl + A)
      Use this command to store the current schematic to a different or new file. The
      file-picker dialog-box, showing the current file name of the schematic, will be
      displayed. Enter the new file name and press OK to save the schematic.




                       Figure 6-4: File/Save as Dialog-box Menu

      If a file of the same name already exists, your will be given the option of
      backing-up that file, writing over that file, or canceling the command.

Print (Ctrl + P)
      Use this command to make hard-copy prints or plots of the current schematic.
      A dialog-box will appear, allowing you to specify the following printing
      controls.

      Format:
      Specifies the printer page size (not the size of the schematic sheet).

      Sheets to Print:
      Lets you specify the sheet(s) you want to print.
                                                                               89




               Figure 6-5: Printing Schematic file dialog-box

Scale:
Specifies the printing scale when not scaled to fit the printer sheet.

Pause each page:
If checked, the printing will pause between each sheet, allowing you to prepare
the printer.

Out put to File:
Logic Creator supports printing your schematic directly to a Dos file. Creating
this print file is useful when the printer or plotter is in a remote location. The
print file can be transferred to another computer or sent to a printing service
via a floppy disk or modem. When a print file is created, the same information
that would normally be sent to the printer is directed into a Dos file.
90

      Enabling the output to file option in the Print dialog box will direct the output
      to a file when printing in Logic Creator. The print file will be created in the
      same directory that the schematic file was loaded from. For instance, when a
      schematic is loaded from the directory:

      C:\CKTCRT\Demo.sch

      The output print file will be created as:

      C:\CKTCRT\Demo.prn

      Note: You can not specify the output path or name of the print file. The file
      name will be your schematic's base name with the extension .prn. Also, be
      certain that you have plenty of disk space available for generating a print file.
      Depending on the size of your schematic and the number of sheets that are
      selected, the print file can easily reach one or more megabytes in size.

      When a print file is generated, a simple Dos copy command (entered at the Dos
      prompt) can be used to send the file to the printer. For example:

      COPY /B Demo.prn LPT1

      In the above example, the file (Demo.prn) will be copied to the printer port
      LPT1 (or parallel port 91). The /B option informs Dos that this file is in a
      binary format. If you find that your file prints stray lines or unrecognizable
      characters, make sure that the /B option is used when the file is copied to your
      printer.

      One final note about creating a print file is that only one file will be generated
      regardless of the number of sheets of the schematic you are printing.

Setup Printer ( I )
      Use this command to select the printer device and set the following printer
      controls.
                                                                               91




                Figure 6-6: Priter Setup Dialog-box

Printer Name:
Specifies the type of the printer device you have installed.

Paper Size/Source:
Specifies the page size and relative quality to use from a list of page sizes
available for this device.

Properties:
You can select all other options related to printer device with these options like
resolution, paper size, Fonts Etc.

Orientations:
Portrait/ Landscape, You can change your print image portrait/landscape as per
your paper size

Port:
The remainder of the controls are used to specify the destination of the print
output and the configuration of the printer port.
92

Preferences
       The system menu provides commands for changing the configuration of the
       Logic Creator system.

       The user configuration settings are stored in the file LC32.CFG. This file must
       reside in the same directory as the LC32P.EXE program. The settings in this
       file are initially set during installation. The commands on this menu may be
       used to change these settings. The file is an ASCII text file. Although not
       recommended, the file may be directly edited with a text editor.




                        Figure 6-7: Preferance Dialog-box

Paths/Options:
      Changes to the configuration are saved when the program is exited. Some may
      not take effect until the program is exited and restarted. Paths/Options use this
      command to configure the default file paths other operating options for the
      Logic Creator program:




                        Figure 6-8: Paths/Options Pop-up Menu
                                                                                  93

Drawings path:
The path to where your drawing (or schematic) files (*.sch) are located is
entered in the above dialog box. This path name is entered in the Drawings
Path field and must be terminated with a backslash This will be the default
directory that is searched for any existing schematic files.

Scratch path:
When objects are cut or copied on the schematic, their image is stored in a
temporary file (paste.$$$) called the paste buffer. The path to where this
temporary file is written is determined in the Scratch Path field in the above
dialog box and must be terminated with a backslash ( / ).

Chaeck Point Path:
The Logic Creator program has an auto-backup (or timed-backup) feature that
will periodically save the current schematic to a check-point file (.ckp) in case
of a power loss. The path to where this file is saved is determined in the
Check-Point Path field of the Paths/Options dialog box and must also be
terminated with a backslash ( \ ). When the Logic Creator program is re-started
after the occurrence of a power loss and you re-open your schematic design,
this path is searched for the existence of a back-up file.

Banner:
The name entered in the Banner field of the Paths/Options dialog box will
appear in any report generated (such as a bill of materials, net-list, pin-list, etc.)
and will also appear in the title block of your schematic. The default banner is
"Your Name Here".

Chaeck Point Seconds:
The amount of time that passes before the schematic is automatically saved is
determined in the Check-Point Seconds field. The number entered here is in
seconds. For example, in the above Paths/Options dialog box, the value 300 is
entered. This will back-up the schematic design every five minutes. To disable
this feature, enter a zero (0) in the Check-Point Seconds field. The maximum
value that may be entered here is 3600 (or one hour).
94

       Ground Net Symbols:
       Finally, with the Ground Net Symbols option enabled, any wire or pin of a
       component that is assigned with the net names: GND, GNDA, or GNDC will
       appear with the appropriate graphic symbol for the ground net. When this
       option is disabled, the ground net name will be spelled out on your schematic
       (instead of displaying the ground symbol).

Libraries:
      Use this command to configure the part libraries that you want to appear on the
      library menu, and the symbol libraries to use. You must enter the full path
      name for each configured library, the text you want to appear on the library
      menu, and the type of library.

       Although the symbol libraries will not appear on the menu, they will be used
       when a part references a symbol to locate the definition of that symbol.




                     Figure 6-9: Library Configuration Menu
                                                                                    95

Drawing Colors/Width:
      The colors and widths of the items used on your schematic can be configured
      by selecting Drawing Colors from the File/Preferences menu. For example,
      you can make the width of the I/O pins for your components wider so that they
      can be easily distinguished from the wires that you have attached to them. This
      would be done by changing the Lead width.

       Any of the changes made in the Drawing Colors/Widths dialog box will affect
       all of the schematics that are loaded into Logic Creator. These changes (to the
       widths) will also affect the appearance of the schematic when it is printed out.
       Also, any of the changes made may require that you exit Logic Creator and
       restart the program for "the changes to take affect". The colors and widths that
       appear in the dialog box on the following page are stored in the configuration
       file for Logic Creator (lc32.cfg) when you exit the program.

       Some experimentation may be required until you obtain colors that are suitable
       to your eyes. The colors that are assigned to dialog boxes, pull-down and
       pop-up menus are determined by the colors that are configured for Windows.
       Refer to your Windows manual for information about configuring these colors.




                   Figure 6-10: Colors/Widths Pop-up Menu
96

Application Colors:
      Use this command to configure the colors for the Logic creator windows, such
      as the color of the rulers, status line, etc.

       Note: Logic Creator like all other windows applications uses the windows
       system colors for menus, dialog-box windows, borders, etc. If you want to
       change these colors, from the windows main program group, double click on
       the Control Panel icon, and then double click on the Color icon. You can now
       change the system colors. Use windows context sensitive help if needed.

       Cautions: While selecting the color, make sure you don’t select the same color
       for background and foreground.




                 Figure 6-11: Application Colors Pop-up Menu

Exit (Alt + X or X)
       Use this command to exit the program and return to the system prompt. If
       changes have been made to the current schematic and not saved, you will be
       given the option of saving the schematic before exiting.
                                                                                  97

File Names (Alt + F and 1, 2, 3, 4)
     The bottom of the file menu will list the file names of the last four schematics
     that were referenced. You may directly open one of these schematics by
     selecting it from the menu. This command provides fast access to the
     schematics that you have used recently.

Draw Menu (Alt + D)
     The draw menu provides commands for drawing schematics. Schematics are
     made by placing part symbols on a schematic sheet and wiring the parts
     together. Optionally, names may be assigned to the wiring nets. Also, reference
     text and lines may be added to enhance the drawings.

     For adding part symbols to a schematic, refer to the commands on the library
     menu.




                               Figure 6-12: Draw Menu

Wire (W)
     Use this command to draw wiring lines on a schematic.

     To draw a wire line, move the cursor to where you want to start drawing one
     end of the wire and Enter. Now, move to the other end of the wire segment and
     Enter to complete this segment. If you want to continue drawing the wire from
     this location, move to the end of the next segment and Enter. To start a wire in
     a new location, Esc , then move to the new location and repeat the process.

     When you want to add a connect dot, move the cursor to where you want the
     dot and press Enter twice. This is the same as drawing a wire with no length.
98


     Wires that touch at their end tips, or cross at a connect dot are electrically
     connected to the same net. Wires that cross, but have no connect dot, are not
     electrically connected.

     Use the O key, or click on the status line with the left mouse button, to set the
     type of wire line segment you want to draw. The current type of line is
     displayed in the bottom status line. Any of the allowed line types may be used
     to draw wires.




                       Figure 6-13: Wire types Pop-up Menu

Net Name (N)
     Use this command to label a wire or part-pin with a net name.

     Move the cursor to a position on a wire, or the tip of a part- pin, and Enter. A
     dialog-box will appear, allowing you to enter the text for the net name and to
     set the location of the net name relative to the wire or pin.
                                                                                  99

     Each net name will have a small dot displayed on the screen at its anchor point.
     This dot helps show which wire or pin the net name it is assigned to.

     This dot is for reference on the screen only, and does not appear in hard-copy
     prints.

     To repeat a series of net names, such as X1, X2, X3, etc., check the Repeate
     box and fill up the repeate number of times. When you press Ok, the current
     net name will be added, and the dialog-box will reappear with the next name
     and location in the sequence. Continue to press Ok until all the names of the
     series have been added. Cancel to stop the repeat cycle.




                    Figure 6-14: Net Name Pop-up Menu

Port (P)
     Ports are also net names. Ports are typically used to label nets that come from
     or continue on other sheets. They show the net name within a graphic symbol
100

      that indicates the directional flow of the net. If desired, ports may also be used
      to label nets on the same sheet of logic.

      Move the cursor to a position on a wire or the tip of a part-pin and Enter. A
      dialog-box will appear, allowing you to enter the text for the net name and to
      choose the direction of the port.

      As with the Net Name command, the port names may also be repeated.




               Figure 6-15: Port Name command Pop-up Menu

Bus (B)
      Use this command to draw bus lines on a schematic.

      To draw a bus line, move the cursor to where you want to start drawing one
      end of the bus and Enter. Now, move to the other end of the bus segment and
      Enter to complete this segment. If you want to continue drawing the bus from
      this location, move to the end of the next segment and Enter. To start a bus in a
      new location, Esc, then move to the new location and repeat the process.
                                                                                 101

     Use the O key, or click on the status line with the left mouse button, to set the
     type of bus line segment you want to draw. The current type of line is
     displayed in the bottom status line. Any of the allowed line types may be used
     to draw buses.




                   Figure 6-16: Bus Line command Pop-up Menu

Line (L)
     Use this command to draw reference lines on a schematic.

     To draw a line, move the cursor to where you want to start drawing one end of
     the line and Enter. Now, move to the other end of the line segment and Enter to
     complete this segment. If you want to continue drawing the line from this
     location, move to the end of the next segment and Enter. To start a line in a
     new location, ESC, then move to the new location and repeat the process.

     Lines are used only to enhance the graphic image of the schematic and carry
     no electrical information. Do not use lines in place of wires.
102

      Use the O key, or click on the status line with the left mouse button, to set the
      type of line segment you want to draw. The current type of line is displayed in
      the bottom status line.




                      Figure 6-17: Line command Pop-up Menu

Text (T)
      Use this command to add reference text to a schematic.

      Move the cursor to the location of where you want the lower left corner of the
      text line and Enter. A dialog-box will appear which lets you enter the text, set
      the size of the text, and other text parameters.

      This command adds text that is for reference only, and internally conveys no
      electrical information. Do not use this command to label net names.
                                                                                103




                 Figure 6-18: Text Command Pop-up Menu

Edit Menu (Alt + E)
     The edit menu provides commands for changing a schematic.




                            Figure 6-19: Edit Menu

Sheet Format (E)
     Use this command to change the accounting information and the format of a
     design. A dialog-box will appear, allowing you to change the design title,
     adjust the sheet size, choose the format symbol for each sheet, as well as other
     house-keeping values.
104




                  Figure 6-20: Edit/Sheet Format Command

      Change the set-up values as desired, then press Ok.

Undo (F2)
      If you make an editing mistake, use this command to undo the command you
      just executed. The schematic will be restored to the way it was prior to
      executing the previous command. Executing undo again will restore the
      mistake.

Cut (Shift + Del)
      This command is used to delete objects from a schematic, placing them in the
      paste buffer.

      Select the objects that you want to delete, then execute this command to delete
      the selected objects.

      The deleted objects are placed in the paste buffer, replacing its previous
      contents. To retrieve objects from the paste buffer, refer to the Paste command.
                                                                                105

Copy (C)
     Use this command to make copies of objects on a schematic.

     Select the objects that you want to copy, then execute this command. A copy
     of all the selected objects will be placed in the paste buffer, replacing its
     previous contents. To retrieve objects from the paste buffer, refer to the Paste
     command.

Paste (Shift + Ins)
     Use this command to retrieve objects stored in the paste buffer.

     After starting this command, a rectangle indicating the area of the objects
     currently in the paste buffer will appear on the cursor. Move the cursor to the
     location where you want a copy of these objects to be placed, and Enter.
     Continue to place more copies, or Esc to cancel the command.

Delete (Del)
     Use this command to delete objects from a schematic.

     Select the objects that you want to delete, then execute this command to delete
     the selecte objects.

     The deleted objects are not placed in the paste buffer. For placing deleted
     objects in the paste buffer, refer to the Cut command.

Update (U)
     This command is used to change the values assigned to objects on the
     schematic. For example, if you want to change the width of a line, or rotate a
     symbol that is already on the schematic, use the update command. This
     command may also be used to review the values currently assigned to an
     object, without making any changes.

     To update an object, first select the object that you want to update, then
     execute this command. This command may also be executed by pressing Enter
     twice while the cursor is on a selected object, or by clicking the left mouse
     button while pointing to a selected object.
106


      A dialog-box specific to each selected object will appear. Change the object's
      values as desired, then press Ok. If more than one object is selected, pressing
      Cancel will stop the update sequence.

Select (S)
      The select command is the default Logic Creator command. That is, when no
      other command is active, the select command is active by default.

      The select command is used when you want to make changes. It is used to
      point out which objects you want to change. Before an object can be changed,
      it must first be selected. Once selected, an object may be deleted, moved,
      stretched, or updated.

      For example, if you want to delete a part from a schematic, first select the part
      you want to delete, then press the Del key. If you want to move an object on a
      schematic to a new location, first select the object, then grab it with mouse and
      move it to the new location.

      To select an item, or group of items, first pick the Select command from the
      Edit menu, or just Esc the current command to start it by default.

      To select a single object, move the cursor on top of the object you want to
      select and press the Enter key twice. With the mouse, just point at the object
      and click the left mouse button. When an object is selected, it will appear on
      the schematic in the configured select color.

      To select more than one object, move the cursor to one corner of the area that
      bounds the objects and Enter. Now, move to the other corner and Enter again
      to select all the objects within this area. With the mouse, hold down the left
      button and move the mouse to stretch-out the desired area. Release the button
      to select the objects.

      Use the O key, or click on the status line with the left mouse button, to pop-up
      the select options dialog-box. This dialog-box allows you to control which
      objects will be selected, and which objects will not be selected.
                                                                           107

When touching is active, any objects touching the selection area will be
selected. When bound-by is active, only the objects completely bound by the
selection rectangle will be selected.

When component is active, selecting a part symbol will also select any other
objects that connect to this symbol. This makes it easy to drag a symbol, along
with the lines and net names that connect to it. When flat is active, only the
symbol is selected.

Each individual object type that appears on a schematic may be enabled or
disabled for selection.

To unselect, make a new selection, select in an area on the screen where there
are no objects, or pick the Edit/Unselect command.

Once an object is selected, the following operations may be applied:

•   Cut, Copy, Erase, Update - Refer to the specific command.
•   Move/Drag - Press Enter while the cursor is within the select area
    indicator, and then use the arrow keys to move/stretch the selected objects.
    Enter again to place the objects (stop moving). With the mouse, press the
    left mouse button down and drag the objects to the new location. Release
    the mouse button to place theobjects.
•   Stretch - Lines, wires, and buses may be stretched by selecting only the
    portion of the object that you want to move. For example, if you only select
    one tip of a line, then the end of the line will stretch as it is moved. The
    other end of the line will remain anchored. This technique may be used to
    quickly reshape wires and bus lines.
•   As you can see, the select command is a very convenient and powerful
    command that works in combination with other commands. All editing
    changes are done through the use of the select command.
108

Unselect (Z)
      Use this command to unselect all objects on a schematic.

      You may also unselect all objects by selecting in an area of the schematic that
      has no objects.

Select Trace (R)
      Use this command to select a wire segment and all the wires that this wire
      segment is connected to. This command is normally used to immediately
      verify that a net connects to all the locations you think it does.

      After starting this command, move the cursor to a point on any of the wires of
      a net and Enter. This wire, and all the wires that are electrically connected to it
      will be selected.

Break Line (Ctrl + B)
      The Break Line command is used to break lines, wires, or buses to two
      sections. First the item to be broken is selected using the Select command, and
      then the Brake Line command is applied.

Library Menu (Alt + L)
      The library menu is used to place part symbols on a schematic, and for
      updating the schematic with the latest part and/or symbol definitions.

      A library is a single Dos file, capable of storing and retrieving many individual
      entries. Each library contains items of a specific type, such as parts or graphic
      symbols.

      The part libraries that you use most often may be configured to appear directly
      on the lower portion of this menu (see the Preferance/Library command). This
      provides fast access to the libraries that are used most often. The Library/Add
      Part command may be used to select libraries that are referenced less often.
                                                                                  109




                          Figure 6-21: Library Menu

Freshen (F)
     Copies of part and symbol definitions used on a schematic are stored in each
     schematic file. If you update the definition of a part or symbol in a library, the
     freshen command may be used to load a fresh copy of the latest definition into
     the schematic.

     After selecting this command, a dialog-box will appear that allows you to
     update symbols, parts, or both symbols and parts.




               Figure 6-22: Freshen command Pop-up Menu
110

Add Part by Name (J)
      Use this command to retrieve a part that you know its part name. This
      command works only with parts in the configured libraries.




                Figure 6-23: Add Part by Name Pop-up Menu

Add Part by Library (A)
      Use this command to add a part from a library that is not shown on the library
      menu.




          Figure 6-24: Add Part by Library command Pop-up Menu
                                                                                 111

     After starting this command, use the file picker dialog-box that appears to
     locate and select the part library you want to use. Next, use the dialog-box that
     appears to select one of the parts from the library.

     The outline of this part will appear on the cursor. Move to the location where
     you want to place the part symbol. The bottom status line will show the current
     rotation and mirror settings. If necessary, use the F9 key to toggle the mirror
     value, and/or the F10 key to toggle the rotation value. Enter to place the
     symbol. An appropriate reference and section designator will be assigned for
     you. Refer to the Edit/Update command if you want to change any of these
     values after the symbol is placed. Continue placing this symbol, or Esc to
     cancel the command.

Configured Libraries
     If the part library that you want to use appears on the library menu, select it
     directly from the menu. Next, select the desired part name from the library.
     Use the technique described above to place it on your schematic.

View Menu (Alt + V)
     The view menu provides commands for selecting the current view of a
     schematic. You may pan, zoom, or select a specific sheet of the schematic for
     viewing.

     In addition to the commands that are directly on the menu, the following
     commands may also be used to pan the view.

     •   The display will automatically pan when the cursor is moved with the
         arrow keys, and the edge of the edit window is bumped.
     •   To pan with the mouse, use the slide-bars along the right and bottom edges
         of the window to select a desired view. Clicking the mouse on the slide-bar
         arrows will pan a small amount in that direction. Clicking in the area
         between the arrows and the slider will pan a full page. Grab the slider with
         the mouse and drag it to select the view directly. The size of the slider
         indicates the portion of the sheet that is currently in view.
112

      •   To center a point on the schematic in the view, move the cursor to the point
          and press the Shift + Numeric 5 Key.




                          Figure 6-25: The View Menu

Sheet (V)
      Use this command to select the sheet of a schematic that you want to view.
      Select the sheet you want to view from the list in dialog-box that appears.




                  Figure 6-26: Sheet View Pop-up command
                                                                               113

Grid / Cursor(G)
     Use this command to turn the reference grid on or off, and to set the step size
     of the reference grid.

     The grid is for reference only, and is not part of the actual schematic. The
     reference grid will not appear on hard-copy prints of the schematic. Also, the
     reference grid does not affect the cursor motion.




                 Figure 6-27: Grid command Pop-up Menu

Pan Up (PgUp)
     Use this command to pan the drawing up. The pan direction refers to the
     change in the view, not the direction that the sheet appears to move. For
     example, panning up indicates that you want to view more of the area toward
     the top edge of the schematic.

Pan Down (PgDn)
     Use this command to pan the schematic view down.

Pan Right (Shift + >)
     Use this command to pan the schematic view right.

Pan Left (Shift + <)
     Use this command to pan the schematic view left.
114

Zoom Home (Ctrl + Home)
      Use this command to view the upper-left corner of a schematic at the standard
      zoom scale.

Zoom In (Ctrl + PgUp)
      Use this command to zoom in on the schematic view. Objects in the view will
      appear bigger and more detailed; however, you will be able to see less area of
      the schematic sheet.

Zoom Out (Ctrl + PgDn)
      Use this command to zoom out on the schematic view. Objects in the view will
      appear smaller and less detailed; however, you will be able to see more area of
      the schematic sheet.

Redraw (Ctrl + R)
      Use this command to redraw the schematic at its current pan and zoom scale.

Reports Menu (Alt + R)
      The reports menu provides commands for showing the current status of your
      schematic, checking your schematic for errors, generating formal production
      and engineering design reports, and for performing back-annotation.




                          Figure 6-28: Reports Menu

Status (Q)
      Use this command to display the current number of objects in your design,
      memory utilization, etc. The report is displayed on the screen only.
                                                                            115




                Figure 6-29: Report/Status Pop-up Menu

Design Check (D)
    Use this command to check your design for errors. If no errors are found, you
    will receive a message "No errors detected".




                   Figure 6-30: Design Check Error Message
116

      If errors are detected, a dialog-box giving details of the exact problem will
      appear. Also, the location of each error will be flashed on the schematic. All of
      the detected errors may be reviewed from this dialog-box, one at a time.

Formal/ Export (Y)
      Use this command to generate production and engineering reports from your
      design.

      Use the dialog-box that appears to check-off the reports that you want to
      generate. Press Ok to start making the reports.




                    Figure 6-31: Formal/Export Dialog-box Menu

      The reports are always written to disk files, and are in ASCII printable format.
      The files have the same path and base name as the schematic. A file name
      extension is added to identify each report:
      • .upd         PCB update list.
      • .bom         Bill of material reports.
      • .net         Net list/Loading.
      • .spc         Net list Spice.
      • .pin         Pin list reports.
      • .dmp         Pin table dump list.
                                                                                    117

     For example, if the file name of a schematic is "mydesign.sch", the net-list
     report will be in "mydesign.net".

     The report files may be printed with the standard Dos print command.

Back Annotate (K)
     Use this command to process a back-annotation list.
     A back-annotation list is a text file which contains a list of "was-is" definitions.
     This operation is usually performed after a PC board is complete, and changes
     are now required to make the schematic agree with how the actual board was
     routed.

     The format of a Logic Creator back-annotation file is as follows:
            $BackAnnotate
            was[-section] is[-section]
            was[-section] is[-section]
            ...    ...
            $End

     In the following example:
             $BackAnnotate
             U25 U21
             U13-C U13-A
             U13-A U14-C
             U14 U15
             ...    ...
             $End

     All part symbol references to U25 will be changed to U21. U13 section C will
     be changed to U13 section A, etc.

     The back-annotation file can be created with a text editor, word-processor, or
     automatically by some PCB layout systems.
118

Help Menu (Alt + H)
      This menu allows you to get on-line help on any command or menu. It is
      organized like a book, with an index of the chapters and detailed information
      in each chapter.




                               Figure 6-32: Help Menu

Context/Index (F1)




                 Figure 6-33: Context/Index Help Dialog-box
                                                                                119

     This option gives you the index of the help manual. Move your mouse pointer
     above the word you need help on. If the arrow changes to a pointing hand then
     help is available, and you can access it by clicking on that word.

     This is the most important feature of the Help menu. It allows you to get direct
     help on the specific command you are interested by highlighting the command
     and then pressing F1.

Using Help (Alt + H and U)
     This is a tutorial on how to use the help menu of Logic Creator. Please go
     through this tutorial as many times as you need. It will help you became a
     better user.

About Logic Creator (H)
     Use this command is display the copyright notice and current version/release
     number of the program.




                           Figure 6-34: About Dialog-box
120
                                                                            121



Chapter 7
How To Section For Logic Creator
How to find library symbol
    All schematic symbols are categarized into various Library file with the
    extension LBP. Most part library are self explanetory for example 74LS or
    Intel or Motorola. But some part number, for example 57402A, may not lead
    to specific group. The following procedure will make it easy for you to find
    these type of unique parts.

    First go to Help pull down menu and select Contex and Index. Then click on
    Index then press Find and the following screen will show.




            Figure 7-1: Logic Creator Topic Help Diaglog-box
122

      Now type in the number you are looking for, in our case 57402 and the bottom
      half of the screen will show Amd.lbp. It tells us that our part is in Amd library.




               Figure 7-2: Logic Creator Topic Find Dialog-box

      If you do not find the part you are looking for this way use the following
      method.

      There two files text files provided on the CD called Ckt_liblist.txt and
      Ckt_liblist.doc.

      These files shold be in your CKTCRT directory. If you don’t have these files,
      you can download the file from our web site:

                       http://www.advancedmsinc.com/download

      TXT file is simple Text file that can be opened by Notepad or Wordpad. DOC
      file is Microsoft Word compatible file. Open one of these file and using Find
      function you can look for the desired component.
                                                                                 123

Copy Part and Symbol from one library to other
library
Copy Part
    Select Library under Part. Select Part. You will see following dialog box.




                      Figure 7-3: Edit Part Dialog-box

    Enter new library name (including Path name if different ) where you want to
    move the part to in section Library.

    Press Ok, Save
124

Copy Symbol
      Now select symbol library and pick symbol you want to move. While the part
      is on your screen, select new library whwer you want to move this part. Then
      Select Save under Symbol.

How to Rotate Components
      When you are placing a component from symbol library on to schematic sheet,
      pick the componen from the symbol library. Move the part at a desired location
      but do not click Mouse or press Enter. As it shows on the following figure the
      component does not show the pin number and components reference number
      clearly. Also notice the status line on the bottom of the screen. It shows

         Enter: Add=ls00.prt, F9:M=None, F10: A=0, O: Options, ESC: Cancel

      F9 function key allows to mirror the part and F10 function key allows to rotate
      the part in 90 degree increment. Once you have the desored location and
      desired direction of the part you are placing, Press Enter or Right Click Mouse.
      Now by pressing F10 you can rotate the part.




                     Figure 7-4: Add Part by Name LS00
                                                                            125

Rotate the Part after Placing on the Sheet
    Once you have placed the part, double click the component. You will see the
    following screen. Select the correct option on the Rotate menu. Here you have
    four selections. None, 90, 180 and 270 Degrees. Select the deisired direction
    and Press Ok.




                   Figure 7-5: Update part Dialog-box
126

Grid
      There are three options for the Grid selection as shown on the following figure.

      No grid, Solid Grid and Dots. Solid Grides and Dots have option for X and X
      Step.




                   Figure 7-6: Grid command Pop-up Menu

      The following screen shows Grid with Dots selection.




                Figure 7-7: Grid command with Dots Selection
                                                                                  127

Adding or Placing Discrete Components




              Figure 7-8: Add Part by Library Pop-up Menu

   Adding Discrete components in Logic Creator has been made much easier in
   the latest version in compare to previous version as well as some of competitor
   version. In previous version, if you want to add a resistor, first you will need to
   create specific graphical representation Symbol and part detail. Now you will
   be able to add all the discrete parts such as resistor, capacitor, inductor, crystal
   etc in the following Easy way.

   First of all make sure you have configured " Discrete Components " as a one of
   the configured Library. To add a part go to Library Pull-down menu and select
   Discrete Components. You will see following Dialog Box.

   Select C.PRT ( to add a capacitor ) from the available selections, and place
   symbol at the desired place. If you need to mirror the part press F9 and F10 to
   Rotate 90 degrees. Now Double click on the Capacitor you just placed on the
   sheet and the following Dialog box will appear.
128




                      Figure 7-9: Part Update Dialog-box

      Enter the desired capacitor value in Rating selection and Corp part number in
      Part # selection. Select desired Footprint in Footprint Selection. If you are not
      sure about the Footprint, turn on Preview option. Press Ok and you are done.
      The same procedure can be use to add crystal, inductor, NPN or PNP transistor
      or FET.
                                                                            129

Add/Search Part by full name or partial name
    Go to Library Menu and Select Add Part by Name…. And you will see the
    following dialog box.




               Figure 7-10: Add Part by Name Dialog-box

    Enter full part for example LM386. and press Search Libraries button.
    You will see the following Dialog Box.




                Figure 7-11: Search Result for LM386 part

    You can also enter parital part number. For example 386 as follows and you
    will find all the part which has 386 string in it.
130




                   Figure 7-12: Serach Part by Name “386”

Using the BUS Command
      Placing a bus on your schematic is completely optional. It is often used to
      clean up the appearance of your schematic. A bus can make it easier to follow
      a group of nets (such as address and data) from one section of your schematic
      to another or from one page of your schematic to another.

      Note: Bus lines do not contain electrical information about how the pins are
      connected on your schematic and are ignored by Logic Creator when
      generating reports or running the design rule checks.

      It is best to explain how a bus is used by an example., The following is an
      example of using a bus line to show a typical design that uses an eight bit data
      bus:
                                                                              131




              Figure 7-12: Using the Bus Command.

The following figure will give the same results as in the previous example:




              Figure 7-13: Using the BUS Command

In both cases, the same net names are assigned to the I/O pins of the
components.

Note: It is the net name that connects the I/O pins together, not the bus line. As
you can see, the bus line helps to clarify the schematic. This may not be as
apparent in the examples shown above, but on a large schematic with many
components, the bus line can be used to show that the groups of nets (D0-D7)
are connected to a different section of your schematic. By following the bus
line on the schematic, you can easily find other components that are utilizing
the same net names.
132

      The following example shows an improper use of the bus line:




                       Figure 7-14: Invalid Use of a Bus.

      In Figure 7-14, there is no information showing which pins of U1 and U2
      should be connected.

      Important: There are only two ways to show that the pins on your schematic
      are electrically connected together. One way is to connect the two pins together
      using a wire. The second way is to assign the two pins with the same net name.
      The following example shows a common mistake that occurs when placing a
      bus on the schematic.




                       Figure 7-15: Invalid Use of a Bus.

      The mistake that was made in the last example is that the ends of the wires
      meet in the middle (where the bus line crosses over them). Remember that bus
                                                                          133

lines are ignored by Logic Creator and are used for appearance only, therefore,
we should not forget the rules for the other items that are placed on the
schematic such as wires. As mentioned earlier in the section "WIRING YOUR
SCHEMATIC", wire segments will be considered as one continuous wire
when they touch end-to-end. Logic Creator will give an error in the previous
example because there are now two net names assigned to each of the wire
nets.
134
                                                                              135



Chapter 8
Symbol Creator Basics
What is Symbol Creator?
   Symbol Creator is the module of the Circuit Creator CAD system that allows
   us to create new part definitions and their graphic symbol that is used by Logic
   Creator. Every part in the Circuit Creator system has three characteristics:
           1. Name
           2. Symbol
           3. Footprint

   In Symbol Creator we create the part definition first. In the part definition we
   specify the part name, part symbol, and part footprint. Then in the graphic
   section of Symbol Creator we design the graphic image of the symbol, and in
   Board Creator we design the graphic of the footprint of the part. I am sure you
   are very anxious to create your first part. Let's get going.

Launching Symbol Creator
   From the Circuit Creator Start Menu group, click the Symbol Creator icon and
   the screen of figure 8-1 will appear.
136




               Figure 8-1: Opening screen of Symbol Creator.

A Tour of Symbol Creator Opening Screen
      Beginning with the top of the screen we have the title bar which displays the
      program we currently run. The next line is the action or menu bar which
      displays the titles of the pull down menus. Underneath we have the large
      editing area. The editing area is divided into two windows. The one on the left
      displays the graphic image of the symbol being edited. The right window
      displays the text definition of the symbol being edited. The bar at the bottom of
      the screen is the command status window. It displays the active command, and
      any options of it.

      Let's examine each menu and talk briefly about its functions.

      The File menu allows you to set the Paths/Options, Libraries, Drawing Colors,
      Application Colors, and Exit the program.

      The Part menu is a major player in Symbol Creator. It is here where you create
      part libraries, create or modify parts, and print the part definition.
                                                                             137

    The Symbol menu is where you will be spending a lot of time creating new
    symbols, or modifying existing ones. From this menu you can also delete, or
    save symbols, and print the symbol text definition as well.

    The Edit menu has the magical command Undo which we should be very
    grateful for. This menu enables you to insert or delete too.

    The View menu provides us with the tools to easily examine the graphic
    symbol being edited.

    The Help menu provides on line help just about all menus and commands.

Looking at a Part Definition
    Let's see how we can examine the definition of an n-type mosfet. From the Part
    menu click on Select Library. The Select Library dialog box pops-up. Click on
    device.lbp, and press OK. The dialog box closes and the tile bar now displays
    Symbol Creator C:\CKTCRT\Device.lbp, i.e. the program title and the path of
    the selected library. Now click again on Part, and select Open. The Open entry
    dialog box appears. The mosfet_n.prt part is not on the displayed window.
    Click the down arrow of the vertical slide bar until it appears in the display
    window. Click on mosfet_n.prt, and then on OK. Finally, the Part:Edit dialog
    box pops up.
138




                       Figure 8-2: Part:Edit Dialog Box.

      It is here in this dialog box that we define a part. We give the part a name,
      assign it a symbol and a footprint. This dialog box is very important. With the
      entries of this dialog box Logic Creator, Symbol Creator, and Board Creator
      can harmoniously work together allowing us to easily produce perfect
      schematics and printed circuit board artwork. Browse through it for now. Do
      not make any changes. We will come back to it later on and create or modify
      parts. Take notice of the contents of the Symbols box. It contains the name of
      the graphic symbol of this part. It is called mosfet_n, and it is stored in the
      same library, device.lbp. Press the cancel button to return to the opening
      screen.
                                                                             139




                   Figure 8-3: Open Entry Dialog Box.

Looking at a Symbol Definition
    How about the symbol definition of the same part? Ok, Click on the Symbol
    menu. Even though the device library was earlier selected under the Part menu,
    we have to select it again and make it active under the Symbol menu. So, click
    on Select Library. The Select Symbol Library dialog box pops up. Select the
    device.lbp library, and the Open Entry dialog box pops up as shown below.

    Scroll down and select mosfet_n.sym. Press Ok, and bingo, the edit screen
    shows the graphic symbol of the part on the left and on the right you have the
    text description of the symbol.
140




                Figure 8-5: Graphic Symbol of Mosfet_n.sym

      Press Ctrl + PgUp to enlarge the graphic symbol, and Ctrl + PgDn to reduce it.
      Move the mouse pointer inside the graphic area and notice the coordinates of
      the cursor on the right hand side of the status bar. The dimensions in Symbol
      Creator are in mils, thousandths of an inch. The right hand side of the edit
      screen contains commands on the Symbol Creator language that are used to
      create the graphic image on the left. Click on the command Moveto 300 150.
      The command is highlighted and a little x is also highlighted marking the
      location (300,150) on the graphic area. Next click on the command Side Left.
      The line (Pin 1) connecting the gate of the mosfet is highlighted. Again do not
      change anything. We are just taking a tour of Symbol Creator. To end the tour
      click on File and then Exit.

      Before we are ready to create new symbols or modify existing ones let's take
      another closer look at parts, symbols and libraries.
                                                                                 141

Parts, Symbols, and Libraries
    This section presents a general discussion of schematic parts, symbols,
    libraries, and how they work with the Logic Creator schematic system.

    An electrical schematic is a drawing that logically represents an electrical
    circuit. A drawing consists of symbols which represent electrical parts, and
    lines which represent how the parts are connected together. When schematics
    are drawn using computer programs, such as Logic Creator, it is not necessary
    to draw the symbols on the schematic sheet. The symbols for standard
    electrical parts are stored in a computer file called a library. The user simply
    indicates the occurrence of a part and the symbol to be used, and it appears on
    the schematic sheet. The schematic is then wired by drawing lines that connect
    the pins of the part symbols together.

    This has proven to be a very efficient and accurate way of capturing electrical
    design in computer form. It is only necessary to define a part, and the symbols
    that are used to represent the part, once. The same part and symbol definition
    may be called up from its library whenever it is used in a design. If proper care
    and testing are done when the part and symbols are created, this reliability can
    be passed on to every design that uses this part.

    What is the difference between a part and a symbol? A part specifies a physical
    electrical part, or section/gate of it. For example, the integrated circuit part
    7400 is an exact physical electrical part that consists of four Nand gates. A
    symbol is the graphic that is used to represent the part. In the case of the 7400,
    its symbol will only represent one gate of the part. For each four symbols of
    this part that are placed on a schematic, only one physical 7400 part is required
    in the design.

    A part may be represented by more than one symbol. However, no matter how
    many different symbols are used to represent a single part, the part is still a
    unique part. Representing a part by different symbols is a matter of
    convenience for the designer, and helps convey his design ideas into the
    appearance of the schematic drawing.
142

      A single symbol may be used to represent different parts. For example, the S00
      symbol is one of the symbols that is used to represent one gate of the 7400
      part. This symbol may be used to represent any part that is a 2 input Nand gate,
      such as the 74LS00, 74F00, etc. This concept is very efficient, since it is only
      necessary to have one symbol that can represent any part that is a two input
      Nand gate.

      How does this all fit together? When a user adds a part to a schematic, he is
      really adding an occurrence of the part to the schematic. The occurrence
      specifies the name of the part and the name of the symbol that is to represent
      the part. Internally, the schematic contains a single copy of the part definition
      and the symbol definition, regardless of how many times the part or symbol
      appears in a single design. It is these part and symbol definitions that are stored
      in the libraries, and are created and maintained by the Symbol Creator
      program.

Printing a Listing of the Parts of a Library
      Here is how you can make a hard copy of the parts contained in one library.




                           Figure 8-6: The Part Menu
                                                                             143

Pull down the Part menu as shown in figure 8-6. Notice that the Print
command at the bottom of the menu is grayed out, meaning that it can not be
used at this time. The reason is that no library has been selected yet.

Let’s print the Caps.lbp library which no so big. Click on Select Library ..., and
select the capacitor library: Caps.lbp. Now pull down the Part menu again, and
you will see that the Print command now is not grayed out. Click on Print and
the following menu will appear as shown in figure 8-6. The destination field is
prn, which mean the printer you have connected to your computer.

The Entry/Mask field is *.prt, which forces all the parts to be printed.
Remember that all part names have the extension “prt” and all symbol names
the extension “sym”. The Directory option is selected as a default. This will
print all the parts of this library. Now go ahead and click on the OK button if
you want the library listing to be printed. The printout should look like the
following one.




                  Figure 8-7: The Part:Print menu
144

      Library: C:\Cktcrt\Caps.lbp
      Mask: *.prt

       1: .001uf.prt         31: .1uf.prt     61: 2200uf.prt
       2: .0001uf.prt        32: .22pf.prt    62: 220pf.prt
       3: .00047uf.prt       33: .22uf.prt    63: 220uf.prt
       4: .0015pf.prt        34: .27pf.prt    64: 22pf.prt
       5: .0015uf.prt        35: .27uf.prt    65: 22uf.prt
       6: .001pf.prt         36: .33pf.prt    66: 2700pf.prt
       7: .001uf.prt         37: .33uf.prt    67: 2700uf.prt
       8: .0022pf.prt        38: .47pf.prt    68: 270pf.prt
       9: .0022uf.prt        39: .47uf.prt    69: 270uf.prt
      10: .0027pf.prt        40: 1.5pf.prt    70: 27pf.prt
      11: .0027uf.prt        41: 1.5uf.prt    71: 27uf.prt
      12: .0033pf.prt        42: 1000pf.prt   72: 3.3pf.prt
      13: .0033uf.prt        43: 1000uf.prt   73: 3.3uf.prt
      14: .0047pf.prt        44: 100pf.prt    74:.0001pf.prt
      15: .0047uf.prt        45: 100uf.prt    75: 3300pf.prt
      16: .015pf.prt         46: 10pf.prt     76: 3300uf.prt
      17: .015uf.prt         47: 10uf.prt     77: 330pf.prt
      18: .01pf.prt          48: 1500pf.prt   78: 330uf.prt
      19: .01uf.prt          49: 1500uf.prt   79: 33pf.prt
      20: .022pf.prt         50: 150pf.prt    80: 33uf.prt
      21: .022uf.prt         51: 150uf.prt    81: 3900pf.prt
      22: .027pf.prt         52: 15pf.prt     82: 4.7pf.prt
      23: .027uf.prt         53: 15uf.prt     83: 4.7uf.prt
      24: .033pf.prt         54: 1pf.prt      84: 4700pf.prt
      25: .033uf.prt         55: 1uf.prt      85: 4700uf.prt
      26: .047pf.prt         56: 2.2pf.prt    86: 470pf.prt
      27: .047uf.prt         57: 2.2uf.prt    87: 470uf.prt
      28: .15pf.prt          58: 2.7pf.prt    88: 47pf.prt
      29: .15uf.prt          59: 2.7uf.prt    89: 47uf.prtb
      30: .1pf.prt           60: 2200pf.prt   90: 560pf.prt
                                                                                145

    As you see these listings can be quite long. This library contains only 90 parts.
    The Motorola library contains 4,250, the Anolog1 1,723, and many other
    libraries are quite large. Please be aware of this so that you wisely decide who
    and how many copies to make. Here is something you may want to do to
    minimize the volume of paper needed to print all libraries. In the destination
    field you can specify a file to which you want the list to be printed. For
    example the above listing was saved as caps_lbp.doc, and the was imported
    into this document. The caps_lbp.doc is an ASCII file and can easily be
    imported and manipulated in most word processors. You can format the your
    word processor page in five or six columns and use a small size font (8 points
    for example). Then you will need five or six times less pages than you would
    need if you print the caps_lbp.doc from Dos.

Symbol Creator Menus
    The following information is a listing of all menus and their commands. Read
    through them and refer to these pages whenever you have a question.

File Menu (Alt + F)
    The file menu provides commands for displaying program version information,
    exiting the program, and executing Dos commands.




                             Figure 8-8: The File Menu

Preferences (Alt + F & P)
    The system menu provides commands for changing the configuration of the
    Symbol Creator system.

    The user configuration settings are stored in the file sc32.cfg. This file must
    reside in the same directory as the sc32p.exe program. The settings in this file
    are initially set during installation. The commands on this menu may be used
146

      to change these settings. The file is an ASCII text file. Although not
      recommended, the file may be directly edited with a text editor.




                        Figure 8-9: File/Preferance Dialog-box

Paths/Options
      Changes to the configuration are saved when the program is exited. Some may
      not take effect until the program is exited and restarted. Paths/Options use this
      command to configure the default file paths other operating options for the
      Symbol Creator program:




                        Figure 8-10: Paths/Options Dialog box

      Drawings Path:
      The path to where your library files (*.lbs & *.lbp) are located is entered in the
      above dialog box. This path name is entered in the Drawings Path field and
                                                                            147

must be terminated with a backslash This will be the default directory that is
searched for any existing schematic files.

Scratch Path:
When objects are cut or copied on the schematic, their image is stored in a
temporary file (paste.$$$) called the paste buffer. The path to where this
temporary file is written is determined in the Scratch Path field in the above
dialog box and must be terminated with a backslash (/).

Chaeck Point Path:
The Symbol Creator program has an auto-backup (or timed-backup) feature
that will periodically save the current schematic to a check-point file (.ckp) in
case of a power loss. The path to where this file is saved is determined in the
Check-Point Path field of the Paths/Options dialog box and must also be
terminated with a backslash (\). When the Symbol Creator program is
re-started after the occurrence of a power loss and you re-open your schematic
design, this path is searched for the existence of a back-up file.

Banner:
The name entered in the Banner field of the Paths/Options dialog box will
appear in any report generated The default banner is "Your Name Here".

Memory Blocks:
The amount of time that passes before the schematic is automatically saved is
determined in the Check-Point Seconds field. The number entered here is in
seconds. For example, in the above Paths/Options dialog box, the value 300 is
entered. This will back-up the schematic design every five minutes. To disable
this feature, enter a zero (0) in the Check-Point Seconds field. The maximum
value that may be entered here is 3600 (or one hour). For more information
about this auto-backup feature, refer to the section "A Check-point File
Exists".

Maxi Pins:
The maximum number of pins to be expected in your schematic design is
entered in the Max Pins field. The value entered here is also used in
148

      determining the amount of memory that is allocated for your design. For more
      information concerning the configuration of memory for Logic Creator.

      Chaeck Point Seconds:
      The amount of time that passes before the schematic is automatically saved is
      determined in the Check-Point Seconds field. The number entered here is in
      seconds. For example, in the above Paths/Options dialog box, the value 300 is
      entered. This will back-up the schematic design every five minutes. To disable
      this feature, enter a zero (0) in the Check-Point Seconds field. The maximum
      value that may be entered here is 3600 (or one hour). For more information
      about this auto-backup feature, refer to the section "A Check-point File
      Exists".

      Pan on Edge Bump:
      Use this command for pan sheet all the way without using pan command when
      this command is enable you can pan automatically same direction you have
      touch the edge of this direction.

      For Expample: When you touch the upper side edge of the edit window the
      program autoamatically shift upper side.

      Ground Net Symbols:
      Finally, with the Ground Net Symbols option enabled, any wire or pin of a
      component that is assigned with the net names: GND, GNDA, or GNDC will
      appear with the appropriate graphic symbol for the ground net. When this
      option is disabled, the ground net name will be spelled out on your schematic
      (instead of displaying the ground symbol).

Libraries
      Use this command to configure the part libraries that you want to appear on the
      library menu, and the symbol libraries to use. You must enter the full path
      name for each configured library, the text you want to appear on the library
      menu, and the type of library.

      Although the symbol libraries will not appear on the menu, they will be used
      when a part references a symbol to locate the definition of that symbol.
                                                                           149




               Figure 8-11: Confiured Libraries Dialog-box

Drawing Colors/Widths
    Use the command to configure the display colors and the drawing line widths
    for objects on a schematic.




                Figure 8-12: Colors/Widths Pop-up Menu
150

Application Colors
      Use this command to configure the colors for the Symbol Creator windows,
      such as the color of the rulers, status line, etc.

      Note: Symbol Creator like all other windows applications uses the windows
      system colors for menus, dialog-box windows, borders, etc. If you want to
      change these colors, from the windows main program group, double click on
      the Control Panel icon, and then double click on the Color icon. You can now
      change the system colors. Use windows context sensitive help if needed.

      Caution: While selecting the color, make sure you don’t select the same color
      for background and foreground.




                Figure 8-13: Application Colors Pop-up Menu

Exit (Alt + X or X)
      Use this command to exit the program. If changes have been made to the
      current symbol and not saved, you will be given the option of saving the
      symbol before exiting.
                                                                               151

Part Menu (Alt + P)
     The part menu provides commands for creating new part libraries, viewing and
     editing part definitions, creating new parts, deleting parts, and printing part
     directories and definitions
     .




                         Figure 6-14: The Part Menu

Create Library (Alt + P & C)
     Use this command to create a new part library. A dialog-box will appear,
     allowing you to specify the path and file name of the new part library. Enter
     the name and press the Ok button to create the library.




                Figure 8-15: Creator Part Library Dialog-box
152

Select Library (Alt + P & S)
      Use this command to select the part library you want to work with. This is
      referred to as the current part library. Once selected, you can view, edit, print,
      or add new part definitions to the library. Only one part library is selected at a
      time. The name of the part library will appear in the program title line when
      you execute any of the part commands.




                  Figure 8-16: Select Part Library Dialog-box

Open (Alt + P & O)
      Use this command to view or edit a part definition in the current part library.

      A dialog-box will appear, allowing you to pick the name of the part you want
      to open. Type the part name, or select it from the list of names shown in the
      dialog box. Press Ok to view or edit the part. A new dialog-box will appear,
      showing the current definition of the part. Each of the fields that define a part
      are discussed in detail in the Parts section of this chapter. Edit the definition as
      required, and press Ok to accept the changes. When you press Ok, the previous
      definition of the part in the current part library is replaced with the new
      definition.
                                                                                 153




                      Figure 8-17: Part Open Entry Dialog-box

New (Alt + P & N)




                       Figure 8-18: Part New entry Dialog-box

     Use this command to create the definition of a new part and add it to the
     currently selected part library. A dialog-box will appear, showing the fields for
154

      this new part. Each of the fields that define a part are discussed in detail in the
      Parts section of this chapter. Enter appropriate values into each of the fields.
      Press Ok to save the new part definition in the current part library.

Delete (Alt + P & D)
      Use this command to delete the definition of a part from the currently selected
      part library. A dialog-box will appear, allowing you to specify the name of the
      part entry to be deleted. Type the name of the part, or select it from the list.
      Press Ok to delete the part. Before the part is actually deleted, you will be
      required to confirm that this is the part you want to delete.




                       Figure 8-19: Part Delete Entry Dialog-box

Print (Alt + P & P)




                       Figure 8-20: Part Print Dialog-box
                                                                                  155

     Use this command to print either a directory of the parts in the current part
     library, or the definition of parts contained in the library. A dialog-box will
     appear, allowing you to specify the destination of the report, type of the report,
     and the part name mask. The mask may be the name of a single part, or it may
     contain the "*" wild card character. For example, a mask of "*.*" will print all
     the parts in the current library.

Symbol Menu (Alt + S)
     The symbol menu provides commands for creating new symbol libraries,
     viewing and editing symbol definitions, creating new symbols, deleting
     symbols, and printing symbol directories and definitions.




                        Figure 8-21: The Symbol Menu

Create Library (Alt + S & C)
      Use this command to create a new symbol library. A dialog-box will appear,
     allowing you to specify the path and file name of the new symbol library. Enter
     the name. Press the Ok button to create the library.
156




               Figure 8-21: Create Symbol Library Dialog-box

Select Library (Alt + S & S)
      Use this command to select the symbol library you want to work with.

      This is referred to as the current symbol library. Once selected, you can view,
      edit, print, or add new symbol definitions to the library. Only one symbol
      library is selected at a time. The name of the symbol library will appear in the
      program title line when you execute any of the symbol commands.




                Figure 8-21: Select Symbol Library Dialog-box
                                                                           157

Open (Alt + S & O)
     Use this command to view or edit a symbol definition in the current symbol
     library.




                  Figure 8-22: Symbol Open Dialog-box




                   Figure 8-23: Opened Symbol window
158

      A dialog-box will appear, allowing you to pick the name of the symbol you
      want to open. Type the symbol name, or select it from the list of names shown
      in the dialog box. Press Ok to display the symbol definition.

      Once opened, the symbol definition may be edited by deleting, inserting, or
      changing the text lines shown the right edit window. The left window will also
      be redisplayed to reflect any changes in the definition of the symbol. Change
      the symbol as required. Use the Save or Save As commands on the Symbol
      Menu to put the symbol into the current symbol library.

New (Alt + S & N)
      Use this command to create the definition of a new symbol.

      A dialog-box will appear, allowing you to specify name of the new symbol and
      whether or not it is a standard box type symbol.




                 Figure 8-23: Create New Symbol Dialog-box

      If you specify that it is a box type symbol, specify the number of pins on each
      side of the symbol. The program will generate the specified number of pins
      and place them along the indicated sides of the symbol. It will also make the
                                                                              159

     basic box shape of the symbol. All you need to do to complete the symbol is
     select each pin and set its parameters to the actual values (pin number, I/O
     type, graphic symbols, etc.)

     If you do not specify a box type symbol, you will have to add the symbol
     statements to define the graphic of the symbol and the symbol pins. Define the
     symbol as required. Use the Save or Save As commands on the Symbol menu
     to put the symbol into the current symbol library.

Delete (Alt + S & D)
     Use this command to delete the definition of a symbol from the current symbol
     library.




                      Figure 8-24: Symbol Delete Dialog-box

     A dialog-box will appear, allowing you to specify the name of the symbol
     entry to be deleted. Type the name of the symbol, or select it from the list.
     Press Ok to delete the symbol. Before the symbol is actually deleted, you will
     be required to confirm that this is the symbol you want to delete.

Save (Alt + S & S)
     Use this command to save the symbol that is displayed to the current symbol
     library. Any previous definition of this symbol is replaced.
160

Save As (Alt + S & A)
      Use this command to save the symbol that is displayed to the current symbol
      library under a new symbol name. A dialog-box will appear, allowing you to
      specify the new symbol name. Enter the name and press Ok to save the
      symbol.




                   Figure 8-25: Symbol Save As Dialog-box

Print (Alt + S & P)
      Use this command to print either a directory of the symbols in the current
      symbol library, or to print the definitions of symbols contained in the library.




                   Figure 8-26: Printing Symbol Dialog-box
                                                                                     161

    A dialog-box will appear, allowing you to specify the destination of the report,
    type of the report, and the symbol name mask. The mask may be the name of a
    single symbol, or it may contain the "*" wild card character.

    For example, a mask of "*.*" will list all the symbols in the current library.

Edit Menu (Alt + E)
    The commands on this menu are used during the creation and editing of
    symbols.




                         Figure 8-27: The Edit Menu
Undo (F2)
    Use this command to undo the last editing change that was made to the current
    symbol.
162

Insert (Ctrl + Enter)




                   Figure 8-28: Insert Command Dialog-box

      Use this command to insert a new statement into the definition of the current
      symbol. The current position in the text window is indicated by the statement
      line that is highlighted. When a statement is inserted, it is inserted before the
      highlighted line.

      A dialog-box will appear, allowing you to type in the new statement. The
      dialog-box contains a list-box, showing the format of all the possible symbol
      statements. Selecting one of the statements from the list will copy the
      statement format to the command line. Replace the command arguments, if
      any, with appropriate values for your symbol.

      Press Ok to insert the new statement. Both of the symbol definition windows
      will be updated to reflect the impact of the new statement.

      When you insert an Io pin statement, the Io and its corresponding End
      statement will be inserted for you. To complete the Io definition, move the
      cursor to the Io statement line and press the Enter key. A dialog-box will
      appear, allowing you to specify all the parameters associated with the pin.
                                                                                  163

Delete (Del)
     This command is used to delete the current symbol definition statement,
     indicated by the highlighted line. The Symbol and End statements cannot be
     deleted. Also, if you delete an Io statement, the entire Io pin definition will be
     deleted for that pin.

Edit Current Statement (Enter)
     To edit the current symbol definition line (highlighted), just press the Enter
     key. You can also point to a line with the mouse and click the left mouse
     button to edit the line.

     If the current line belongs to an Io pin definition, a dialog-box will appear,
     allowing you to edit all of the parameters associated with that I/O pin. You do
     not have to edit the individual lines of an I/O pin as shown in the text window.




                   Figure 8-29: Edit Command Dialog-box

View Menu (Alt + V)
     The view menu provides commands for selecting the current view of the
     symbol being displayed or edited. You may pan or zoom the view.
164




                         Figure 8-30: The View Menu

      In addition to the commands that are directly on the menu, the view can also be
      changed with the mouse. To pan with the mouse, use the slide-bars along the
      right and bottom edges of the window to select a desired view. Clicking the
      mouse on the slide-bar arrows will pan a small amount in that direction.
      Clicking in the area between the arrows and the slider will pan a full page.
      Grab the slider with the mouse and drag it to select the view directly. The size
      of the slider indicates the portion of the symbol or text that is currently
      displayed.

Section (Alt + V & S)
      Use this command to select the section of the current symbol that is to be
      viewed. The pin numbers that appear on each pin of the symbol are the pin
      numbers defined for the current symbol section being viewed. Changing to
      another section of the symbol will display the symbol with the pin numbers
      defined for that section. This command is very useful for verifying that the pin
      numbers assigned to each section of a symbol are correct.
                                                                              165




                       Figure 8-31: View Section Dialog-box

Pan Up (PgUp)
     Use this command to pan the symbol display up. The pan direction refers to the
     change in the view, not the direction that the symbol appears to move. For
     example, panning up indicates that you want to view more of the area toward
     the top edge of the symbol.

Pan Down (PgDn)
     Use this command to pan the symbol view down.

Pan Right (Shift + >)
     Use this command to pan the symbol view right.
Pan Left (Shift + <)
     Use this command to pan the symbol view left.

Zoom Home (Ctrl + Home)
     Use this command to view the upper-left corner of the symbol at the standard
     zoom scale.

Zoom In (Ctrl + PgUp)
     Use this command to zoom in on the symbol view. Objects in the view will
     appear bigger and more detailed; however, you will be able to see less area of
     the symbol.
166

Zoom Out (Ctrl + PgDn)
      Use this command to zoom out on the symbol view. Objects in the view will
      appear smaller and less detailed; however, you will be able to see more area of
      the symbol.

Redraw (Ctrl + R)
      Use this command to redraw the symbol at its current pan and zoom scale.

Help Menu (Alt + H)
      This menu allows you to get on-line help on any command or menu. It is
      organized like a book, with an index of the chapters and detailed information
      in each chapter.




                             Figure 8-32: The Help Menu

Context/Index (F1)
      This option gives you the index of the help manual. Move your mouse pointer
      above the word you need help on. If the arrow changes to a pointing hand then
      help is available, and you can access it by clicking on that word.

      This is the most important feature of the Help menu. It allows you to get direct
      help on the specific command you are interested by highlighting the command
      and then pressing F1.
                                                                             167




                Figure 8-33: Context/Index Help Dialog-box

Using Help (Alt + H and U)
     This is a tutorial on how to use the help menu of Logic Creator. Please go
     through this tutorial as many times as you need. It will help you became a
     better user.

About Symbol Creator (H)
     Use this command is display the copyright notice and current version/release
     number of the program.




                          Figure 8-34: About Dialog-box
168
                                                                                  169



Chapter 9
Creating a Part and its Symbol
Introduction
In this Chapter you will get actual hands-on experience in making parts and symbols.
You will be guided through the creation of a part and its symbol. The part and symbol
are put in an Logic Creator library, then placed on a schematic sheet. Although this is
a simple part, it demonstrates the ease with which any part or symbol may be created
for use on your schematics.

Parts
       In this portion of the Chapter you will learn how to:

              •   Part Definitions.
              •   Create a Part Library
              •   Creating a Part
              •   Edit Existing Part

Part Definitions
       All parts used with the Logic Creator schematic system are stored in part
       libraries. A part library is just a Dos file which contains the part information
       for many different parts. Before we can look at the values assigned with a part,
       we must first indicate the library that contains the part.
170




                             Figure 9-1: Select Part Library

      Pull-down the Part Menu and execute the Select Library command. A dialog-
      box will appear, showing the names of the part libraries that are configured for
      you system. Select the first library shown in the list and press the Ok button.

      This library is our current part library. We can now perform any of the
      commands associated with parts. Execute the Open command on the Part
      Menu. A dialog-box will appear, showing a list of all the parts contained in this
      library. Select the first part name shown and press the Ok button. A new
      dialog-box will appear, showing all the values assigned to this part. To become
      familiar with what constitutes a part, briefly study the field names and the field
      values.
                                                                             171




                        Figure 9-2: Part Open

This is all that is required to look-up a part definition. Press the Cancel button
to exit this part. Now, lets look-up another part. Once again, execute the
Part/Open command. Scan through the list of part names, and select one that
appears of interest to you. Press the OK button to display the part definition.
Observe the part, the press Cancel to close the dialog-box.




                     Figure 9-3: Part Definitions
172

Creating a Part Library
      Now we will create a new part library. Execute the Create Library command
      on the Part Menu. A dialog-box will appear, asking you for the file name of the
      new library. Enter "Test" and press Ok. We have just created a new part
      library. The name of the library file is "Test.lbp"




                   Figure 9-4: Creating “TEST” Part Library

Creating a Part
      The new part library that we just created is empty. That is, it does not currently
      have any parts in it. We will now make a new part and put it in our library. The
      actual part and symbol used for the tutorial Chapters is the "7474 Dual D-type
      Flop-Flop"; however, for the purposes of this tutorial, we will use another
      name (we don't want to confuse it with the real 7474 part in another library).

      Execute the New command on the Part menu. Now, the part dialog-box is
      shown just as when we were viewing a part. However, this time it is up to us to
      enter all the values for the new part. Enter the following values in the dialog-
      box fields. Leave the library field as is, and all the other fields not mentioned
      here blank.
                                                                                  173




                   Figure 9-5: Creating New “TEST” Part

    Now, press the Ok button. This part definition is now stored in the "TEST"
    library under the name "Testpart". That's all there is to creating new parts.

Edit a Existing Part
    Now, let's make a change to the part that we just created. Execute the
    Part/Open command. Select the "Testpart" entry and press Ok. Now, our part
    will reappear in the dialog-box. Change the description field to "Test part from
    tutorial Chapter". Press the Ok button. This is all that is required to make
    changes to existing part definitions. In actual practice, always remember that
    before you can edit an existing part, you must select the part library that
    contains the part. If the part you want is not in the current part library, use the
    Part/Select Library command to select the library.
174




      Figure 9-6: Open “testpart.prt” part




      Figure 9-7: Edit “testpart.prt” Part
                                                                             175

Symbols
    In this portion of the Chapter you will learn how to:

           •   View Symbol Definitions.
           •   Create New Symbol.
           •   Edit Existing Symbol.

View Symbol Definitions
    All symbols used with the Logic Creator schematic system are stored in part or
    symbol libraries. A library is just a Dos file which contains the symbol
    definitions. Before we can look at a symbol definition, we must first indicate
    the library that contains the symbol.

    Pull-down the Symbol Menu and execute the Select Library command. A
    dialog-box will appear, showing the names of the part libraries that are
    configured for your system. Select the "Symbol.lbs" library shown in the list
    and press the Ok button.




                     Figure 9-8: Select Symbol Library
176

      This library is our current symbol library. We can now perform any of the
      commands associated with symbols. Execute the Open command on the
      Symbol menu. A dialog-box will appear, showing a list of all the symbols
      contained in this library. Select the first symbol name shown and press the Ok
      button. The definition of this symbol will now appear on the screen. The
      graphic representation of the symbol appears in the left window. The text
      representation of the symbol appears in the right window.

      This is all that is required to look-up a symbol definition. Now, let's look-up
      another symbol. Once again, execute the Symbol/Open command. Scan
      through the list of symbol names, and select one that appears of interest to you.
      Press the Ok button to display the symbol definition. Use the up and down
      arrow keys to move the line that is highlighted in the text window. As the
      highlight bars moves, notice that the corresponding object shown in the
      graphic window is also highlighted.

Creating a New Symbol
      Execute the New command on the Symbol Menu. A dialog-box will appear,
      allowing you to specify the name of the symbol, and the option to make the
      initial shape and pins for a standard box type symbol. Set the following values
      in the dialog fields:




                         Figure 9-9: Open New Symbol
                                                                             177

Press the Ok button to begin this symbol. The box shape of this symbol, and
the number and location of the specified I/O pins have been generated for us.
What we need to do to complete the symbol is to set the number of sections,
set the true pin numbers for each, and add any other graphics or pin attributes
that may be required. Execute the View/Zoom In command to make the
symbol display larger.




                    Figure 9-10: Symbol Zoom In

We want this symbol to be able to represent two different sections of a part.
Use the      and      arrow keys to move the position indicator in the text
window. The current position is the line that is highlighted. Position to the line
that contains "Section 1" line and press the Enter key. You may also position
with the mouse, and select by clicking the left mouse button. This is the
178

      symbol statement dialog-box. Change the value 1 in this line to 2, and press the
      Ok button. Notice that the line in the text window reflects the change.




                            Figure 9-11: Symbol Edit

      Next, we will adjust the value of each I/O pin to its true pin number and I/O
      type. Move the text position indicator to the first "Io" statement, and press the
      Enter key. In the case of an Io pin, a special dialog-box will pop-up, allowing
      you to edit all the parameters associated with the pin at the same time. For this
      pin, set the following fields to these values. Leave all other fields as they are
      and press OK.

      Since this symbol has two sections, we must assign a pin number for each
      section (or gate). This is pin two for section one of the part, and pin twelve for
                                                                             179

section two of the part. Notice the change to both the text window and the
graphic representation of this pin.




                         Edit Upper Left Pin

Now, move down to the next Io pin and Enter. For this pin set the following
field values:




                         Edit Lower Left Pin

Using this same procedure, set the remaining pins to the following values.
180




                    Edit Upper Right Pin




      Edit Lower Right Pin (~ Will Show Bar Over Text)




                     Edit Top Side Pin
                                                                           181




                        Edit Bottom Side Pin

The @Instance and @Part fields represent where the reference number and the
part number will appear when the symbol is used on a schematic. Let's move
them to better locations. Use the PgUp key until the top line of the text window
is displayed. Move the position pointer to the statement Moveto 800,420 which
is just above the @Instance statement. This statement sets the position for the
instance location. Enter and change this statement to Moveto 1200,200. Now,
change the Moveto 800,870 statement that is just above the @Part statement to
Moveto 1200,1100.




                               Section 1 View

To check that the pin numbers have been assigned correctly, look at each pin in
the graphic display. Does it have the correct pin number for section one of the
182

      part? Now, execute the View/Section command. Enter 2 for the section
      number, and press Ok. The display will change to show the pin numbers
      assigned to section two of the part.




                                    Section 2 View

      This completes this symbol. Execute the Save command on the Symbol Menu
      to Save this symbol to the symbol library.

Editing a Symbol
      To learn how to edit an existing symbol, we will modify one of the pins of the
      symbol we just created. Execute the Open command on the Symbol Menu.
      When prompted for the symbol name, enter "Testsym" and press Ok. Now we
      have retrieved the symbol from the library, and it is displayed on the screen.
                                                                          183




                             Symbol Edit Wiew

Position to the Io statement for the pin labeled "CK", and Enter. Set the SymIn
field value to Dynamic. Notice that the IEEE symbol for a dynamic input is
now shown for this pin.
184




                                   Edit SymIn Dynamic

      Execute the Save command from the Symbol Menu. We have now changed an
      existing symbol, and put the new version of the symbol back into the symbol
      library.

Testing
      In this Chapter we will test the part and symbol that was created in the
      previous Chapters.

      Exit the Symbol Creator program and run the Logic Creator program. Execute
      the File/New command. Press Ok to accept the drawing set-up parameters.

      Now, we have a new schematic to test our part and symbol. Execute the
      Library/Add Part by Library command. This will allow us to select our new
      part library without configuring into the list of the high-use libraries. Enter
      "Test" for the library name and press Ok.

      Now the list of entries in this library are shown. Our test part is the only entry
      in this library. Select the part "Testpart, and press Ok.

      Now, the symbol for our new part should appear on the cursor. Move the
      cursor to location (2.000,1.000) and Enter to add section one of this part to the
      schematic. Move to (4.000,1.000) and Enter to add section two of this part. Esc
      to end the command.
                                                                              185

   Zoom in and look at each of the part occurrences closely. Verify the following:

   •   Does the symbol look like the symbol that was specified in the part?
   •   Does the reference number show the prefix, U, as specified in the symbol?
   •   Does each pin show the correct pin number? Check both part sections.
   •   Can you draw a wire that connects exactly to each of the pins?
   •   Generate a net list for this schematic. Does it show the proper net names on
       the power pins (7=GND, 14=+5V)?
   •   Generate a part list report for this schematic. Does it show the proper
       information that you expect from this part?

   If the part or symbol fails any of these tests, try to correct the problem by
   editing the part and/or symbol. Re-test until there are no problems.

What is a Hierarchy Design?
   A hierarchy design is used when you have more than one schematic file that is
   to be used for a single design (or when you need more than the thirty-two
   sheets that are available on a schematic). This can also be useful when there is
   more than one engineer working on a design. For example, each engineer can
   edit and maintain his or her own schematic file. When everyone has completed
   the work, the overall design can be linked together by one main schematic.

   Special components must be created using the Part/Symbol editor (Symbol
   Creator) that represent each schematic used in the hierarchy design. These
   components are then placed on one main schematic. When reports are
   generated against this schematic (such as bill of materials, net list, pin list,
   etc.), all of the schematic files used in the design will be linked together.

Creating a Hierarchy Component
   Let's create a hierarchy component that represents the schematic demo.sch. We
   must first start-up the library Part/Symbol editor (Symbol Creator). To do this,
   double click on the Symbol Creator icon located in the Circuit Creator group.
   We will be creating the hierarchy part and symbol and storing them both in the
   Logic Creator library Misc.lbp.
186

      After starting Symbol Creator, pull down the Part Menu and choose the Select
      Library command and the following dialog box will appear:




               Figure 9-12: The Select Part Library Dialog Box.

      Select the library Misc.lbp from the Select Part Library dialog box and point at
      the Ok button with the mouse and click the left mouse button (or press the key
      combination Alt plus the letter O) to accept this library.

      Pull down the Part Menu again and select New and the following dialog box
      will appear allowing you to enter the definition for this new part that we are
      creating. Fill-in the options as it are shown in the following dialog box.
                                                                              187




       Figure 9-13: Hierarchy Part Description Dialog Box.

The section in the above dialog box that separates a hierarchy part from all of
the other parts in the library is the Link to field. The complete path for the
schematic (that this hierarchy part is to represent) must be entered in the Link
to field. After all of the items have been entered for this new part, press the Ok,
Save button to accept this new part definition.

Note: You must have 1 pin entered in the Max Pin# field when defining a
hierarchy part.

Now we will create the hierarchy symbol. The name given to this symbol must
match the name entered in the Symbols field of the New Part dialog box
188

      (Figure 9-13). Choose the Select Library command from the Symbol pull down
      menu and the following dialog box will appear:




               Figure 9-14: Select Symbol Library Dialog Box.

      Choose the same library (Misc.lbp) as you did when we created the hierarchy
      part and press the Ok button to accept this library.

      Note: You may create both the part and symbol definitions in the same library
      file. In fact, this is highly recommended. A part definition will be stored with a
      .prt extension in the library and a symbol is stored with a sym extension. More
      information about creating new parts and symbols will be presented in the
      Symbol Creator section of this manual.

      Pull down the Symbol menu once more and select New and the following
      dialog box will appear:
                                                                           189




            Figure 9-15: The New Symbol Dialog Box.

The Name for this new symbol will be hierarch. Change the number of Pins
Left and Pins Right to zero (0) and press the Ok button to accept these options.
The following symbol will appear on the left hand side of the screen and the
description for this symbol will appear on the right.




Save this symbol by selecting Save from the Symbol pull down menu. We are
now ready to demonstrate how to use this new part and symbol in a hierarchy
design. Select Exit from the File pull down menu in Symbol Creator and start-
up the Logic Creator schematic editor. Select New from the File pull down
menu in Logic Creator and press the Ok button in the Format: New dialog box
to accept the default values for this new schematic. This will be our main
schematic where all of the hierarchy parts will be placed. Note: For our
example, we only have one hierarchy part. From the Library Menu select Add
Part by Library and select the library Misc.lbp in the following dialog box:
190




              Figure 9-16: The Add Part by Library Dialog Box.

      Select the hierarchy part demo.prt (that was just created using the library
      Part/Symbol editor) from the list of parts in the Misc.lbp library and place it
      anywhere on this new schematic. This part represents the schematic demo.sch.
      Press the right mouse button or the ESC key to cancel placing another part on
      the schematic.

      Next, choose the Select command from the Edit pull down menu (or press the
      letter S which is the hot key for the Select command). Select the hierarchy part
      by pointing at the part with the mouse and clicking the left mouse button (or
      move the cursor with the arrow keys so that it is touching the hierarchy part
      and press the Enter key twice), The hierarchy part will become highlighted
      showing you that it has been selected. Select the Hierarchy Push command
      from the File Menu and the schematic, demo.sch, will be automatically loaded.

      To return to the main schematic, select Hierarchy Pop from the File menu and
      the schematic containing the hierarchy part will be re-loaded. If there was
      another schematic that we wanted to link to our design, we would simply place
      its hierarchy part on the same main schematic. In order to view/edit the other
      schematic, you would simply select the other hierarchy part and use the
      Hierarchy Push command. All of the reports and net lists are generated while
                                                                       191

the main schematic (the schematic that contains the hierarchy parts) is the
current schematic displayed.
192
                                                                                         193



Chapter 10
Part and Symbol Reference Section
This is a reference section. It lists all the Symbol Creator menus and their commands.
A brief explanation follows each command with an example of its use if needed.

Read through this section to familiarize yourself with all the Symbol Creator
commands. Please refer to this section when you create new parts and symbols to
answer your questions. Between this section and the context sensitive help you should
be able to answer all of your questions.

Part Reference
Parts
       As described above, part definitions are used to represent a single physical
       electrical component used in the design of an electrical circuit. Parts do not
       directly contain the definition of the symbols that are used to represent the part,
       but only contain the names of the symbols that are allowed to represent the
       part.

       A part definition is made by supplying values for the following items or data
       fields. Unless indicated otherwise, the field is optional.

Library
       The library field is the path to the part library file that is used to hold this part.

       Example: Library: C:\CKTCRT\74.lbp

       The library name is used only for retrieving and storing parts. It is not saved
       within part definition or the library itself.
194

Name
       The part name is used to define the name of the part. Each part must have a
       name unique to its library. This name will be used when the part is stored or
       loaded from a part library.

       Example: Name: 7400

CORP #
       The corporate number field is used to hold the corporate part number for the
       part. This is a private part number, assigned by your own company. It is used
       in generating reports.

       Example: Corp #: 001-07400-03

Description
       The description field is used to provide a short description of the part. This
       description is used on the bill of material and other reports.

       Example: Description: Four input NAND gates

No. Pins
       The number of pins field is used to define the total number of pins on an
       electrical part. Please note! This is the total number of pins on the physical
       part. It may or may not be the same as the number of pins on the symbol used
       by the part, since the symbol may be only a portion of the part, and does not
       usually show the power and ground pins.

       Example: No. Pins: 14

Cost
       The cost field is used to assign a cost to the part. Enter the cost as a number.

       Example: Cost: 1.95
                                                                                  195

Footprint
     The footprint field is used to assign the name of the part footprint. This name is
     used in the PCB update list report as the name of the footprint symbol to use
     with this part when laying out the PCB board.

     Example: Footprint: DIP-14

Symbols
     The symbols field is used to assign the names of all the symbols that may be
     used to represent this part. List the symbol names separated by commas or
     blanks.

     Example: Symbols: SNAND2, SNAND2N

Power Pins
     The power pins field is used to assign pins of the part to a default power net.
     When the part is used on a schematic, the power pins are not usually shown on
     the part symbols. This allows the part to be properly powered, even though the
     power pins are never actually shown on the schematic. The net name will
     appear on the pins of this part in the reports generated from the schematic.

     Example: Power Pins: 7=GND, 14=+5V

Values
     The value fields are used to define up to five separate values associated with a
     part. They are used to define a value in the part which will be displayed when
     the part's symbol is drawn. The resistor symbol is a typical usage of a part
     value. Only one symbol is required to represent many different resistors. This
     is because the resistor value is stored in the part and passed on to the symbol.
     The symbol definition contains information about where the value is to be
     displayed, but the value itself comes from the part definition.

     Example: Value1: 100K
196

Link To
       This field is used in the definition of a hierarchical part to define the path to the
       schematic that is represented by this part. The link to value is the complete path
       name of the schematic file that is to be loaded when this part is pushed.

       Example: Link To: c:\CKTCRT\mydesign2.sch

       To use the hierarchical part feature on your schematics, you must have the
       "LOGIC CREATOR - Professional Edition" version of the product.

PKG Type
       This field is used to assign the part to a package type. This field is for future
       use and is not currently used by LOGIC CREATOR.

       Example: PKG Type: DIP

Type
       The type field is used to assign the part to a part type. This field is for future
       use and is not currently used by LOGIC CREATOR.

       Example: Type: IC

Family
       The family field is used to assign the part to a part family. This field is for
       future use and is not currently used by LOGIC CREATOR.

       Example: Family: 7400

Symbol Reference
Symbols are the graphic shapes that are used to represent parts on a schematic
drawing. A symbol definition is made up of some appropriate combination of the
following symbol statements or symbol commands. Do not be overwhelmed by the
number of possible symbol statements. There are many different statements that can
                                                                                    197

be used to define a symbol; however, a given symbol will usually only require a small
portion of the possible statements to actually be used.

Most symbols consist of the graphic of the body of the symbol, and the I/O pins used
to connect the symbol to other parts (on the schematic). Some special symbols contain
only graphics, such as the schematic sheet format symbols, which do not contain any
I/O pins.

The graphic of a symbol is made by including statements which describe how to draw
the lines and curves that make up the symbol shape. Commands are included to make
the drawing of standard box type symbols easy. The outline of the box may be drawn
with a single symbol command.

All symbol graphic coordinate values are in mils. One mil is 1/1000 of an inch (or
1000 mils equals one inch). The coordinate system origin is the upper-left corner of
the symbol area. The positive X axis is to the right. The positive Y axis is downward.

When you use the SYMBOL CREATOR program to define symbols, the screen will
be split into two windows, allowing you to always see the definition of the symbol as
it appears graphically in the left window, and the exact text definition of the symbol in
the right window.

You will not have to type in all these commands. In the case of box type symbols, the
initial symbol graphic and number of I/O pins will be generated for you. When you do
add a symbol statement directly, the text of the statement, and its arguments can be
picked from a list shown in the editing dialog-box.

The following section lists each symbol statement and describes its use:

@APPROVEDBY (Syntax: @APPROVEDBY)
    Use this statement to display the approved by schematic value. The text is left-
    justified about the current point. This statement is normally only used in the
    construction of sheet format symbols.

       For example:MOVETO 500,300
                   @APPROVEDBY
198


       will display the schematic approved by value at symbol location (500,300).

@BANNER (Syntax: @Banner)
    Use this statement to display the configured banner value (company name) on
    the symbol. The text for the banner is center-justified about the current point.
    This statement is normally only used in the construction of sheet format
    symbols.

       For example:MOVETO 500,300
                   @BANNER

       will display the schematic banner value at symbol location (500,300).

@DATE (Syntax: @DATE)
    Use this statement to display the system date on the symbol. The text for the
    date is left-justified about the current point. This statement is normally only
    used in the construction of sheet format symbols.

       For example: MOVETO 500,300
                    @DATE

       will display the current date at symbol location (500,300).

@DRAWNBY (Syntax: @DRAWNBY)
    Use this statement to display the drawn by schematic value. The text is left-
    justified about the current point. This statement is normally only used in the
    construction of sheet format symbols.

       For example: MOVETO 500,300
                    @DRAWNBY

       will display the schematic drawn by value at symbol location (500,300).
                                                                                  199

@INSTANCE (Syntax: @INSTANCE prefix)
     Use this statement to display the part reference designator on the symbol. The
     text for the designator is center-justified about the current point. Prefix is a
     single character that is prefixed to the designator number ("U" for IC's, "R" for
     resistors, etc.) when the part is first added to a schematic.

       For example: MOVETO 500,300
                    @INSTANCE U

       will display the schematic reference number for the part at symbol location
       (500,300).

@PART (Syntax: @PART)
    Use this statement to display the name of the part that is using this symbol. The
    text is center-justified about the current point.

       For example: MOVETO 500,300
                    @PART

       will display the part name at symbol location (500,300).

@SHEETNUMBER (Syntax: @SHEETNUMBER)
    Use this statement to display the current sheet number of the schematic. The
    text for the sheet number is left-justified about the current point. This statement
    is normally only used in the construction of sheet format symbols

       For example: MOVETO 500,300
                    @SHEETNUMBER

       will display the schematic sheet number at symbol location (500,300).

@SHEETTITLE (Syntax: @SHEETTITLE)
    Use this statement to display the sheet title of the schematic. The text for the
    sheet title is left-justified about the current point. This statement is normally
    only used in the construction of sheet format symbols.
200

       For example: MOVETO 500,300
                    @SHEETTITLE

       will display the title of the schematic sheet at symbol location (500,300).

@TITLE (Syntax: @TITLE)
     Use this statement to display the design title of the schematic. The text for the
     title is center-justified about the current point. This statement is normally only
     used in the construction of sheet format symbols.

       For example: MOVETO 500,300
                    @TITLE

       will display the title of the schematic at symbol location (500,300).

@VALUE (Syntax: @VALUE 1-5)
    Use the VALUE1, VALUE2, ... statements to display the associated value
    defined in the current part that is using this symbol. The text for the value is
    center-justified about the current point.

       For example: MOVETO 500,300
                    @VALUE1

       will display the value assigned in the part to VALUE1 at symbol location
       (500,300).

ARC (Syntax: ARC rx, ry, angle, arc)
     Use this statement to draw an arc segment centered about the current position.
     RX and RY are the horizontal and vertical radii values of the arc. ANGLE is
     the beginning angle of the arc in degrees. This angle is measured counter-
     clockwise from the X axis. ARC is the length of the arc, in degrees.

       For example: MOVETO 500,300
                    ARC 100,100,0,90

       will draw a 90 degree arc of radius 100, centered about the point (500,300).
                                                                                  201

       The arc will begin at angle 0. The new current position is (2000,300).

AREA (Syntax: AREA width, height)
    Use this statement to define the overall size of the symbol. The symbol's
    graphic image and all of its pins must fit within this area. Width is the size of
    the symbol in the X direction, height is the size of the symbol in the Y
    direction.

       For example : AREA 1000,3000

       indicates the symbol is one inch wide by three inches tall.

CIRCLE (Syntax: CIRCLE radius)
     Use this statement to draw a circle centered about the current position.
     RADIUS is the radius of the circle.

       For example: MOVETO 500,300
                    CIRCLE 100

       will draw a circle of radius 100 centered about the symbol location (500,300).

CONTROLBLOCK (Syntax: CONTROLBLOCK width,length)
    Use this statement to draw the "IEEE control block" shape. The current
    position is the upper-left corner of the shape. WIDTH and LENGTH are the
    size of the shape.

       For example: MOVETO 500,300
                    CONTROLBLOCK 500,1000

       will draw a control block whose upper-left corner is at location (500,300), and
       is 500 wide by 1000 long.

CURVETO (Syntax: CURVETO xc1,yc1, xc2,yc2, x,y)
    Use this statement to draw a Bezier curve segment starting at the current
    position, using point (xc1,yc1) as the 1st control point, (xc2,yc2) as the 2nd
    control point, and (x,y) as the Bezier termination point. The new current
202

      position is at the end of the curve.

      For example: MOVETO 500,300
                   CURVETO 1000,600 1500,600, 2000,300

      will draw a curve which begins at symbol location (500,300). The curve starts
      toward the point (1000,600), bends toward point (1500,600), and ends at
      (2000,300). The new current position is (2000,300).

DOT (Syntax: DOT radius)
     Use this statement to draw a solid dot centered about the current position.
     radius is the radius of the dot.

      For example: MOVETO 500,300
                   DOT 32

      will draw a solid dot centered about the point (500,300) with a diameter of 64.

DRAW (Syntax DRAW)




                           Figure 10.1       Graphic Symbols

      Use this statement to enable drawing of all symbol items. Drawing is enabled
      by default.

      For example: DRAW
                                                                                   203


       will enable the drawing of the symbol at this point in the symbol definition.

END (Syntax: END)
     This statement indicates the end of the symbol definition. This statement will
     always be inserted for you when a new symbol is created. It is the last
     statement of each symbol definition.

       For example: SYMBOL
                    ...
                    END

       indicates the definition of this symbol is complete.

GRAPHIC (Syntax: GRAPHIC id)
    Use this statement to place one of the graphic symbols defined in the table at
    the right at the current position. ID is the symbol number from the table.

       For example: MOVETO 500,300
                    GRAPHIC 3

       will display the graphic symbol number three at location (500,300).

GROUPBIT (Syntax: GROUPBIT xstart,ystart, xend,yend)
    Use this statement to draw the group bit symbol from the (XSTART,YSTART)
    point to the (XEND,YEND) point. The group bit symbol is used to draw the
    "}" symbol to group I/O pins together. This is a graphic symbol only; it does
    not affect the electrical definition of the symbol. The start and end points
    define the area of the GROUPBIT symbol.

       For example: GROUPBIT 500,300 530,800

       will draw the group symbol within the area bound by the two points (500,300)
       and (530,800).
204

GROUPLINE (Syntax: GROUPLINE xstart,ystart, xend,yend)
    Use this statement to draw the group line symbol from the
    (XSTART,YSTART) point to the (XEND,YEND) point. The group line
    symbol is used to draw the "[" symbol to group I/O pins together. This is a
    graphic symbol only; it does not affect the electrical definition of the symbol.
    The start and end points define the area of the GROUPLINE symbol.

       For example: GROUPLINE 500,300 530,800

       will draw a GROUPLINE indicator bound by the area enclosed by the two
       points (500,300) and (530,800).

GROUPNAME (Syntax: GROUPNAME xstart,ystart, xend,yend)
    Use this statement to draw the group name symbol from the
    (XSTART,YSTART) point to the (XEND,YEND) point. The group name
    symbol is used to draw the "|" symbol to group I/O pins together. This is a
    graphic symbol only; it does not affect the electrical definition of the symbol.
    The start and end points define the area of the GROUPNAME symbol.

       For example: GROUPNAME 500,300 500,800

       will draw the group indicator between the two points (500,300) and (500,800).

IO     Syntax: IO
       Use this statement to begin the definition of one pin of the symbol. The
       statements that follow up to the next END statement are used to define this
       single pin.

       When an IO statement is inserted, its corresponding END statement is added
       automatically. The section below describes each of the statements that are used
       to further define an IO pin. In actual practice, you never have to directly enter
       these statements. All the statements that make up the definition of one IO pin
       are edited at once in a single dialog-box.

       When an IO is deleted, all the statements from the IO to its corresponding
       END are deleted. That is, the entire pin is deleted.
                                                                                   205


       For example: IO
                    SIDE LEFT
                    AT (300,300)
                    PIN 3
                    LABEL "CLK"
                    TYPE IN
                    END

       defines pin 3 of the symbol. The pin lead will be drawn on the left side of the
       symbol drawn from location (300,300). The pin will be labeled "CLK" and is
       electrically an IN type pin.

AT (Syntax: AT x,y)
     This statement defines the end coordinate for the I/O pin. The pin line will be
     drawn from this point to the symbol edge.

       For example: IO
                    AT 300,300
                    SIDE LEFT
                     ...
                    END

       will draw the pin lead location (300,300) to the left side of the symbol.

END (Syntax: END)
     This statements indicates the end of the definition of the current IO pin.

       For example: IO
                     ...
                    END

       indicates the end of the definition of this one I/O pin.
206

LABEL (Syntax: LABEL "string")
    This statement defines the logical name of the IO pin. STRING is the text for
    the logical name. If the text is prefixed with the "~" character, the text will be
    displayed with a bar over the text (invert).

       For example: IO
                     ...
                    LABEL "~XYZ"
                    END

       will display the text "XYZ" for this I/O pin label.

NEGATE (Syntax: NEGATE)
    This statement causes the I/O pin to be drawn with an inverter bubble.

       For example: IO
                    NEGATE
                     ...
                    END

       will draw this pin lead with an inverter bubble.

NOSHOW (Syntax: NOSHOW)
    This statement indicates that the I/O pin will not be shown when the symbol is
    drawn. This can be used to define power and ground pins for a symbol which
    you do not want to be shown on the schematic.

       For example: IO
                     ...
                    NOSHOW
                    END

       will define a pin, but it will not be shown when the symbol is drawn.
                                                                                    207

PIN (Syntax: PIN pinnumbers)
      This statement defines the pin numbers that are valid for this I/O pen. Define
      one pin number for each section of the part that uses this symbol. For example,
      the symbol "SNAND2" used with part "7400 Quad 4 Nand Gates", defines
      three pins like this:

                      IO
                      Pin "1,4,9,12"
                      Label "A"
                       ...
                      End

                      IO
                      Pin "2,5,10,13"
                      Label "B"
                       ...
                      End

                      IO
                      Pin "3,6,8,11"
                      Label "Y"
                      Negate
                      ...
                      End

       From this, we see the logical pin A is physical pin 1 in section 1 of the part,
       physical pin 4 in section 2 of the part, pin 9 for section 3, etc. If the symbol
       being defined cannot be used with a particular section of a part, put zero (0) for
       its section pin number.

       For example: IO
                    Pin "1,0,9,12"
                    Label "A"
                    End

       indicates that this symbol may be used with sections 1, 3, and 4 of the part, but
208

       not with the second section.

SIDE (Syntax: SIDE edge)
      This statement defines the side of the symbol the I/O pin will be drawn on.
      EDGE is one of the following key-words: LEFT, TOP, RIGHT, or BOTTOM.

       For example: IO
                    SIDE RIGHT
                    AT 1300,300
                     ...
                    END

       will draw the pin lead from location (1300,300) to the right side of the symbol.

SYMIN (Syntax: SYMIN symin)
     This statement draws one of the IEEE pin symbols on the inside end of the I/O
     pin. SYMIN is one of the following: NONE, DYNAMIC, POSTPONE,
     HYSTERESIS, OPEN, OPENH, OPENL, PPD, PPU, 3SOUT, AMP,
     ANALOG, COMPLEX, GENERATOR, DIGITAL, SHIFTOUT, SHIFTIN,
     EXTENDED, COMPARE, ON, or OFF. NONE is the default value.

       For example: IO
                     ...
                     SYMIN DYNAMIC
                    END

       will add the IEEE dynamic symbol on the inside when the lead is drawn.

SYMOUT (Syntax: SYMOUT symoutt)
    This statement draws one of the IEEE pin symbols on the outside area of the
    I/O pin. SYMOUT is one of the following: NONE. POLAROUT, POLARIN,
    NONLOGIC, OUT, IN, or INOUT. The default value is NONE.
    For example: IO
                   ...
                   SYMOUT POLAROUT
                  END
                                                                                  209


will show the IEEE polar out symbol on the outside when the lead is drawn.

TYPE (Syntax: TYPE type)
     This statement defines the basic electrical type of the I/O pin. TYPE is one of
     the following: NONE, IN, OUT, INOUT, POWER, NC, or UNKNOWN. This
     value is used in checking schematics for proper net construction.

       For example: IO
                    TYPE OUT
                     ...
                    END

       indicates this pin is an output type pin.

LINETO (Syntax: LINETO x,y)
     Use this statement to draw a line from the current position to the coordinate
     (x,y). The end of this line is the new current position.

       For example: MOVETO 500,300
                    LINETO 1000,300

       will draw a line beginning at symbol location (500,300) and ending at symbol
       location (1000,300). The new current position is (1000,300).

LINEWIDTH (Syntax: LINEWIDTH width)
     By default, each symbol will draw symbol body lines of the width specified in
     the system configuration. You can use this statement to over-ride the line-
     width used to draw the symbol. Setting this value will not affect the line-width
     used to draw the pin leads.

       For example: LINEWIDTH 20

       will cause symbol lines to be drawn 20 mils wide. This width will stay in affect
       until it is changed by another LINEWIDTH or LINEWIDTHSYMBOL
       statement. It will not affect other symbols.
210

LINEWIDTHLEAD (Syntax: LINEWIDTHLEAD)
     Use this statement to set the current line-width for drawing the symbol to be
     the same as the configured pin lead line-width.

       For example: LINEWIDTHLEAD

       will cause symbol lines to be drawn the same width as the pin lead lines.

LINEWIDTHSYMBOL (Syntax: LINEWIDTHSYMBOL)
     Use this statement to restore the drawing line-width to the configured value.

       For example: LINEWIDTHSYMBOL

       will cause lines to be drawn using the configured width for drawing symbols.

MOVETO (Syntax: MOVETO x,y)
    Several of the symbol statements depend on the current location for
    positioning. Use this statement to set the current position to coordinate (x,y).

       For example: MOVETO 500,300

       will set the current position at symbol location (500,300).

NAME (Syntax: NAME "string")
    Use this statement to define the name of the symbol. String is the name of the
    symbol. This name is used when it is stored or loaded from a library.

       For example: NAME "7400"

       defines the name of this symbol to be 7400.SYM.

NODRAWXOR (Syntax: NODRAWXOR)
    Use this statement to disable further drawing of the symbol if the current draw
    mode is XOR. The draw mode will be XOR when a symbol is on the cursor, or
    a symbol is being dragged to a new location. Drawing will resume when the
    DRAW statement is encountered. Proper use of this statement can improve
                                                                                211

       performance by not drawing portions of a symbol when it is on the cursor, or
       being moved.

       For example: NODRAWXOR

       will disable further drawing of the symbol until a DRAW statement is
       encountered.

OUTLINE (Syntax: OUTLINE width,length)
    Use this statement to draw the IEEE outline shape. This is the standard box
    type shape. The current position is the upper-left corner of the shape. WIDTH
    and HEIGHT are the size of the shape.

       For example: MOVETO 500,300
                    OUTLINE 500,1000

       will draw an outline box whose upper-left corner is at location (500,300), and
       is 500 wide by 1000 long.

OUTPUTELEMENT (Syntax: OUTPUTELEMENT width,length)
    Use this statement to draw the IEEE output element shape. The current position
    is the upper-left corner of the shape. WIDTH and HEIGHT are the size of the
    shape.

       For example: MOVETO 500,300
                    OUTPUTELEMENT 500,1000

       will draw an output element block whose upper-left corner is at location
       (500,300), and is 500 wide by 1000 long.

SYMBOL (Syntax: SYMBOL)
    This statement indicates the beginning of a symbol definition. This item, along
    with its corresponding END statement will always be automatically added for
    you when a symbol is created.
212

       Example:       SYMBOL
                      ... (statements to define symbol)
                      ...
                      END

TEXTC (Syntax: TEXTC "string")
    Use this statement to display a text string on a symbol, center-justified about
    the current point.

       For example: MOVETO 500,300
                    TEXTC "Hi there!"

       will display the text "Hi there!" at center-justified about location (500,300).

TEXTL (Syntax: TEXTL "string")
    Use this statement to display a text string on a symbol, left-justified about the
    current point.

       For example: MOVETO 500,300
                    TEXTL "Hi there!"

       will display the text "Hi there!" at left-justified about location (500,300).

TEXTR (Syntax: TEXTR "string")
    Use this statement to display a text string on a symbol, right-justified about the
    current point.

       For example: MOVETO 500,300
                    TEXTR "Hi there!"

       will display the text "Hi there!" at right-justified about location (500,300).

RCURVETO (Syntax: RCURVETO dxc1,dyc1, dxc2,dyc2, dx,dy)
    Use this statement to draw a Bezier curve segment starting at the current
    position, using relative point (dxc1,dyc1) as the 1st control point, relative point
                                                                                 213

       (dxc2,dyc2) as the 2nd control point, and relative point (dx,dy) as the Bezier
       termination point. The new current position is at the end of the curve.

       For example: MOVETO 500,300
                    RCURVETO 500,300 1000,300, 1500,0

       will draw a curve which begins at symbol location (500,300). The curve starts
       toward the point (1000,600), bends toward point (1500,600), and ends at
       (2000,300). The new current position is (2000,300).

RLINETO (Syntax: RLINETO dx,dy)
     Use this statement to draw a line from the current position to the relative
     coordinate (dx,dy). The end of this line is the new current position.

       For example: MOVETO 500,300
                    RLINETO 1000,300

       will draw a line beginning at symbol location (500,300) and ending at symbol
       location (1500,600). The new current position is (1500,600).

RMOVETO (Syntax: RMOVETO dx,dy)
    Use this statement to translate the current position by the distance (dx,dy). This
    is a relative moveto.

       For example: RMOVETO 500,300

       will set the current position 500 to the right and 300 down from its current
       position.

SECTIONS (Syntax: SECTIONS nsections)
     Use this statement to define the number of sections that this symbol may
     represent. NSECTIONS is the number of sections. For example, the "7400
     Quad Nand Gates" part has four sections (four gates per package). A single
     symbol may represent any one of these individual sections. If the SECTIONS
     statement is not included, the part is assumed to have only one section.
214

      For example: SECTIONS 4

      indicates this symbol has four sections.

      The reference grid is for reference only, and is not part of the actual board. It
      may be turned on to aid in the placement of parts or the alignment of other
      objects. The reference grid will not appear on hard-copy prints of the board.
      Also, the reference grid does not affect the cursor motion.

      Normally, the cursor coordinate represents the distance from the upper-left
      corner of the board. Enabling a relative cursor allows you to measure relative
      to any coordinate. Although you can set the relative cursor parameters from
      this dialog-box, the easiest way is simply to move the cursor to the coordinate
      from which you want to measure and press the "." (period) key. This will set
      the relative cursor at this point. When a relative cursor is active, the coordinate,
      displayed in the upper-right of the screen will appear reversed. Just press the
      period key again to return to absolute mode.
                                                                                  215



Chapter 11
BOARD CREATOR Basics
Printed Circuit Board Nomenclature
Types of Masks and Drawings
Several different types of masks and drawings are used in the construction of printed
circuit boards. Each of these drawing types are summarized in the following sections.

Conductor Mask




                           Figure 11-1 Conductor Mask

A conductor mask is used to represent the electrical networks on a single layer of a PC
board. There is a different conductor mask for each electrical layer of the board.

A conductor mask contains the following type of data.
      • Lines for the conducting networks.
      • Pads for attachment to electrical components.
      • Vias to connect through the board.
      • Optional text strings to document the mask.
      • Board limit and crop marks.
216

Solder Mask




                              Figure 11-2 Solder Mask

A solder mask is used to paint the solder side of a board. Usually this is the bottom
side of the board, but if surface mount devices (SMD's) are used, a solder mask may
also be required for the top side of the board. This mask allows the board to be painted
on all but the pad, via and other special areas. By painting a board in this manner, only
the non-painted areas will attract solder during the wave soldering step of
construction.

Paste Mask




                              Figure 11-3 Paste Mask

A paste mask is used to aid in the assembly of PC boards that contain surface mount
devices. The mask allows only the component pads on a board that have no hole (the
SMD's) to be applied with a solder paste prior to soldering the SMD parts to the board.
                                                                                     217

Silk-Screen Mask




                           Figure 11-4 Silk-Screen Mask

A silk-screen mask is used to paint component outlines, part references, part numbers
and other text onto the top or bottom side of a board. The text labels and documents
the board, and also aids in the assembly of the board. It does not electrically affect the
board.

Drill Drawing




                              Figure 11-5 Drill Drawing

A drill drawing is used to indicate the location and size of all holes to be drilled in a
board. A path, showing the order that the holes are to be drilled is also shown. The
hole locations may be digitized and used to drive automated drilling equipment.
218

Assembly Drawing




                          Figure 11-6 Assembly Drawing

An assembly drawing is used to show the board outline, component locations, and
other mechanical information. This drawing is used for reference during the final
assembly of the board.

Power/Ground Plane Masks




                         Figure 11-7 Power Plane Masks

A power/ground mask is used to make a conducting layer of a board which is
dedicated to a single net, usually one of the power or ground signal levels. This layer
is a solid sheet of conductor which connects directly to the component pins of the
dedicated net. All other component pins have a cutout around them to prevent making
contact with the conductor.
                                                                                    219

Power/ground masks are optional, and are normally only used on boards which can
justify the cost involved in making boards of more than two conducting layers.

Power planes may also be used to reduce the size of a board. Using power/ground
layers can greatly simplify the routing of the other nets. This is because the lines used
to route the power and ground networks no longer need to be routed on the conductor
masks. Since nearly every component will connect to power and ground, a large
amount of net routing area is freed.

Schedule Drawing




                          Figure 11-8 Schedule Drawing

A schedule drawing is not required in the building process of a PC board. However, it
may prove very useful during the lay-out of a board. It shows all the connections that
have not yet been completed for a board. It is also useful in planning component
placement on large boards.

Sketches
Sketches may be used to make any additional drawings or sketches associated with the
board. Drawing on the sketch mask does not electrically affect the board.
220

Launching BOARD CREATOR
From the CIRCUIT CREATOR Start Menu group click on BOARD CREATOR and
the opening screen appears as shown in the following figure.




                 Figure 11-9: Board Creator Opening Screen

Presentation
      The screen is divided into several windows. Each window contains a specific
      type of information.

      The top area of the screen is the title-bar window. This line displays the name
      of the program, the file currently being edited and the current cursor's location.

      Just down from the top is the action-bar window. This window displays the
      title of each of the pull-down menus assigned to it.
                                                                                 221

       The bottom area of the screen is the command status window. This line
       displays the current command that is active, and additional values and sub-
       commands that are of particular interest for this command.

       The center area of the screen is the editing window. It is used to display the
       schematic that is currently being edited. Also, dialog-boxes may pop-up in this
       area from time-to-time.

       The editing window is bordered on the top and left with rulers to assist in the
       location and positioning of items.

       The editing window is bordered on the right and bottom with slide-bars. The
       slide bars are used in conjunction with a mouse to change the view of the edit
       window. The view may also be set by keyboard and menu commands.

BOARD CREATOR: PC BOARD TUTORIAL
INTRODUCTION
This chapter present tutorial for the BOARD CREATOR PC board layout program,
and the ROUTE CREATOR program. These tutorials will give you actual hands-on
experience using the CIRCUIT CREATOR system. The tutorials will lead you
through the creation of a simple schematic and its PC board layout.

NOTATION
The following notation is used throughout the tutorials.

The notation "XXX" indicates that the characters shown between the quotes are to be
typed. For example, "XYZ" indicates that the characters X, Y, and Z are to be typed.
Do not type the quotes.

The notation, XXX, indicates this single key, key combination, menu/command, or
dialog-box button should be pressed. For example, ENTER means press the enter key
while G indicates the G key is to be pressed. FILE/OPEN means to select the OPEN
command from the FILE menu. OK means to select the OK button in a dialog-box.
Unless otherwise noted, either upper or lower case may be used.
222


The notation, (xxx,yyy), indicates a coordinate. For example, (10.0,15.250) indicates
the horizontal position is 10 inches and the vertical position is 15.250 inches.

The tutorial steps are listed in terms of the keyboard. If your system has a mouse, feel
free to use it. The left button of the mouse is equivalent to the ENTER key, while the
right button is equivalent to the ESC key.

Initially, great detail is given. As we proceed through each of the tutorials, and you
learn the basics; less detail will be given. If you will be using a plotter connected to a
serial port.

This tutorial leads you, step by step, through the creation of a simple PC board. If you
have not yet installed the evaluation software, refer to Chapter 5 for instructions.

STARTING BOARD CREATOR
To run the BOARD CREATOR program, double click on the CIRCUIT CREATOR
program group (if it has been minimized) and then double click on the BOARD
CREATOR icon.

LOADING A BOARD
To get a feel for the system, we will first load a sample PC board file. We will then
learn how to navigate about the board on the display. First, an explanation of how to
select commands from the pull-down menus and dialog-boxes will be given.

If you are using the keyboard, a pull-down menu may be displayed (pulled-down) by
holding the CTRL key down and pressing the key indicated by the underlined
character in its name on the title-bar. Upper or lower case may be used.

When a pull-down menu is displayed, the       and  arrow keys may be used to move
to the next menu to the right or left. The NUMLCK key must be off. Use the and
arrow keys to move the menu selector up and down. Move to the FILE/OPEN
command and select it by pressing the ENTER key.

If you are using a mouse, you may pull-down a menu by moving the pointer to the
menu name in the title-bar and pressing the left mouse button and releasing it. The
                                                                                 223

menu will appear when the button is released. To select a menu item, move the pointer
to the desired item and press the left mouse button and release it. The selection is
made when the button is released. For quicker menu selections, move the pointer to
the title and press the left mouse button and do not release the button yet. Now, move
the pointer to the desired menu item and release the button to make the selection.

After selecting the FILE/OPEN command, a dialog-box will appear which is
prompting for the name of a PC board file. At this point, we can type the file name of
a file, or select one from the list that is displayed. Use the arrow keys to move the
selector to the file in the list named "DEMO.PCB" and press ENTER. This will copy
the file name from the list into the file field of the dialog-box. Now press ENTER
again to directly accept this name, or press the HOME key to move the selector to the
OK button, then press ENTER.

When a dialog-box is displayed, clicking the left mouse button on the OK button, or
pressing the ALT-O key combination will immediately accept the values in the dialog-
box. Pressing the Home key will move the selector to the OK button.

Clicking on the CANCEL button, or pressing the ALT-C combination will
immediately cancel the dialog-box. Pressing the END key or the ESC key will move
the selector to the cancel button. Once the selector is on the cancel button, pressing
ESC again will cancel the dialog-box. Any changes made to the values shown in a
dialog-box do not actually take effect until the OK button is pressed. If the cancel
button is pressed, the changes made to values in the dialog-box are ignored.

For a file-selection or part-selection dialog-box, pressing ENTER twice while on the
same name in the list implies that this is the name you want to accept immediately.

GETTING HELP
Press the F1 key to pop-up a window of help information. Notice that the help
information is specific to the current command being performed. The UP and DOWN
buttons may be used to page the help text up and down in the window. You may also
use the NEXT, PREV, or GENERAL buttons to view other help topics.

Now, select the EXIT button to close the help window. Help is always available with
the F1 key.
224

NAVIGATION
We will now learn how to change the view of a PC board displayed on the screen.
Pull-down the VIEW menu. Now, move down and select the ZOOM OUT command.
The display will be redrawn at a smaller scale. You will notice that the ZOOM OUT
menu item has CTRL+PGDN listed in the right margin next to it. This indicates that
this command has a hot-key. This key combination may be used when the menu is not
displayed to directly execute this command. Let's try it. Now, hold the CTRL key
down and press the PGDN key to zoom-out. Once you are more familiar with the
program, using hot-keys will improve your productivity, especially if you do not have
a mouse.

Zoom back to the original scale by pressing the CTRL+PGUP key twice.

It should be noted that if you pick the pan and zoom commands directly, you do not
need to wait for the redraw to complete before entering another pan or zoom
command. In this case, the current redraw will be stopped, and the next redraw will
begin directly.

The current coordinate of the cursor is displayed in the upper-right corner of the
screen. Use the cursor keys to move the cursor to coordinate (2.000,1.000). Follow the
track of the cursor on the screen, and watch the value in the upper-right corner change.
Notice that the active cursor (the little cross) is not always the same as the mouse
pointer position.

Holding the SHIFT key down and using the cursor keys will move the cursor one inch
at a time. Hold the SHIFT key down and use the arrow key to move quickly to
coordinate (0.000,0.000), the upper-left corner of the sheet.

The display may be panned using the keyboard by bumping into one of the edit
window edges. First, zoom in with the CTRL+PGUP key. Now, let's pan right. Move
the cursor with the SHIFT      key until it bumps the right edge of the window. The
portion of the board that was out of view to the right of the screen is now displayed.

With a mouse, the view may be panned by using the vertical slide-bar at the right, or
the horizontal slide-bar at the bottom.
                                                                                    225

Display the upper-left corner of the board at normal scale by pressing CTRL+HOME.

We will now explore how to select the layers of information that are displayed on the
screen. Execute the LAYER/MASKS command on the VIEW menu.

You will notice that each layer of the board is listed along with its type and current
conductor color. If there is not a check-mark by a layer, then items on that layer will
not be displayed. The actual colors and number of colors available will depend on
your particular hardware. The display state of each layer is changed by moving the
focus indicator to that layer and pressing ENTER to turn it on or off.

Also, this dialog-box allows you to select which masks will be displayed.

Turn off all layers except layer 1 and all masks except the silk-screen mask. Press the
OK button. Notice that only items which are on the silk-screen mask for layer 1 of the
board are displayed.

Now, let's display just the solder-side layer of the board. Select the
VIEW/LAYERS/MASKS command again. Enable the "all" layer, and layer 4 (solder-
side, last layer). Enable all the masks. Press OK. Notice that only the items that belong
to the solder-side, or go through the board, are displayed.

CURSOR GRID
The cursor grid is set to 50 mils by default. You have probably noticed that the cursor
steps 50 units each time the arrow keys are pressed. Select the GRID/CURSOR
command on the VIEW menu. Set the cursor grid X and Y grid steps to "0.025" and
press OK. This sets both the cursor grid step values to 25 mils. Move the cursor about
the screen with the arrow keys. Notice that the cursor now moves in steps of 25 mils.

This completes a summary of how to start the BOARD CREATOR editor, load an
existing board, view the board, choose which layers and masks are to be displayed,
and how to set the cursor grid step values.
226

CREATING A NEW PC BOARD




                                     Figure 11.10

Our assignment is to create a PC board which implements the design shown in the
following figure. Once created, it will be checked for errors, with assistance from the
program. Masks and reports about the design will be generated. This circuit is
intentionally simple and small; however, it demonstrates the basic steps by which any
circuit, regardless of size, is created. This circuit corresponds to the tutorial lesson
used in the companion LOGIC CREATOR schematic system.

The overall board specification is as follows:

       1.   Board size is 3.00" x 2.00".
       2.   Board has 2 signal routing layers, route 10 mil lines.
       3.   Power and ground provided by power planes.
       4.   Conductor masks required.
       5.   Solder mask required.
       6.   Silk-screen required.
       7.   Drill-drawing required.
                                                                                       227

Bill of Material:
        Count Part-Name            Description
---------------------------------------------------------------------------
         1        7420             Dual 4-Input Nand Gates
         1        7474             Dual D-Type Flip-Flop
         1        CONN-12          12 Pin Connector
         2        LED-RED Light Emitting Diode, Red
         2        R330             330 Ohm Resistor

Since this board corresponds to a schematic drawn with the LOGIC CREATOR
schematic system, we will use the "update-list" produced by LOGIC CREATOR to
create out initial PC board. We will begin the new board by selecting the CREATE
FROM LOGIC CREATOR command on the I/O menu. Since we already have a board
loaded, we will be questioned as to whether or not we wish to save the changes made
to the current board. Answer NO when prompted.

The following is the complete LOGIC CREATOR update-list for the "MYDESIGN"
tutorial lesson. It defines each part, part-footprint, and net assignment for every pin on
the board. This is all the information that is required to create the initial PC board for a
design.

        BOARD CREATOR upd
        UPDATE_LIST
        PART 7420 U1 DIP-14
        PAD U1 1 #0007
        PAD U1 2 #0008
        PAD U1 3 NC
        PAD U1 4 #0009
        PAD U1 5 #0010
        PAD U1 6 #0001
        PAD U1 7 GND
        PAD U1 8 #0002
        PAD U1 9 #0011
        PAD U1 10 #0012
        PAD U1 11 NC
228

      PAD U1 12 #0013
      PAD U1 13 #0014
      PAD U1 14 +5V
      PART 7474 U2 DIP-14
      PAD U2 1 RESET
      PAD U2
      2 +5V
      PAD U2 3 #0001
      PAD U2 4 NC
      PAD U2 5 NC
      PAD U2 6 #0003
      PAD U2 7 GND
      PAD U2 8 #0005
      PAD U2 9 NC
      PAD U2 10 NC
      PAD U2 11 #0002
      PAD U2 12 +5V
      PAD U2 13 RESET
      PAD U2 14 +5V
      PART R330 R1
      DISC-2
      PAD R1 1 #0003
      PAD R1 2 #0004
      PART R330 R2
      DISC-2
      PAD R2 1 #0005
      PAD R2 2 #0006
      PART LED-RED D1 DISC-2
      PAD D1 1 +5V
      PAD D1 2 #0004
      PART LED-RED D2 DISC-2
      PAD D2 1 +5V
      PAD D2 2 #0006
      PART CONN-12 W1
      CONN12
      PAD W1 1 #0007
                                                                                   229

       PAD W1 2 #0008
       PAD W1 3 #0009
       PAD W1 4 #0010
       PAD W1 5 #0011
       PAD W1 6 #0012
       PAD W1 7 #0013
       PAD W1 8 #0014
       PAD W1 9 RESET
       PAD W1 10 +5V
       PAD W1 11 NC
       PAD W1 12 GND
       END_UPDATE_LIST

We are now prompted for the name of the update-list file to be used. Select the
"MYDESIGN.UPD" file from the list. BOARD CREATOR will now read the part and
net assignment information from the update-list file and create a board with these parts
on it.

Component Placement
We now have a PC board with all the required component parts. The next step is to
move each part to its actual location on the board, then we will adjust the board to its
true size and number of layers. Although moving the parts is a manual process, we
will be assisted by the program. It will show us how the parts connect to one another.
To do this we will need a routing schedule.

Run the CHECK/SCHEDULE command from the REPORTS menu. Use a default
routing line width of 0.010" (10 mils). This will generate a routing schedule for us.
The schedule "rats-nest" lines are visible on the screen when the schedule mask is
enabled, or when a component is selected. Since these lines show us exactly the pin-
to-pin connections that must be routed, we will want to place the parts so the length of
these lines are as short as is reasonable.

Before we begin placing parts, we will setup the select options for doing component
placement. Execute the SELECT command on the EDIT menu and press the O key to
pop-up the select command options. Set the select layer to ALL. Enable
COMPONENT and TOUCHING modes. Enable all the other check-boxes except the
230

SCHEDULE mask. By not enabling the schedule mask for selection, we will not
accidentally select schedule lines that are "just passing through" our select area.
Selecting a component will still select the schedule lines that belong to that particular
component. Press OK.

We are now ready to begin placing the parts. Move the cursor to location
(0.000,0.000) and zoom in twice (CTRL+PGUP). This is a good working scale for
placing this board.

For this tutorial lesson, we will move all the components by selecting pin one of each
component. This is done to establish the coordinate numbers listed in this tutorial.
When you are working on your own, you may move a component by selecting
anywhere on the component.

Move the cursor to location (0.200,1.300) and press ENTER twice, or click with the
left mouse button. This will select component U2. Now, press ENTER, or press the
left mouse button and continue to hold it down. This will "grab" the component for
moving. Move the part with the arrow keys, or by moving the mouse. Notice how the
schedule lines stretch to show you how this part connects to other parts. Move until
you are at location (2.100,0.650). Press ENTER, or release the left mouse button, to
place the part at this location. If you make a mistake, press F2 (undo), try again.

You do not need to un-select the component, it will be un-selected when the next
component is selected. Using the procedure just established, place the following
components:

       Select U1 at (0.200,0.300). Move it to (1.250,0.650).
       Select R1 at (0.200,2.300). Move it to (2.100,1.500).
       Select R2 at (0.200,2.700). Move it to (1.100,1.500).
       Select D2 at (0.200,3.100). Move it to (1.100,1.700).
       Select D1 at (0.200,3.500). Move it to (2.100,1.700).

Now we have placed all the components except the edge connector. In addition to
moving it, it also needs to be rotated. Select the connector, W1, at (0.300,4.100). Grab
the connector and begin to move it just like the other components. While the connector
is on the cursor, we may press the O key (or F10) to rotate the part 90 degrees. Press
                                                                                    231

the O key three times to rotate the part a total of 270 degrees. Move to (0.150,0.450)
and place the part. Press the Z key to unselect the component.

Now all the components are placed in a reasonable location for routing the electrical
connections.

Set True Board Size/Layers
Execute the BOARD FORMAT command on the EDIT menu. Set the number of
layers to 4, the width to 3.000", and the length to 2.000". To set a layer type, move the
layer focus indicator to the layer number and press ENTER to pop-up a menu. Select
the layer type from the menu. Set the layer types as follows:

       1 - Top conductor (already set).
       2 - Top power layer, net name "GND".
       3 - Bottom power layer, net name "+5V".
       4 - Bottom conductor (already set).

To set the net names, move the layer focus indicator to one of the power layers. Since
this is a power layer, the net name field will now become enabled. If you use the
keyboard, type ALT+N to pop-up the net name field. Type the net name into the net
field. Do this for both of the power layers.

Set the title, engineer, and other "accounting" fields to appropriate values. These
values will be printed on reports generated for this board.

Press OK to accept the new board definition.

Routing The Board
We are ready to route the conductor lines that make the desired circuit. Before we
begin routing the board, we will run the CHECK/SCHEDULE command on the
REPORTS menu again. This is done for two reasons. First, we have just done a major
placement of the board. With the new component locations, it may be possible to
generate a more efficient routing schedule. Also, we have just added a power and
ground layer to the board. There is no longer a need to schedule lines for the "GND"
and "+5V" nets. Pads assigned to these nets will connect directly to the power and
ground layers.
232

Now we will begin routing the board. Execute the LINE/CURVE command on the
DRAW menu. From our specification, the width of the routing lines is 10 mils. The
current line width is displayed in the bottom status line. If this is not 0.010", press the
O key, or click on the status line with the mouse pointer, to display the line drawing
options. Set the line width to 0.010" (10 mils).

For this board, we will the use the component-side for the mostly horizontal routes,
and the solder-side for the mostly vertical routes.

From our procedures given in Chapter 2 for routing a board, we will route the shortest
lines first. Since we can see from the routing schedule lines shown on the screen
which pads need to be connected together, look for some short ones.

Move to coordinate (1.600,1.500) and press ENTER, or click with the left mouse
button. The schedule line from this pad is now high-lighted, showing us the
connection that needs to be made. Since this route will be mostly vertical, we will
route this line on layer 4, the solder side of the board. Notice that the status line
indicates the current edit layer is layer number 1. Press F9 to "toggle" to routing layer
to layer 4. Now move to (1.600,1.700) and press ENTER, or click with the left mouse
button. This will complete the first route. Notice that the schedule line is now gone,
indicating that this route is complete. Press ESC, or click the right mouse button to
stop drawing this line. If you make a mistake while still drawing a route, press
BACKSPACE to "backup" (instead of UNDO).

Now let's do another route. Move to (2.600,1.500), ENTER, move to (2.600,1.700),
ENTER, and ESC.

Got the hang of it? Routing lines on your own will actually be much easier. You will
work directly from the screen instead of reading coordinates from a book. Now let's
route a line with some bends in it. Move to (2.100,1.500), ENTER, move to
(2.100,1.400), ENTER, move to (2.150,1.350), ENTER, move to (2.150,1.200),
ENTER, move to (2.100,1.150), ENTER, and ESC.

Now, press F9 to toggle back to layer 1. Route lines between the following points.
More instruction will be given when we add a via for the first time.
                                                                                      233

       Layer 1:        (2.100,0.650), (2.200,0.650), (2.300,0.750, (2.400,0.750).

       Layer 1:        (0.150,0.450), (0.800,0.450), (1.000,0.650), (1.250,0.650).

       Layer 1:        (0.150,0.550), (0.800,0.550), (1.000,0.750), (1.250,0.750).

       Layer 1:        (0.150,0.650), (0.800,0.650), (1.100,0.950), (1.250, 0.950).

       Layer 1:        (0.150,0.750), (0.800,0.750), (1.100,1.050), (1.250,1.050).

       Layer 1:        (0.150,0.850), (0.800,0.850), (1.150,1.200), (1.450,1.200),
                       (1.500,1.150), (1.550, 1.150).

The next line will require a via. Route the line as before, up to the point where a via is
noted. At the point just ENTER again, or click the left mouse button. This is the same
as drawing a line segment with no length. This will add a via at this point, and toggle
the routing layer. Continue drawing the remainder of the line on the other layer.

       Layer 1:        (0.150,0.950), (0.750,0.950), (0.900,1.100), VIA, (1.350,1.100),
                       (1.400,1.050), (1.550,1.050).

Remember to start each line on the proper layer.

       Layer 1:        (0.150,1.050), (0.750,1.050), VIA, (0.900,0.900), (1.450,0.900),
                       (1.500,0.850), (1.550,0.850).

       Layer 1:        (0.150,1.150), (0.650,1.150), VIA, (0.650,1.000), (0.850,0.800),
                       (1.400,0.800), (1.450,0.750), (1.550,0.750).

       Layer 1:        (1.550,1.250), (1.800,1.250), (1.950,1.100), (2.200,1.100),
                       (2.350,0.950), (2.400,0.950).

       Layer 1:        (1.250,1.150), (1.400,1.150), (1.450,1.100), (1.700,1.100),
                       (1.950,0.850), (2.100,0.850).
234

       Layer 1:        (1.100,1.500), (1.350,1.500), (1.500,1.350), (2.200,1.350),
                       (2.300,1.250), (2.400,1.250).

       Layer 1:        (0.150,1.250), (1.000,1.250), (1.100,1.350), (1.350,1.350),
                       (1.500,1.200), (1.750,1.200), (1.950,1.000), (2.200,1.000),
                       (2.200,0.800), (2.000,0.800), (2.000,0.650), (2.100,0.650).

The remaining two routes deserve some special attention. Even though this board has
power and ground planes, the planes themselves must receive power from some
external connection. For this board, one pin on the edge connector is assigned to net
"GND", and another one is assigned to net "+5V". Since these pins do not have holes,
they do not connect to the power planes directly, and must be routed to a point that
does. Otherwise the board will not be powered.

Power lines are normally routed with a wider than normal line width. Set the line
width to 0.025" (use the O key to pop-up the line dialog-box). Now, route the
following power lines:

       Layer 1:        (0.150,1.350), (0.850,1.350), (0.900,1.400), (0.900,1.650),
                       (0.950,1.700), (1.100,1.700).

       Layer 1:        (0.150,1.550), (0.750,1.550), VIA, (0.750,1.300), (0.800,1.250),
                       (1.250,1.250).

This completes the routing of the board. Notice that there was never a need to refer
directly to the update-list, or any other lists. All the information necessary to place and
route the board was presented directly on the screen where you were working.

Adding Text
Next, we will learn how to add notational text strings to the board. Text is often added
to directly identify the layer of the mask, the company name, copyright notice, etc. Be
careful when adding text to a conductor layer. The text will be etched in copper on the
actual board. Do not place the text where it will touch any conductor lines.

Select the DRAW/TEXT command. Move to (1.000,0.300) and ENTER to begin
adding a text string. In the dialog-box, enter "Copyright (c) 2000 by Me" for the text,
                                                                                     235

layer 1, mask SILK-SCREEN, size 0.062", angle 0, font NORMAL, and mirroring
NONE. Press OK to add the text. The text will appear on the board at the location of
the cursor and have attributes which match these settings.

Move to location (2.800,1.300). Press ENTER and add the string "Component Side"
to the CONDUCTOR mask with an angle of UP. Put "GND" on power layer 2. Notice
how the display adjusted to show a power layer. Put "+5V" on power layer 3.

Move to (2.750,1.300) and add "Solder Side" on layer 4 with an angle of DOWN, and
mirroring set to RIGHT-TO-LEFT. This will make this text readable when it is viewed
from the back-side of the board.

Add the string "ASSEMBLY DRAWING" on the ASSEMBLY DRAWING mask of
layer 1 (angle 0, no mirroring). Likewise, add the string "DRILL DRAWING" to the
DRILL DRAWING mask of layer 1.

You may add any additional text as desired. Set the angle, size, and mirror factors as
desired in the dialog-box.

Check The Layout
To check our board for routing completeness, run the CHECK-SCHEDULE command
from the REPORTS menu. If you have completed the board correctly, a message "All
scheduled routes complete" will appear; otherwise, the schedule lines for any
uncompleted routes will be generated. If you have routed two nets together, creating a
"short", the location of the problem will be displayed directly on the screen.

Also, run the CHECK CLEARANCE command from the REPORT menu. This
command will check that all lines, pads, vias, etc. have at least the specified clearance
distance from each other. If errors are detected, they will be pointed out directly on the
screen.

If any errors are detected, try to correct the problem and re-run the checks until there
are no errors.
236

Printing The Masks
Now that the board is complete, and has passed all the error checks, it is time to print
the masks for this board. If you have not yet selected the printer device, use the SET-
UP PRINTER command on the FILE menu to select your printer device and set the
basic printing options.

Execute the FILE/PRINT command. The dialog-box for printing allows you to queue
up to ten masks to be printed. Queue the following masks:

       1.   Layer 1, Conductor mask.
       2.   Layer 1, Silk-screen mask.
       3.   Layer 1, Assembly drawing.
       4.   Layer 1, Drill Drawing.
       5.   Layer 2, Conductor mask.
       6.   Layer 3, Conductor mask.
       7.   Layer 4, Conductor mask.
       8.   Layer 4, Solder mask.

Enable TARGETS, BANNER, and BORDER. Set the method to PANELS to save
paper. Set the other options as desired. If your printing device requires you to change
paper between each print (as required by some plotters), enable the PAUSE option.
Review the settings and make sure a check mark, indicating that the queue slot is
enabled for printing, appears next to each of the first seven queue slots. Press OK to
begin printing the masks.

For most boards, it is necessary to set-up the printing parameters for a board only
once. The printing set-up parameters are saved with the board.

REPORTS
From the commands on the REPORT menu, generate a PARTS LIST, a NET LIST
(pads only option), and a SUMMARY report. If you have a printer, you may direct the
reports directly to the printer. Compare these reports with the schematic net and parts
list. They should agree.
                                                                                   237

SAVING THE BOARD
Now we will save our board to a file. Select SAVE AS command from the FILE
menu. Enter "MYDESIGN" for the file name and press OK. This will save the board
into the file "MYDESIGN.PCB".

EXIT THE PROGRAM
We are finished with the board for now. Select the EXIT command on the FILE menu,
or just press ALT-X, to exit the program.

ADDITIONAL TRAINING
The tutorial you have just completed is designed to familiarize you with the basic
steps in using BOARD CREATOR to create a board. To become a more advanced
user of BOARD CREATOR, and to use its features to your best advantage, the
following self-training procedure is suggested.

Start the BOARD CREATOR program and use the FILE/NEW command to create a
new board (any reasonable size). Go through each of the commands on the menus, one
at a time. For each command, display the help information with the F1 key. Study the
options for each command and practice each of these operations on the board. It is not
necessary to construct a real or complete board. Just use the board as a scratch area to
practice the commands. For example, practice the DRAW/TEXT command by placing
text of various sizes, angles, mirroring, layers, etc. on the board. Move a text string.
Move and rotate an area of text strings. Update a text string. Delete a text string. Do
this for each command and you will quickly become a "power user" of BOARD
CREATOR.

In the tutorial just completed, you were instructed how to perform each step in the
construction of a simple board. Therefore, there was little or no opportunity to make
changes to the board during the tutorial. In the real world, you will need to make
changes, move things around, and correct mistakes. Changes are made with the
SELECT command. In fact, it is the default command. Just press ESC to exit the
current command, and you are running the SELECT command. Before any object can
be changed, it must first be selected. For more information on the select command,
execute the SELECT command and then press F1 for detailed help about the
command and its usage.
238

ROUTE CREATOR: AUTO ROUTE TUTORIAL
This chapter shows you how to run ROUTE CREATOR demos. In actual practice, the
ROUTE CREATOR auto-router is used to automatically route the connections for a
board. Although the router cannot route every board to 100% completion, it does
perform the vast majority of the board layout.

Before a board is routed, the board is first "scheduled" for routing. The routing
schedule is generated with the BOARD CREATOR editor. The schedule gets a board
ready for routing by determining which points on the board need to be connected. The
sample boards used in the demos have already been scheduled.

Once a board is prepared, the auto-router uses artificial intelligence to route the
connections of the board. The auto-router will preserve any nets that you have pre-
routed. Also, the auto-router may be interrupted while it is running. At this point, the
BOARD CREATOR editor may be used to manually make adjustments to the board.
The board may then be resubmitted to the auto-router to continue the remainder of the
routing.

ROUTE CREATOR Pro
Note: Make sure that the pads that are placed for mounting purposes are assigned pin
numbers that will not conflict with the pins that are used for routing. For example, we
want to create a footprint for a small transformer. Thisfootprint has four pins. Pins 1
and 2 are the primary side of the transformer and pins 3 and 4 will be used for the
secondary side. In addition to these four pads, we need to place two pads to be used as
mounting holes. As long as the pin numbers assigned to these two pads are not the
same as the routing pins (ie. 1, 2, 3, or 4) we will not cause any conflicts.
                                                                                239

STARTING ROUTE CREATOR




                                   Figure 11.11

To run the ROUTE CREATOR program, open the Start Menu and go to the CIRCUIT
CREATOR program group and then click on the ROUTE CREATOR icon.

ROUTE CREATOR begins by prompting you for the name of the PC board file that is
to be routed. Select one of the demo boards, "RCDEMO1" or "RCDEMO2".
RCDEMO1 demonstrates routing a board with no pre-routed nets. RCDEMO2
demonstrates routing a board which has the power and ground lines pre-routed.

The default routing options for the board will be displayed. Observe the option
settings, but do not change any of them at this time.

Press the OK, BEGIN ROUTING button to begin routing the demo board.

The program will first display the board in its current state. Next, the program will
begin routing the board. This board will take a few minutes to route. This is a real
board. It corresponds to the sample "voice synthesizer" circuit used in the LOGIC
CREATOR schematic editor. When the routing is complete, a message box will
appear, indicating the status of the routing. Press the OK button to continue.
240

Menu and Command Selection
If you are using the keyboard, a pull-down menu may be displayed (pulled-down) by
holding the ALT key down and pressing the key indicated by the underlined character
in its name on the title-bar. Upper or lower case may be used.

When a pull-down menu is displayed, the → and ← arrow keys may be used to move
to the next menu to the right or left. The NUMLCK key must be off. Use the ↑ and ↓
arrow keys to move the menu selector up and down. Move to the FILE/OPEN
command and select it by pressing the ENTER key.

If you are using a mouse, you may pull-down a menu by moving the pointer to the
menu name in the title-bar and pressing the left mouse button and releasing it. The
menu will appear when the button is released. To select a menu item, move the pointer
to the desired item and press the left mouse button and release it. The selection is
made when the button is released. For quicker menu selections, move the pointer to
the title and press the left mouse button and do not release the button yet. Now, move
the pointer to the desired menu item and release the button to make the selection.

After selecting the FILE/OPEN command, a dialog-box will appear which is
prompting for the name of a PC board file. At this point, we can type the file name of
a file, or select one from the list that is displayed. Use the arrow keys to move the
selector to the file in the list named "DEMO.PCB" and press ENTER. This will copy
the file name from the list into the file field of the dialog-box. Now press ENTER
again to directly accept this name, or press the key to move the selector to the OK
button, then press ENTER.

When a dialog-box is displayed, clicking the left mouse button on the OK button, or
pressing the ALT-O key combination will immediately accept the values in the dialog-
box.

For a file-selection or part-selection dialog-box, pressing ENTER twice while on the
same name in the list implies that this is the name you want to accept immediately.
                                                                                 241

Getting Help
Press the F1 key to pop-up a window of help information. Notice that the help
information is specific to the current command being performed. The UP and DOWN
buttons may be used to page the help text up and down in the window. You may also
use the NEXT, PREV, or GENERAL buttons to view other help topics.

Now, select the EXIT button to close the help window. Help is always available with
the F1 key.

Navigation
We will now learn how to change the view of a PC board displayed on the screen.
Pull-down the VIEW menu. Now, move down and select the ZOOM OUT command.
The display will be redrawn at a smaller scale. You will notice that the ZOOM OUT
menu item has CTRL+PGDN listed in the right margin next to it. This indicates that
this command has a hot-key. This key combination may be used when the menu is not
displayed to directly execute this command. Let's try it. Now, hold the CTRL key
down and press the PGDN key to zoom-out. Once you are more familiar with the
program, using hot-keys will improve your productivity, especially if you do not have
a mouse. Zoom back to the original scale by pressing the CTRL+PGUP key twice.

It should be noted that if you pick the pan and zoom commands directly, you do not
need to wait for the redraw to complete before entering another pan or zoom
command. In this case, the current redraw will be stopped, and the next redraw will
begin directly.

The current coordinate of the cursor is displayed in the upper-right corner of the
screen. Use the cursor keys to move the cursor to coordinate (2.000,1.000). Follow
the track of the cursor on the screen, and watch the value in the upper-right corner
change. Notice that the active cursor (the little cross) is not always the same as the
mouse pointer position.

Holding the SHIFT key down and using the cursor keys will move the cursor one inch
at a time. Hold the SHIFT key down and use the ← and ↑ arrows to move quickly to
coordinate (0.000,0.000), the upper-left corner of the sheet.
242

The display may be panned using the keyboard by bumping into one of the edit
window edges. First, zoom in with the CTRL+PGUP key. Now, let's pan right. Move
the cursor with the SHIFT → key until it bumps the right edge of the window. The
portion of the board that was out of view to the right of the screen is now displayed.

With a mouse, the view may be panned by using the vertical slide-bar at the right, or
the horizontal slide-bar at the bottom.

Display the upper-left corner of the board at normal scale by pressing CTRL+HOME.

We will now explore how to select the layers of information that are displayed on the
screen. Execute the LAYER/MASKS command on the VIEW menu.

You will notice that each layer of the board is listed along with its type and current
conductor color. If there is not a check-mark by a layer, then items on that layer will
not be displayed. The actual colors and number of colors available will depend on
your particular hardware. The display state of each layer is changed by moving the
focus indicator to that layer and pressing ENTER to turn it on or off.

Also, this dialog-box allows you to select which masks will be displayed.

Turn off all layers except layer 1 and all masks except the silk-screen mask. Press the
OK button. Notice that only items which are on the silk-screen mask for layer 1 of the
board are displayed.

Now, let's display just the solder-side layer of the board. Select the
VIEW/LAYERS/MASKS command again. Enable the "all" layer, and layer 4 (solder-
side, last layer). Enable all the masks. Press OK. Notice that only the items that belong
to the solder-side, or go through the board, are displayed.
                                                                                  243

Setting the Colors in BOARD CREATOR
FILE/PREFERENCES
The FILE/PREFERENCES sub-menu provides commands for changing the system
configuration of the BOARD CREATOR system.

The user configuration settings are stored in the file BC32.CFG. This file must reside
in the same directory as the BC32.EXE program. The settings in this file are initially
set during installation. The commands on this menu may be used to change these
settings. The file is an ASCII text file. Although not recommended, the file may be
directly edited with a text editor.

Changes to the configuration are saved when the program is exited. Some
configuration changes may not take effect until the program is exited and restarted.

Board Colors
Use this command to set the color of the board and the select color of objects.

Application Colors
Use this command to configure the colors for the BOARD CREATOR windows, such
as the color of the rulers, status line, etc.

Cursor Grid
The cursor grid is set to 50 mils by default. You have probably noticed that the cursor
steps 50 units each time the arrow keys are pressed. Select the GRID/CURSOR
command on the VIEW menu. Set the cursor grid X and Y grid steps to "0.025" and
press OK. This sets both the cursor grid step values to 25 mils. Move the cursor about
the screen with the arrow keys. Notice that the cursor now moves in steps of 25 mils.

This completes a summary of how to start the BOARD CREATOR editor, load an
existing board, view the board, choose which layers and masks are to be displayed,
and how to set the cursor grid step values.
244
                                                                                  245



Chapter 12
Creating A Printed Circuit Board
Introduction
In this Chapter we are going to create a PC board for the "detector circuit" created in
Chapter three. Once created, it will be checked for errors, with assistance from the
program. Masks and reports about the design will be generated. This circuit is
intentionally simple and small; however, it demonstrates the basic steps by which any
circuit, regardless of size, is created.


Board specifications
           •    Board size is 3.00" x 2.00".
           •    Board has 2 signal routing layers, route 10 mil lines.
           •    Power and ground provided by power planes.
           •    Conductor masks required.
           •    Solder mask required.
           •    Silk-screen required.
           •    Drill-drawing required.

Bill of Material:
       Count Part-Name            Description
       ----------------------------------------------------------------
       1 7420                     Dual 4-Input Nand Gates
       1 7474                     Dual D-Type Flip-Flop
       1 CONN-12                  12 Pin Connector
       2 LED-RED                  Light Emitting Diode, Red
       2 R330                     330 Ohm Resistor
246

Board Design
Since this board corresponds to a schematic drawn with the LOGIC CREATOR
schematic system, we will use the update-list file produced by LOGIC CREATOR to
create our initial PC board. We will begin the new board by selecting the CREATE
FROM LOGIC CREATOR command on the I/O menu. Since we already have a board
loaded, we will be questioned as to whether or not we wish to save the changes made
to the current board. Answer NO when prompted.

We are now prompted for the name of the update-list file to be used. Select the
"MYDESIGN.UPD" file from the list. BOARD CREATOR will now read the part and
net assignment information from the update-list file and create a board with these parts
on it.

Component Placement
We now have a PC board with all the required component parts. The next step is to
move each part to its actual location on the board, then we will adjust the board to its
true size and number of layers. Although moving the parts is a manual process, we
will be assisted by the program. It will show us how the parts connect to one another.
To do this we will need a routing schedule.

Run the CHECK/SCHEDULE command from the REPORTS menu. Use a default
routing line width of 0.010" (10 mils). This will generate a routing schedule for us.
The schedule rats-nest lines are visible on the screen when the schedule mask is
enabled, or when a component is selected. Since these lines show us exactly the pin-
to-pin connections that must be routed, we will want to place the parts so the length of
these lines are as short as is reasonable.

Before we begin placing parts, we will set-up the select options for doing component
placement. Execute the SELECT command on the EDIT menu and press the O key to
pop-up the select command options. Set the select layer to ALL. Enable
COMPONENT and TOUCHING modes. Enable all the other check-boxes except the
SCHEDULE mask. By not enabling the schedule mask for selection, we will not
accidentally select schedule lines that are just passing through our select area.
Selecting a component will still select the schedule lines that belong to that particular
component. Press OK.
                                                                                   247


We are now ready to begin placing the parts. Move the cursor to location
(0.000,0.000) and zoom in twice (CTRL+PGUP). This is a good working scale for
placing this board.

For this tutorial Chapter, we will move all the components by selecting pin one of
each component. This is done to establish the coordinate numbers listed in this
tutorial. When you are working on your own, you may move a component by selecting
anywhere on the component.

Move the cursor to location (0.200,1.300) and press ENTER twice, or click with the
left mouse button. This will select component U2. Now, press ENTER, or press the
left mouse button and continue to hold it down. This will grab the component for
moving. Move the part with the arrow keys, or by moving the mouse. Notice how the
schedule lines stretch to show you how this part connects to other parts. Move until
you are at location (2.100,0.650). Press ENTER, or release the left mouse button, to
place the part at this location. If you make a mistake, press F2 (undo), and try again.

You do not need to unselect the component, it will be unselected when the next
component is selected. Using the procedure just established, place the following
components:

               Select U1 at (0.200,0.300). Move it to (1.250,0.650).
               Select R1 at (0.200,2.300). Move it to (2.100,1.500).
               Select R2 at (0.200,2.700). Move it to (1.100,1.500).
               Select D2 at (0.200,2.500). Move it to (1.100,1.700).
               Select D1 at (0.200,3.100). Move it to (2.100,1.700).

Now we have placed all the components except the edge connector. In addition to
moving it, it also needs to be rotated. Select the connector, W1, at (0.300,4.100). Grab
the connector and begin to move it just like the other components. While the connector
is on the cursor, we may press the O key (or F10) to rotate the part 90 degrees. Press
the O key three times to rotate the part a total of 270 degrees. Move to (0.150,0.450)
and place the part. Press the Z key to unselect the component. Now all the components
are placed in a reasonable location for routing the electrical connections.
248

Set True Board Size/Layers
Execute the BOARD FORMAT command on the EDIT menu. Set the number of
layers to 4, the width to 3.000", and the length to 2.000". To set a layer type, move the
layer focus indicator to the layer number and press ENTER to pop-up a menu. Select
the layer type from the menu. Set the layer types as follows:

       1 - Top conductor (already set).
       2 - Top power layer, net name "GND".
       3 - Bottom power layer, net name "+5V".
       4 - Bottom conductor (already set).

To set the net names, move the layer focus indicator to one of the power layers. Since
this is a power layer, the net name field will now become enabled. If you use the
keyboard, type ALT+N to pop-up the net name field. Type the net name into the net
field. Do this for both of the power layers.

Set the title, engineer, and other accounting fields to appropriate values. These values
will be printed on reports generated for this board. Press OK to accept the new board
definition.

How to Create a Footprint
New footprints are created directly in BOARD CREATOR, therefore, start-up
BOARD CREATOR and select New from the FILE menu. The default settings will do
for this example, therefore, press the OK button in the Format:New dialog box. Select
the Pad command from the DRAW pull down menu (or press the letter P which is the
hot key for the Pad command) and the bottom status line will display the following
information:

       ENTER: Add pad #1, Type=2, ESC:Cancel, O:Options, (0/Conductor)

We will require a pad type #3 for the footprint that we will be creating (the default
dimension for pad type #3 is 0.062" round with a 0.031" diarneter hole).

To select this pad type, press the letter O to pop-up the Pad Options dialog box:
                                                                                    249

The current pad type selected will be highlighted in the above dialog box. Also, the
size, shape, and hole size will be displayed for the current pad type selected. Select
pad type #3 from the dialog box above and the dimensions for that pad should be
displayed as the following:




                                     Figure 12-1

Press the OK button to accept this pad type. Notice that the bottom status line says that
we are about to Add pad #1 (or pin #1) of pad Type 3. The pads will be placed on the
0/Conductor layer (which is Layer 0 and the conductor mask) because these pads will
need to go through all the layers of the board.

If you are going to change the PAD defination you need to change System Pad as well
as board table. Make sure you keep the same pad number.

Next, move to location (1.000,1.000) and click the left mouse button to place a pad at
this location (or press the ENTER key). This pad will have been assigned a pin
number of 1. The bottom status line will now show the next pad's pin number that will
be placed:
250

       ENTER: Add pad #2, Type=3, ESC:Cancel, O:Options, (O/Conductor)

Move to location (1.000,1.100) and place another pad. This will be pin number 2 of
our footprint. Continue to place the remaining twelve pads at the following locations:

               Location              Pln #
               (1.000,1.200)         3
               (1.000,1.300)         4
               (1.000,1.400)         5
               (1.000,1.500)         6
               (1.000,1.600)         7
               (1.300,1.600)         8
               (1.300,1.500)         9
               (1.300,1.400)         10
               (1.300,1.300)         11
               (1.300,1.200)         12
               (1.300,1.100)         13
               (1.300,1.000)         14

Notice that the pads are being placed in the order that they are numbered (in the
manufacturer's specifications). Once all of the pads have been placed, select the
Line/Curve command from the DRAW menu.

We will now outline this footprint with lines placed on the silkscreen mask. Note:
These lines will be painted (or silkscreened) onto the surface of the PC board when it
is manufactured and will assist the technician when inserting the components into their
proper locations. The silkscreen lines do not affect the board electrically.

First, we must select the silkscreen mask as the current mask for placing lines. To
change the current layer/mask for lines, press the letter O to pop-up the Line Options
dialog box:

In the Line Options dialog box, select Silkscreen for the Mask and then press the OK
button to accept this change. Move the cursor to location (0.950,0.950) and click the
left mouse button (or press the ENTER key if you are using the keyboard) to begin the
line. Move to location (0.950,1.650) and click the left mouse button (or press the
                                                                                  251

ENTER key) again to place this line. Now move to the following locations and place
the remainder of the lines on the silkscreen mask for this footprint:

When you have finished, press the right mouse button (or press the ESC key) to cancel
placing any more lines for the footprint. The final item that needs to be placed to
complete the footprint is a component reference. Select the Component Ref command
from the DRAW pull down menu. Move the cursor to location (1.100,0.850) and click
the left mouse button (or press the ENTER key) and the following dialog box will
appear allowing you to enter a component reference:

The default component reference (U1) will do for this example, therefore, press the
OK button to accept this value. The component reference U1 should now appear
above the footprint. Now we must save our footprint. From the EDIT menu choose the
Select command and the bottom status line will display the following information:

       ENTER:Start Select, Touching Area, ESC:Cancel, O:Options, (Layer=0)

Move the cursor to the location (0.850,0.750) and press and hold the left mouse button
(or press the ENTER key if you are using the keyboard). Next, drag the mouse to the
location (1.450,1.800) and release the left mouse button (or use the arrow keys to
move the cursor and press the ENTER key once more) and all of the pads, lines, and
component reference that we have just placed to create our footprint will become
selected. After selecting these objects, choose the Save Symbol command from the
FILE menu and the following dialog box will appear:

Enter the name test.pcs in the File field of the above dialog box. Note: The name given
to your footprint must be valid DOS file name. Each footprint is saved as a separate
file with the extension pcs. The extension pcs will be automatically appended to the
name that you enter for your footprint, therefore, it is not necessary to type the
extension. Any other extension that you try to enter will be ignored when the footprint
is saved.
252

Routing the Board
We are ready to route the conductor lines that make the desired circuit. Before we
begin routing the board, we will run the CHECK/SCHEDULE command on the
REPORTS menu again. This is done for two reasons. First, we have just done a major
placement of the board. With the new component locations, it may be possible to
generate a more efficient routing schedule. Also, we have just added a power and
ground layer to the board. There is no longer a need to schedule lines for the "GND"
and "+5V" nets. Pads assigned to these nets will connect directly to the power and
ground layers.

Now we will begin routing the board. Execute the LINE command on the DRAW
menu. From our specification, the width of the routing lines is 10 mils. The current
line width is displayed in the bottom status line. If this is not 0.010", press the O key,
or click on the status line with the mouse pointer, to display the line drawing options
dialog-box. Set the line width to 0.010" (10 mils).

For this board, we will use the component-side for the mostly horizontal routes, and
the solder-side for the mostly vertical routes.

We will route the shortest lines first. Since we can see from the routing schedule lines
shown on the screen which pads need to be connected together, look for some short
ones.

Move to coordinate (1.600,1.500) and press ENTER, or click with the left mouse
button. The schedule line from this pad is now high-lighted, showing us the
connection that needs to be made. Since this route will be mostly vertical, we will
route this line on layer 4, the solder side of the board. Notice that the status line
indicates the current edit layer is layer number 1. Press F9 to toggle to routing layer to
layer 4. Now move to (1.600,1.700) and press ENTER, or click with the left mouse
button. This will complete the first route. Notice that the schedule line is now gone,
indicating that this route is complete. Press ESC, or click the right mouse button to
stop drawing this line. If you make a mistake while still drawing a route, press
BACKSPACE to backup (instead of UNDO).

Now let's do another route. Move to (2.600,1.500), ENTER, move to (2.600,1.700),
ENTER, and ESC.
                                                                                      253

Got the hang of it? Routing lines on your own will actually be much easier. You will
work directly from the screen instead of reading coordinates from a book. Now let's
route a line with some bends in it. Move to (2.100,1.500), ENTER, move to
(2.100,1.400), ENTER, move to (2.150,1.350), ENTER, move to (2.150,1.200),
ENTER, move to (2.100,1.150), ENTER, and ESC.

Now, press F9 to toggle back to layer 1. Route lines between the following points.
More instruction will be given when we add a via for the first time.

       Layer 1:        (2.100,0.650), (2.200,0.650), (2.300,0.750), (2.400,0.750).
       Layer 1:        (0.150,0.450), (0.800,0.450), (1.000,0.650), (1.250,0.650).
       Layer 1:        (0.150,0.550), (0.800,0.550), (1.000,0.750), (1.250,0.750)
       Layer 1:        (0.150,0.650), (0.800,0.650), (1.100,0.950), (1.250, 0.950).
       Layer 1:        (0.150,0.750), (0.800,0.750), (1.100,1.050), (1.250,1.050).
       Layer 1:        (0.150,0.850), (0.800,0.850), (1.150,1.200), (1.450,1.200),
                       (1.500,1.150), (1.550,1.150).

The next line will require a via. Route the line as before, up to the point where a via is
noted. At the point just ENTER again, or click the left mouse button. This is the same
as drawing a line segment with no length. This will add a via at this point, and toggle
the routing layer. Continue drawing the remainder of the line on the other layer.

       Layer 1:        (0.150,0.950), (0.750,0.950), (0.900,1.100), VIA, (1.350,1.100),
                       (1.400,1.050), (1.550,1.050).

Remember to start each line on the proper layer.

       Layer 1:        (0.150,1.050), (0.750,1.050), VIA, (0.900,0.900), (1.450,0.900),
                       (1.500,0.850), (1.550,0.850).

       Layer 1:        (0.150,1.150), (0.650,1.150), VIA, (0.650,1.000), (0.850,0.800),
                       (1.400,0.800), (1.450,0.750), (1.550,0.750).

       Layer 1:        (1.550,1.250), (1.800,1.250), (1.950,1.100), (2.200,1.100),
                       (2.350,0.950), (2.400,0.950).
254

       Layer 1:        (1.250,1.150), (1.400,1.150), (1.450,1.100), (1.700,1.100),
                       (1.950,0.850), (2.100,0.850).

       Layer 1:        (1.100,1.500), (1.350,1.500), (1.500,1.350), (2.200,1.350),
                       (2.300,1.250), (2.400,1.250).

       Layer 1:        (0.150,1.250), (1.000,1.250), (1.100,1.350), (1.350,1.350),
                       (1.500,1.200), (1.750,1.200), (1.950,1.000), (2.200,1.000),
                       (2.200,0.800), (2.000,0.800), (2.000,0.650), (2.100,0.650).

The remaining two routes deserve some special attention. Even though this board has
power and ground planes, the planes themselves must receive power from some
external connection. For this board, one pin on the edge connector is assigned to net
"GND", and another one is assigned to net "+5V". Since these pins do not have holes,
they do not connect to the power planes directly, and must be routed to a point that
does. Otherwise the board will not be powered.

Power lines are normally routed with a wider than normal line width. Set the line
width to 0.050" (use the O key to pop-up the line dialog-box). Now, route the
following power lines:

       Layer 1:        (0.150,1.350), (0.850,1.350), (0.900,1.400), (0.900,1.650),
                       (0.950,1.700), (1.100,1.700).

       Layer 1:        (0.150,1.550), (0.750,1.550), VIA, (0.750,1.300), (0.800,1.250),
                       (1.250,1.250).

This completes the routing of the board. Notice that there was never a need to refer
directly to the update-list, or any other lists. All the information necessary to place and
route the board was presented directly on the screen where you were working.

Adding Text to the Board
Next, we will learn how to add notational text strings to the board. Text is often added
to directly identify the layer of the mask, the company name, copyright notice, etc. Be
careful when adding text to a conductor layer. The text will be etched in copper on the
actual board. Do not place the text where it will touch any conductor lines.
                                                                                   255


Select the DRAW/TEXT command. Move to (1.000,0.300) and ENTER to begin
adding a text string. In the dialog-box, enter "Copyright (c) 1994 by Me" for the text,
layer 1, mask SILK-SCREEN, size 0.062", angle 0, font NORMAL, and mirroring
NONE. Press OK to add the text. The text will appear on the board at the location of
the cursor and have attributes which match these settings.

Move to location (2.800,1.300). Press ENTER and add the string "Component Side" to
the CONDUCTOR mask with an angle of UP. Put "GND" on power layer 2. Notice
how the display adjusted to show a power layer. Put "+5V" on power layer number 3.

Move to (2.75,0.550) and add "Solder Side" on layer 4 with an angle of DOWN, and
mirroring set to RIGHT-TO-LEFT. This will make this text readable when it is viewed
from the back-side of the board.

Add the string "Assembly" on the ASSEMBLY DRAWING mask of layer 1 (angle 0,
no mirroring). Likewise, add the string "Drill Drawing" to the DRILL DRAWING
mask of layer 1.

You may add any additional text as desired. Set the angle, size, and mirror factors as
desired in the dialog-box.

Check the Layout
To check our board for routing completeness, run the CHECK-SCHEDULE command
from the REPORTS menu. If you have completed the board correctly, a message "All
scheduled routes complete" will appear, otherwise the schedule lines for any
uncompleted routes will be generated. If you have routed two nets together, creating a
short, the location of the problem will be displayed directly on the screen.

If any errors are detected, try to correct the problem and re-run the check until there
are no errors.

Printing the Masks
Now that the board is complete, and has passed all the error checks, it is time to print
the masks for this board. If you have not yet selected the printer device, use the SET-
UP PRINTER command on the FILE menu to select your printer device and set the
256

basic printing options.

Execute the FILE/PRINT command. The dialog-box for printing allows you to queue
up to ten masks to be printed. Queue the following masks:

               1.   Layer 1, Conductor mask.
               2.   Layer 1, Silk-screen mask.
               3.   Layer 1, Assembly drawing.
               4.   Layer 1, Drill Drawing.
               5.   Layer 2, Conductor mask.
               6.   Layer 3, Conductor mask.
               7.   Layer 4, Conductor mask.
               8.   Layer 4, Solder mask.

Enable TARGETS, BANNER, and BORDER. Set the other options as desired. If your
printing device requires you to change paper between each print (as required by some
plotters), enable the PAUSE option. Review the settings and make sure a check mark,
indicating that the queue slot is enabled for printing, appears next to each of the first
seven queue slots. Press OK to begin printing the masks.

For most boards, it is necessary to set-up the printing parameters for a board only
once. The printing set-up parameters are saved with the board.

Generating Reports
From the commands on the REPORT menu, generate a PARTS LIST, a NET LIST
(pads only option), and a SUMMARY report. If you have a printer, you may direct the
reports directly to the printer. Compare these reports with the schematic net and parts
list. They should agree.

Saving the Board
Now we will save our board to a file. Select SAVE AS command from the FILE
menu. Enter "MYDESIGN" for the file name and press OK. This will save the board
into the file "MYDESIGN.PCB".
                                                                                   257

Exit the Program
We are finished with the board for now. Select the EXIT command on the FILE menu,
or just press ALT-X, to exit the program.

Becoming a Power User
The Chapter you have just completed was designed to familiarize you with the basic
steps in using BOARD CREATOR to create a board. To become an advanced user of
BOARD CREATOR, and to use its features to your best advantage, the following self-
training procedure is suggested.

Start the BOARD CREATOR program and use the FILE/NEW command to create a
new board (any reasonable size). Go through each of the commands on the menus, one
at a time. For each command, display the help information with the F1 key. Study the
options for each command and practice each of these operations on the board. It is not
necessary to construct a real or complete board. Just use the board as a scratch area to
practice the commands. For example, practice the DRAW/TEXT command by placing
text of various sizes, angles, mirroring, layers, etc. on the board. Move a text string.
Move and rotate an area of text strings. Update a text string. Delete a text string. Do
this for each command and you will quickly become a power user of BOARD
CREATOR.

In the Chapter just completed, you were instructed how to perform each step in the
construction of a simple board. Therefore, there was little or no opportunity to make
changes to the board during the tutorial. In the real world, you will need to make
changes, move things around, and correct mistakes. Changes are made with the
SELECT command. In fact, it is the default command. Just press ESC to exit the
current command, and you are running the SELECT command.

Before any object on a board can be changed, it must first be selected. For a detailed
description of the SELECT command, and how it is used to move, drag, stretch, and
update objects, refer to the EDIT/SELECT command in the next chapter. Please
practice using the select command. It will be used often.

Refer to the next chapter for a complete user's reference to each of the BOARD
CREATOR commands.
258

ICONS Defination in Board Creator
UNDO
      This is a UNDO ICON. Clicking this ICON will undo the last operation you
      performaed. For example, if a line, a pad or for that matter any item was
      accidently deleted, Choosing UNDO ICON would replace one or all of the
      deleted items.

Options
      Choosing this ICON will display the options for the current command that is
      selected. This is the same as Choosing the letter O or clicking on the bottom
      status line with the mouse.

Delete
      Choosing this ICON on the tool bar will delete the current selected object(s).
      First Select the object and press this ICON to delete it.

Layer View/Configuration
      Choosing this ICON will allow you to configure the colors that are assigned to
      the various layers and masks of your PC board. These colors are saved with the
      PC board file (.peb) and will not affect any existing or new PC boards that are
      created. This is the same as selecting the Layers/Masks command from the
      VIEW menu.

Toggle Layer ( HOT KEY F9 )
      Selecting this option will toggle the current layer to the opposite layer pair. For
      example, if you are placing lines (or track3 on the top component side of the
      board, Choosing this ICON will toggle the current layer to the bottom solder
      side. This is the same as Choosing the F9 key or selecting the Toggle Layer
      command from the EDIT menu.

      Choosing this ICON will make the Select command the current command. The
      Select command is the most commonly used command in BOARD
      CREATOR. This command is used for moving, updating, copying and deleting
      objects from your PC board.
                                                                                  259

Load Symbol ( Ctrl + L )
     This ICON will load symbol ( Footprint ) from the footprint Library.
     PCSVIEW will show the selection of all the footprints available in the system.

Pad ( P )
     Choosing this ICON will make the Pad command the current command. Pads
     are used when creating footprints or whenever a hole is needed on the PC
     board. There are fifty different pad types available in BOARD CREATOR.

Line/Curve ( L )
     This ICON will allow you to place Line/Curve on your board. The current line
     width, type, layer and mask that is selected for lines will be displayed in the
     bottom status line when this command is selected.

Text ( T )
     When you are ready to place assembly or design notes on your PC board, you
     can press this ICON to select the Text command. Text may be placed on any
     layer or mask, however, you should be extremely careful when placing text on
     a conductor mask because the text will be etched in copper (just as the lines or
     track) and may cause shorts on the board.

SOLID ( D )
     To place a solid area of copper on a conductor mask, select this ICON in the
     tool bar. There are three options for the type of solid that can be placed on your
     PC board design. These options are: solid, mesh and cross hatch.

VOID ( V )
     To place a void area on your board, click on this ICON with the mouse. A void
     is only used by the auto-router program ROUTE CREATOR. If an area is
     marked as a void area, then the auto-router will not route lines (or track) or
     place vias in that region.
260

COPPER POUR ( R )
      In order to pour copper on a conductor mask of your PC board design, you
      may select this option. The Region Pour command is similar to the Solid Area
      command except that it will not place copper on top of existing routes, pads
      and vias.

ARC ( A )
      Choosing this ICON will allow you to place an arc on your PC board. An arc
      may be placed on any layer or mask, however, it should not be used for routing
      the pins (or pads) of your components together.
                                                                                  261



Chapter 13
Board Creator Reference
This is a reference section. It lists all BOARD CREATOR menus and their commands.
A brief explanation follows each command on how it is generally used. Read through
this section to familiarize yourself with all the BOARD CREATOR commands. Please
refer to it while you create new boards to answer your questions. This section along
with the context sensitive help should be able to answer all your questions.

BOARD CREATOR Commands
File Menu
       The file menu provides commands for loading and storing PC boards, foot-
       print symbols, printing, printer set-up, displaying program version information,
       exiting the program, and executing DOS commands. You normally start and
       end an BOARD CREATOR session by using commands on this menu.

Open (Ctrl+O)
       Use this command to load an existing board file for editing, viewing, or
       printing. Upon loading a file, the program will automatically display the board
       in the edit window. Select the file to be loaded from the dialog-box that
       appears. If the name of the board that you want to load is in the list-box, you
       may press ENTER twice or double click with the mouse to directly make the
       selection. If you had experienced a power loss, you will be prompted that a
       "checkpoint" file exists and you will be asked if you wish to load this
       "checkpoint" file instead. More about this auto-backup feature is described in
       the SYSTEM menu section. All BOARD CREATOR PC board files must have
       the extension ".PCB".
262

New (Ctrl+N)
      Use this command to create a new PC board. If a board is already loaded and
      changes have been made, you will be allowed to save it before making the new
      board. Fill in appropriate values in the format dialog-box that appears, and
      press OK to start the new design.

Save (Ctrl+S)
      Use this command to immediately store a board to its file. Any previous
      version of this file is replaced.

Save As (Ctrl+A)
      Use this command to store the current board to a different or new file. The file-
      picker dialog-box, showing the current file name of the board, will be
      displayed. Enter the new file name and press OK to save the board.

      If a file of the same name already exists, you will be given the option of
      backing-up that file, writing over that file, or canceling the command.

Load Symbol (Ctrl+L)
      Use this command to load a foot-print symbol file, and place the symbol on the
      board.

      The file-picker dialog-box, showing a list of symbol files will be displayed.
      Enter the name of the symbol file to be loaded and press OK. The selected
      symbol will appear on the cursor. Move the cursor to the desired location and
      press OK to add a copy of the symbol to the board.

      While the symbol appears on the cursor, you may press the F10 key to rotate
      the symbol in 90 degree increments or press "O" to mirror the symbol to the
      solder side of the board.
                                                                                    263

Save Symbol (Ctrl+V)
     Use this command to create a new symbol or to update an existing symbol.
     First, select all the objects on the current board that you want to be included in
     your symbol, then execute this command. You will be prompted for the name
     of the file to hold the symbol. Enter the file name and press OK. The selected
     objects will be stored in the symbol file. To load this symbol, refer to the
     FILE/LOAD SYMBOL command.

Print (Ctrl+P)
     Use this command to make hard-copy prints of the current board masks.

     A dialog-box will appear, allowing you to queue up to ten different mask
     specifications to be printed. To enable or disable a queue slot for printing, click
     on the queue number. All the queued items that show the enable check-mark
     by its queue number will be printed when you press the OK button.

     Printing has many options to choose from:

     Format:
     Selects the page size and quality of the print. This is the size of the paper/film
     in the printer, not the board size.

     Port:
     Selects the destination of the printing. This can be a hardware port or a file(s).

     Output to File:

     Separate files:
     If checked, and the output port is a file, then a separate file will be generated
     for each queued entry. Otherwise, a single file will contain the output of all the
     queued entries. The print file names are constructed by using the base file
     name of the board and adding extensions of "G01", "G02", etc. for as many
     files as required.
264

      Method:
      Specifies how to process the queued items. Use DIRECT/TILE for one mask
      per sheet. If a mask will not fit on a single sheet, it will be printed on multiple
      sheets (tiled). PANELS will print as many masks on a single sheet as will fit.
      This can greatly reduce the cost of photo-plotting. If COMPOSITE is selected,
      all the queued items will be printed as a single print. This is useful if you want
      to print multiple layers as a single image.

      Layer:
      Selects the PC board layer to be used in making the print.

      Mask:
      Selects the type of mask to be printed.

      Scale:
      Specifies the scale to use in generating the print.

      Show PAD:

      Oversize:
      This is used for solder, paste, and power-plane masks. It specifies the amount
      to increase the diameter of pads/cut-outs when they are printed.

      Mirror:
      Allows the print image of the mask to be mirrored about the X or Y axis.
      Allowable values are: NONE, RIGHT-TO-LEFT, TOP-TO-BOTTOM, or
      BOTH AXIS.

      Pan:

      Offset X/Y:
      Allows you to specify an offset to be applied to the image when the print is
      generated. The print will be shifted by this amount when it is output. There is
      usually no need to apply an offset.
                                                                               265

Banner:
If checked, the configured banner along with the mask layer number, mask
type, and time/date stamp will be printed just outside the bottom board area.
This helps to document the print.

Border:
If checked, a rectangular border will be printed outside the board area.

Targets:
If checked, alignment marks (targets) will be printed just outside the board area
at each corner of the board.

Pause:
If checked, the program will pause before it begins the printing of each queued
item. This gives you a chance to prepare the printer (such as changing the
paper). You will be required to confirm that it is OK to proceed.

Negative:
If checked, program will automatically reverse your printing image.

Draft:
This command is use full when you are using PAN Plotter. If checked, program is
automatically print border instade of all over the solide image. This command is use
full to reducing time and cost of Pan Plotter.

Rotate:
If checked, the mask image will be rotated 90 degrees when it is printed. This
command considers the orientation you select.

Set the printing parameters as desired for each queued slot. Make sure that all
the queued items you want to print at this time have the enable check mark
showing. Press OK to start printing. If you need to interrupt printing once it
has started, press the ESC key.

If you do not want to print at this time, but you want to save the settings, press
the SAVE button. This allows you leave the dialog box without canceling the
setting changes.
266


      For most boards, you only need to define the printing parameters you want to
      use once. The printing parameters are saved as part of the board data when the
      board is saved to a file.

Setup Printer (I)
      Use this command to select the printer device and set the following printer
      controls.

      Printer Name:
      Specifies the type of the printer device.

      Paper Size/Source:
      Specifies the page size and relative quality to use from a list of page sizes
      available for this device.

      Properties:
      This command is useful to change the configuration of Printer you choose, you
      can also change default settings of printer for good quality printout.

      Orientations:Portrait/Landscape
      This command is useful to change the orientation of paper when ready to print.

      Port:
      The remainder of the controls are used to specify the destination of the print
      output and the configuration of the printer port.

Pan Plotter
      PAN Plotter is a specific device to print the images using PAN. You have to
      configured your Pan Plotter device here so you can print out put on Pan plotter.

Photo Plotter
      Photo Plotter is specific device to print the images sing laser photo lights. You
      can generate your print file on this format using this command.
                                                                                     267

Preferance

Paths/Options
    Use this command to configure the default file paths and other program
    operating controls for the BOARD CREATOR program:

    Drawings Path:
    Specifies the default path for PC board files.

    Scratch Path:
    Specifies the default path for temporary scratch files.

    Check Point Path:
    Specifies the path of where check point files are to be stored. These are
    temporary files that are used to recover data in case of a power failure or
    system failure.

    Banner:
    The name entered in the Banner field of the Paths/Options dialog box will
    appear in any report generated (such as a bill of materials, net-list, pin-list, etc.)
    and will also appear in the title block of your schematic. The default banner is
    "Your Name Here".

    Plotter PCF:
    Use this command to configure your Photo Plotter or Pen Plotter to generate
    print file on specific format.

    Grid Cursor:
    If Checked, You can see the “+” cursore on your current PCB file edit window.

    Check Point Sec.:
    Specifies the time interval (in seconds) for automatically saving the current
    board to a check-point file. Setting the checkpoint time to zero (0) disables this
    feature.
268

      Please note that all path names must end with the system path name separator,
      "\". The program must be able to take the given configured path name and
      append a file name and extension to make a complete path name for a file.

Edit System Pad Table
      Use the command to define the shape of the pads that will be used when a new
      board is created. A dialog-box will appear, letting you define pad types.
      Changing these pad definitions will not affect the shape of the pads on the
      current board.

Load System Pad Table
      Use the command to replace the definition of the current board's pad table with
      the configured default pad table definitions. After selecting this command, you
      will be warned that the pad table for the current board will be replaced with the
      currently configured system pad table. You will be required to verify that this
      is what you want to do.

Colors Board Colors
      Use the command to set the color of the board and the select color of objects.

Application Colors
      Use this command to configure the colors for the BOARD CREATOR
      windows, such as the color of the rulers, status line, etc.

System Colors
      Use this command to configure the colors for the BOARD CREATOR
      SYSTEM, such as the color of menus, dialog-box windows, borders, etc.

Select Colors
      Use this command to choose color for selection area. E.g. If you choose Blue,
      your selection area will appear blue when select an object.
                                                                                 269

Exit (Alt+X, X)
     Use this command to exit the program and return to the system prompt. If
     changes have been made to the current board and not saved, you will be given
     the option of saving the board before exiting.

File Names
     The bottom of the file menu will list the file names of the last four boards that
     were referenced. You may directly open one of these boards by selecting it
     from the menu. This command provides fast access to the boards that you have
     used recently.

Edit Menu
     The edit menu provides commands for changing a board.

Board Format
     Use this command to change the board size, number of layers, layer types,
     accounting information, and other overall board design parameters. A dialog-
     box will appear, showing the current values of these items.

     Change the board format values as desired, then press OK.

Undo (F2)
     If you make an editing mistake, use this command to undo the command you
     just executed. The board will be restored to the way it was prior to executing
     the previous command. Executing undo again will restore the mistake.

Cut (Shift+Del)
     This command is used to delete objects from a board, placing them in the paste
     buffer. Select the objects that you want to delete, then execute this command to
     delete the selected objects.

     The deleted objects are placed in the paste buffer, replacing its previous
     contents. To retrieve objects from the paste buffer, refer to the EDIT/PASTE
     command.
270

Copy (C)
      Use this command to make copies of objects on a board.

      Select the objects that you want to copy, then execute this command. A copy
      of all the selected objects will be placed in the paste buffer, replacing its
      previous contents. To retrieve objects from the paste buffer, refer to the
      EDIT/PASTE command.

Paste (Shift+Ins)
      Use this command to retrieve objects stored in the paste buffer.

      After starting this command, a rectangle indicating the area of the objects
      currently in the paste buffer will appear on the cursor. Move the cursor to the
      location where you want a copy of these objects to be placed, and ENTER.
      Continue to place more copies, or ESC to cancel the command.

      If you want to paste the objects to a layer other than the layer they were copied
      from, press the O key or click with the mouse pointer on the status line to pop-
      up the paste dialog-box. This dialog-box will allow you specify the layer you
      want the objects pasted to.

Delete (Del)
      Use this command to delete objects from a board.

      Select the objects that you want to delete, then execute this command to delete
      the selected objects.

      The deleted objects are not placed in the paste buffer. For placing deleted
      objects in the paste buffer, refer to the EDIT/CUT command.

Update (U)
      This command is used to change the values assigned to objects on the board.
      For example, if you want to change the width of a line, or the size of text that
      is already on the board, use the update command. This command may also be
      used to review the values currently assigned to an object, without making any
      changes.
                                                                                 271


     To update an object, first select the object that you want to update, then
     execute this command. This command may also be executed by pressing
     ENTER twice while the cursor is on a selected object, or by clicking the left
     mouse button while pointing to a selected object.

     A dialog-box specific to each selected object will appear. Change the object's
     values as desired, then press OK. If more than one object is selected, pressing
     CANCEL will stop the update sequence.

Select (S)
     The select command is the default BOARD CREATOR command. That is,
     when no other command is active, the select command is active by default.

     The select command is used when you want to make changes. It is used to
     point out which objects you want to change. Before an object can be changed,
     it must first be selected. Once selected, an object may be deleted, moved,
     stretched, or updated.

     For example, if you want to delete a line from a board, first select the line you
     want to delete, then press the DEL key. If you want to move an object on a
     board to a new location, first select the object, then grab it with mouse and
     move it to the new location.

     To select an item, or group of items, first pick the EDIT/SELECT command,
     or just ESC the current command to start it by default.

     To select a single object, place the cursor on top of the object you want to
     select and press the ENTER key twice. With the mouse, just point at the object
     and click the left mouse button. When an object is selected, it will appear on
     the board in the configured select color.

     To select more than one object, move the cursor to one corner of the area that
     bounds the objects and ENTER. Now, move to the other corner and ENTER
     again to select all the objects within this area. With the mouse, hold down the
272

      left button and move the mouse to stretch-out the desired area. Release the
      button to select the objects.

      Press the O key or click the left mouse button on the status line to pop-up the
      select parameters dialog-box. This dialog-box allows you to control which
      items will get selected and which items will not. You may enable/disable
      selection by any combination of layer, mask, or object type.

      You can choose between a selection method of touching or bound by, as
      indicated in the bottom status line. When touching is active, any matching
      objects touching the selection area will be selected. When bound-by is active,
      only the matching objects completely bound by the selection rectangle will be
      selected.

      You can also choose between a selection method of component or flat. When
      component mode is active, selecting any portion of a component will cause all
      the objects that belong to this component to be selected as well. When flat
      mode is active, individual objects within a component may be selected.

      You may unselect by making a new selection, selecting in an area on the
      screen where there are no objects, or by executing the EDIT/UNSELECT
      command.

      Once an object is selected, the following operations may be applied:

      CUT, COPY, ERASE, UPDATE - Refer to the specific command.

      Move/Drag:
       Press ENTER while the cursor is within the select area indicator, and then use
      the arrow keys to move/stretch the selected objects. ENTER again to place the
      objects (stop moving). With the mouse, press the left mouse button down and
      drag the objects to the new location. Release the mouse button to place the
      objects.
                                                                                 273

     Stretch:
     Lines may be stretched by selecting only the portion of the line(s) that you
     want to move. For example, if you only select one tip of a line, then that end of
     the line will stretch as it is moved. The other end of the line will remain
     anchored. This technique may be used to quickly reshape conductor routes.

     As you can see, the select command is a very convenient and powerful
     command that works in combination with other commands. All editing
     changes are done through the use of the select command.

Unselect (Z)
     Use this command to unselect all objects on a board.

     You may also unselect all objects by selecting in an area of the board that has
     no objects.

Toggle Layer (F9)
     Use this command to change the current layer being edited to its other routing
     layer pair. This command is used to quickly flip between the two layers you
     are using for the mostly horizontal and vertical routes.

Trace NET
     Using this command you can select trace you want to highlight, by doing this
     you can highlight whole trave on the PC board file.

Change All
     Use this command to change all of one or more of the following:

     Change all lines of a given width to a new width.
     Change all pads of a given pad type number to a new type.
     Change all vias of a given pad type number to a new type.
     Change all text of a given size to a new size.
274

Pad Table
      Use this command to define pad shapes for this board. A dialog-box will
      appear, showing the current pad definitions. Define the pad shapes as required
      for this board, and press OK.

      Changing a pad definition will cause all pads on the board that refer to this pad
      number to be changed to the new definition.

Draw Menu
      The draw menu provides commands for drawing the objects that appear on PC
      boards. Boards are made by placing part foot-print symbols on a board and
      wiring the parts together. Also, reference text and additional graphic effects
      may be added to enhance the drawings and further document the board.

      For adding part foot-print symbols to a board, refer to the FILE/LOAD
      SYMBOL command.

Component Reference (N)
      Use this command to add a component reference to the current board. A
      component reference consists of a reference name which is shown on the board
      (such as U1, U2, R4, etc.) and a part number which may optionally be shown
      on the board. Component references are used to tie all the separate objects of a
      single component together, and give them a name.

      You will not normally have any need to add a component reference directly.
      Component references are included in the foot-print symbol definitions, and
      will be added as part of a symbol when the symbol is placed on the board. If
      you are making your own symbols, then you will want to include a component
      reference as part of the symbol. Note: that the component reference may only
      be one letter (i.e. CONN is not a valid component reference.)

      To add a component reference, select this command, move the cursor to the
      location where you want the reference to appear and press ENTER. A dialog-
      box will appear, allowing you to enter the reference name, part name, and to
      set parameters which control the appearance of the reference name. Fill in the
      fields and press OK to add the reference.
                                                                                   275


     You may continue to add more references by positioning the cursor and
     pressing ENTER. Press ESC to end this command.

     Component references are normally added on the silk-screen mask of layer 1,
     but may also appear on the bottom layer for boards which have SMD devices
     on the bottom of the board.

Pad (P)
     Use this command to add a component pad to the current board.

     You will not normally have any need to add a pad directly to a board. Pads are
     included in the foot-print symbol definitions, and will be added as part of a
     symbol when the symbol is placed on the board. If you are making your own
     symbols, then you must include the pads that define the symbol.

     To add a pad, select this command, move the cursor to where you want the pad
     to be located, and press ENTER. If the current pad selected is not the pad that
     you desire, press the letter O or click the left mouse button on the status line to
     pop-up the pad options dialog box. The dialog-box that appears will allow you
     to select which one of the possible pad shapes you want to add. You must also
     specify the layer, mask, component pin-number, and other related parameters
     for the pad. Fill in the fields, and press OK to accept these options. Note: as
     you add a pad, a pin number is assigned to that pad. The next pad's pin number
     is displayed in the status line as ADD PAD #. When creating a new footprint
     symbol, it is recommended that you place the pads in the order that they are
     numbered in the design specification.

     Pads which go through the board must be added on layer zero (all layers). If
     the layer is not zero, then the pad will appear only on that specific layer.
     Examples of pads which are only on one layer are the fingers of an edge
     connector, and the pads of an SMD part.

     Add the pad to the CONDUCTOR mask. Only use a mask other than
     conductor if the pad is being used as some graphic effect, and is not part of the
     electrical circuit.
276


      If you do not find a pad of the required type and shape, refer to the EDIT/PAD
      TABLE command. This command will allow you to define your own pad
      shapes.

Line/Curve(L)
      Use this command to draw line and/or curve segments on a board. This
      command is used primarily to draw the routing lines that connect parts together
      electrically.

      To draw a line segment, select this command, move the cursor to where you
      want to start drawing one end of the line and ENTER to begin the segment.
      Notice that the current line parameters, such as line shape, line width, layer
      number, and mask are displayed in the bottom status line. If the settings are not
      what you want, press the O key or click the left mouse button on the status line
      to pop-up the line dialog-box. This dialog-box is also used to choose the pad to
      be used when vias are added, and whether or not blind/buried-vias are to be
      used. Set the line parameters to the desired values and press OK.

      Now, move to the other end of the line segment and ENTER to complete this
      segment. If you want to continue drawing another line segment from this
      location, move to the end of the next segment and ENTER. To start a line in a
      new location, ESC, then move to the new location and repeat the procedure.

      When you want to add a via as part of the line drawing process, move the
      cursor to where you want the via and press ENTER twice. This is the same as
      drawing a line with no length. Adding a via will toggle the current layer to its
      associated layer pair. This allows you to quickly add electrical routes by
      drawing line segments, adding a via, and continuing the line on the other layer
      without having to stop and set the layer directly each time a via is added.
                                                                         277




                           Figure 13.1.1

When you are routing conductor lines and your board has a routing schedule
(see CHECK/SCHEDULE on the REPORTS menu), the schedule lines will
show you which points on the board have not yet been routed. To route one of
these connections, start the line at one of the two pads linked by a schedule
line. The schedule lines from this pad will be high-lighted, helping to show
you exactly what needs to be connected. Draw an appropriate connection route.
When you make connection to the other pad indicated by the schedule line, the
schedule line will be deleted, indicating that the connection is now complete.
When you are routing conductor lines between parts, always make sure that
you are drawing the lines/vias on the CONDUCTOR mask.

While the line command is active, you may press F5 to toggle the line drawing
type. This is a quick way of changing the line shape without popping up the
line parameters dialog-box.

If you make a mistake while you are routing a line, press the BACKSPACE
key (instead of UNDO). This will remove the line segment or via you just
added, and position you to where you were when you started this segment. You
may backspace, one segment at a time, all the way back to where you started
278

      this trace (up to twenty times). This feature works only while you are drawing
      a route. Once you press ESC to begin the next route, you will have to use
      UNDO or the SELECT command to make corrections.

      Another feature of the line command is the ability to break an existing line into
      two separate segments. To break a line, position the cursor to the point on a
      line where you want to break it and press the B key.

Text (T)
      Use this command to add reference text to a board.

      Move the cursor to the location of where you want the lower-left corner of the
      text line to appear and ENTER. A dialog-box will appear which lets you enter
      the text, set the size of the text, and set other text related parameters. If you are
      adding text to a conductor mask, make sure the text does not overlap any of the
      electrical networks, causing a short. Text added to a conductor mask will be
      etched in copper just like the pads and routes.

Solid Area (D)
      Use this command to draw rectangular solid areas on a board. The rectangular
      areas may be filled solid, with a grid mesh, or with a cross-hatch pattern.

      To draw a solid area, select this command, move the cursor to where you want
      to start drawing one corner of the area and ENTER to begin drawing the
      bounding rectangle.

      Notice that the current solid parameter settings are displayed in the bottom
      status line. If the settings are not what you want, press the O key or click the
      left mouse button on the status line to pop-up the solid dialog-box. Set the
      parameters to the desired values and press OK.

      Now, move to the other corner of the solid area and ENTER to complete the
      bounding rectangle. If you want to continue drawing more solids, just repeat
      this process. Press ESC to end this command.
                                                                                   279

Void Area (V)
     Use this command to draw rectangular void areas on a board. A void area is
     used in conjunction with the ROUTE CREATOR product to indicate an area
     the router is to avoid. It does not restrict you from manually routing lines in
     this area.

     Notice that the current void parameter settings are displayed in the bottom
     status line. If the settings are not what you want, press the O key or click with
     the mouse pointer on the status line to pop-up the void dialog-box. Set the
     parameters to the desired values and press OK.

     To draw a void area, select this command, move the cursor to where you want
     to start drawing one corner of the area and ENTER to begin drawing the
     rectangle.

     Now, move to the other corner of the void area and ENTER to complete this
     rectangle. If you want to continue drawing more voids, just repeat this process.
     Press ESC to end this command.

Region Pour (R)
     Use this command to fill the unused area of a rectangular region with a net
     grid, such as power or ground. This command is normally used after all other
     routing is complete.

     A dialog-box will appear, allowing you to set the width of the lines to be used
     for the grid, the spacing of the grid lines, and the net name assigned to the grid.
     Make the settings and press OK.

     To "pour" an area, move the cursor to where you want to start drawing one
     corner of the pour area and ENTER. Now, move to the other corner of the pour
     area and ENTER. The unused regions within this rectangle be filled with
     conductor grid lines. The grid will connect to pads (if not blocked) that have
     the specified net name. All other pads will be avoided.

     For boards which use edge connectors, you may need to manually route lines
     from the connector to a point on the grid to "hook-up" the grid to its power
280

      source. You may also need to route lines to pads of the net which could not be
      reached by the grid. Use the CHECK/SCHEDULE command on the
      REPORTS menu to show you which routes are not complete.

      All the grid lines of a single pour operation are treated as a single component.
      The SELECT command may be used in "component" mode to select the entire
      grid for editing. Use "flat" mode if you need to edit individual lines of the grid.

Arc (A)
      Use this command to draw an arc, circle, or ellipse on a board.

      To draw an arc, select this command, move the cursor to where you want the
      center of the arc and ENTER.

      Notice that the current parameter settings are displayed in the bottom status
      line. If the settings are not what you want, press the O key or click the left
      mouse pointer button on the status line to pop-up the arc dialog-box. Set the
      parameters to the desired values and press OK.

      Now, move the cursor. You will see the shape of a circle/ellipse segment as
      you move the cursor. Move the cursor until you have the shape of the arc you
      want and ENTER. If you want to continue drawing more arcs, just repeat this
      process. Press ESC to end this command. Do not use the arc command to draw
      portions of conductor lines. Use arcs for graphic effects, and in drawing the
      component outlines of foot-print symbols.

View Menu
      The view menu provides commands for selecting the current view of a board.
      You may pan, zoom, or select specific layers/masks of the board for viewing.

      In addition to the commands that are directly on the menu, the following
      commands may also be used to pan the view.

      The display will automatically pan when the cursor is moved with the arrow
      keys, and the edge of the edit window is bumped.
                                                                                 281

     To pan with the mouse, use the slide-bars along the right and bottom edges of
     the window to select a desired view. Clicking the left mouse button on the
     slide-bar arrows will pan a small amount in that direction. Clicking in the area
     between the arrows and the slider will pan a full page. Grab the slider with the
     mouse and drag it to select the view directly. The size of the slider indicates
     the portion of the board that is currently in view.

     To center a point on the board in the view, move the cursor to the point and
     press the SHIFT+NUMERIC 5 key.

Layers Masks        (M)
     Use this command to select the layers and masks of a board that you want to
     view, and set the display colors of the conductor masks. This command is also
     used to select the display colors for conductor layers and masks.

     Set the display layer, masks, and colors you want to view in the dialog-box that
     appears.

Grid Cursor (G)
     Use this command to define the cursor motion snap-grid, the reference grid,
     and to set various cursor parameters.

     The cursor grid controls the stopping location of the cursor. The cursor grid is
     set to 50 mils by default. This means that the cursor coordinate will always be
     on a multiple of 50 mils. Disabling the cursor grid allows you to move in 1 mil
     increments.

     The reference grid is for reference only, and is not part of the actual board. It
     may be turned on to aid in the placement of parts or the alignment of other
     objects. The reference grid will not appear on hard-copy prints of the board.
     Also, the reference grid does not affect the cursor motion.

     Normally, the cursor coordinate represents the distance from the upper-left
     corner of the board. Enabling a relative cursor allows you to measure relative
     to any coordinate. Although you can set the relative cursor parameters from
     this dialog-box, the easiest way is simply to move the cursor to the coordinate
282

      from which you want to measure and press the "." (period) key. This will set
      the relative cursor at this point. When a relative cursor is active, the coordinate,
      displayed in the upper-right of the screen will appear reversed. Just press the
      period key again to return to absolute mode.

Pan Up (PgUp)
      Use this command to pan the drawing up. The pan direction refers to the
      change in the view, not the direction that the board appears to move. For
      example, panning up indicates that you want to view more of the area toward
      the top edge of the board.

Pan Down (PgDn)
      Use this command to pan the board view down.

Pan Right (Shift+>)
      Use this command to pan the board view right.

Pan Left (Shift+<)
      Use this command to pan the board view left.

Pan Point (F4)
      Use this command to pan a specific coordinate to the center of the edit
      window. A dialog-box will appear, letting you specify the coordinate.

Pan Center (NunLock+#5)
      Use this command to pan the current cursor location to the center of the edit
      window.

      To use this command effectively, it must be executed from the keyboard. If
      you pick this command with the mouse, the board cursor will probably not
      positioned about the desired pan point.
                                                                               283

Locate (K)
     Use this command to locate text strings on a board, and optionally select the
     object if found. A dialog-box will appear, letting you specify the string to be
     searched for. The string will be searched for without regard to upper or lower
     case.

Snap To PAD (F)
     Using this command you can let your objects snap with the PAD while
     drawing.

Zoom Home (Ctrl+Home)
     Use this command to view the upper-left corner of a board at the standard
     zoom scale.

Zoom In (Ctrl+PgUp)
     Use this command to zoom in on the board view. Objects in the view will
     appear bigger and more detailed; however, you will be able to see less area of
     the board sheet.

Zoom Out (Ctrl+PgDn)
     Use this command to zoom out on the board view. Objects in the view will
     appear smaller and less detailed; however, you will be able to see more area of
     the board sheet.

Redraw (CTRL+R)
     Use this command to redraw the board at its current pan and zoom scale.

Reports Menu
     The report menu provides commands for showing the current status of your
     board, checking your board for errors, generating formal production and
     engineering design reports, and for generating a routing schedule.

     All of the printed report commands will display a dialog-box which allows you
     to specify the destination of the report, a file or the printer. You can also
     choose between a formal or informal report. A formal report will be formatted
284

       with page banners, time and date stamps, page numbers, and page breaks. An
       informal report will just contain the raw data of the report. Formal reports are
       intended to be read by people. Informal reports are usually read by other
       programs.

Status
       Use this command to display the current number of objects in your design,
       memory utilization, etc. The report is displayed on the screen only.

Drill-Hole
       Use this command to generate a drill-hole report. This report will list the
       coordinate of each hole on the board and the size of the hole. You can specify
       the location of the coordinate system origin for the report.

       The following is an example portion of a drill-hole report:

               Measured from LOWER-LEFT corner
               X offset: 0, Y offset: 0

               # X Y DIA.
               1 1650 1950 31
               2 1650 1850 31
               3 1650 1750 31
               4 1650 1650 31
               5 1350 1650 31
               6 1350 1750 31
               7 1350 1850 31

Pad Locations
Use this command to generate a PAD Locations report. This report will list the
coordinate of each hole on the board and the size of the hole. You can specify the
location of the coordinate system origin for the report. .exl is ths default extention of
the file name.

The following is an example portion of a PAD Locations report:
                                                                                   285

             Measured from LOWER-LEFT corner
             X offset: 0, Y offset: 0

             # X Y DIA.
             1 1650 1950 31
             2 1650 1850 31
             3 1650 1750 31
             4 1650 1650 31
             5 1350 1650 31
             6 1350 1750 31
             7 1350 1850 31

Net-list
      Use this command to generate a net-list report. This report will list each net, or
      sub-net, and all the component pads that belong to this net. You may optionally
      specify that the line segments and vias that belong to each net's conductor trace
      are to be listed also.

      The following is an example portion of a net-list report:

                     NET_LIST
                          NET 552, RS232OUT
                                PAD ( 6700, 2100, 0) CONN1:3
                                PAD ( 4900, 2700, 0) U003:3
                                PAD ( 5700, 2600, 0) C003:1
                          END_NET
                          NET 561, +15V
                                PAD ( 6700, 1800, 0) CONN1:6
                          END_NET
                          NET 566, CTS
                                PAD ( 6700, 1900, 0) CONN1:5
                                PAD ( 5900, 1300, 0) U006:6
                          END_NET
                          ...
                     END_NET_LIST
286

Part-List
      Use this command to generate a parts list report. This report will list each
      component on the board, its assigned part, and its reference name.

      The following is an example portion of a part-list report:

                             PART_LIST
                                  SW2 DSW16
                                  C008 0.1M
                                  U001 CTS256A-AL2
                                  U007 SP0256A-AL2
                                  R001 10K
                                  R004 100K
                                  U008 74LS373
                                  SW1 DSW16
                                  CONN1 RS232-25PIN
                                  ...
                             END_PART_LIST

Summary
      Use this command to generate a summary report. This report will list the
      number of objects on the board, the different line widths, pad shapes, drill
      holes, etc. that occur on the board.

Excellon Drill Tape
      Use this command to generate an NC drill tape (file) for driving an
      EXCELLON drilling machine. Note: this file is in a 3-3 format (i.e. three
      integer, three decimal).

Check/Schedule
      Use this command to check your design for logical routing errors and/or to
      generate a routing schedule for the board. A dialog-box will appear, allowing
      you to specify the default routing line width, and names of any nets that require
      a special width, such as power and ground nets. Enter or adjust the widths and
      press OK to check and re-schedule the board.
                                                                                287

    If the board is complete, you will receive a message "All scheduled routes
    complete".

    If no errors are found, but the board has not been completely routed yet, you
    will receive a message indicating the number of routes that are not yet
    complete.

    If errors are detected, a dialog-box giving details of the exact problem will
    appear. Also, the location of each error will be flashed on the board. All of the
    detected errors may be reviewed from this dialog-box, one at a time.

Check/Clearance
    Use this command to check your design for proper object-to-object clearance.
    A dialog-box will appear, letting you specify the minimum clearance distance
    between various object types. Enter or adjust the values and press OK to begin
    the check. If errors are detected, a dialog-box giving details of the exact
    problem will appear. Also, the location of each error will be flashed on the
    board. All of the detected errors may be reviewed from this dialog-box, one at
    a time.

I/O Menu
    The I/O menu provides commands for importing data from, and exporting data
    to, other CAD systems.

Create from LOGIC CREATOR
    Use this command to create an initial PC board from the data supplied b an
    LOGIC CREATOR schematic update-list file.

    A dialog-box will appear, requiring you to specify the name of the LOGIC
    CREATOR update-list file to be used. Select the file and press OK. The
    program will proceed to create the initial board per the information contained
    in the update-list file. The board will contain all the parts and net assignment
    information. You will need to place the parts, adjust the board to the actual
    size, and route the board.
288

Update from LOGIC CREATOR
      Use this command to update a PC board with the latest data for the design from
      the LOGIC CREATOR schematic system. This command is used when
      changes are made to the schematics for a design. This will update the part and
      net name assignments to agree with the LOGIC CREATOR update-list. If
      components are added to your LOGIC CREATOR design, then the
      corresponding footprint must be added (manually) to you BOARD CREATOR
      PCB design before updating it with a newly generated LOGIC CREATOR
      update list. Note: the component reference of this newly added part must match
      the component reference assigned to it in LOGIC CREATOR.

      A dialog-box will appear, requiring you to specify the name of the LOGIC
      CREATOR update-list file to be used. Select the file and press OK. The
      program will proceed to update the board. You will need to use the
      CHECK/SCHEDULE command on the REPORTS menu to generate a new
      routing schedule, and check the board for routing completeness and possible
      errors.

Export ASCII
      Use this command to export the current board to one of the many supported
      ASCII text formats. This command allows you to supply data to other CAD
      systems, directly in that system's own file format.

      A dialog-box will appear, requiring you to specify the name of the text file to
      be exported, and to specify the target CAD system format.

Import ASCII
      Use this command to import data from other CAD systems. This command
      creates an BOARD CREATOR/LOGIC CREATOR compatible "update-list"
      file from one of the many supported ASCII text file formats.

      A dialog-box will appear, requiring you to specify the name of the text file to
      be imported/converted, and the CAD format of the import file.

      An update-list file will be created from the import file. If any errors are
      detected during the conversion, they will be displayed. The update-list file is
                                                                               289

     itself an ASCII text file with extension ".upd". If necessary, it may be edited
     with a text editor.

     Once you have an update-list file, even if you make it by hand with a text
     editor, it may be used with the CREATE FROM LOGIC CREATOR or
     UPDATE FROM LOGIC CREATOR commands on the I/O menu.

Help Menu
     This menu allows you to get on-line help on any command or menu. It is
     organized like a book, with an index of the chapters and detailed information
     in each chapter.

Context/Index - F1
     This option gives you the index of the help manual. Move your mouse pointer
     above the word you need help on. If the arrow changes to a pointing hand then
     help is available, and you can access it by clicking on that word.

     This is the most important feature of the HELP menu. It allows you to get
     direct help on the specific command you are interested by highlighting the
     command and then pressing F1.

Using Help
     This is a tutorial on how to use the help menu of BOARD CREATOR. Please
     go through this tutorial as many times as you need. It will help you became a

About Board Creator (H)
     Use this command to display the copyright notice and current version/release
     number of the program.
290
                                                                                 291



Chapter 14
Creating a THD Footprint
(Through Hole Device )
Introduction
In this Chapter we will create a footprint for the part IRF530, a power mosfet. We
need to have all the mechanical data for the device which are available on its data
sheet, which is included in program's help file (look for IRF530). Take a look at the
data sheet right now and notice the two diagrams and all the marked dimensions on the
table underneath. The figure on the left is the front view of the package, and the one
on the right the side view. We will probably need to use both to extract the
information we need.


Determining the hole diameter of a pad
First we need to find the dimensions of the cross section of a lead in order to
determine the size of the hole we will need in the pad. All the dimensions we will be
using are in mil, thousandth of one inch. The lead is rectangular in shape and has
maximum dimensions 22(J)X25(D). So the hole needs to be at least 25 mil in
diameter. Now lets find the maximum size of the hole. This is determined by
dimension L and its minimum value 45 mil. If the hole is more than 45 mil there is a
chance for the wider portion of the lead close to the body of the component to go
through the hole. So it makes sense to use the average of the min and max values
(25+45)/2 = 35 mil.

Determining the overall diameter of a pad
This overall diameter includes the hole and the annular ring of cooper around it. What
limits the size of the overall diameter of the pad is the pin to pin spacing. From the
data sheet, dimension G, 95 mil minimum and 105 mil maximum, the pin to pin
spacing. We will again use the average which is 100mil. So we can have up to 95 mil
292

overall pad diameter which will leave 10 mil spacing from pad to pad. At 95 mil we
will have an annular cooper ring of thickness 95 - 35 = 60 mil. For regular pads for
250 mw components the annular ring is 19 mil. For this transistor an annular ring of
70 mil will be sufficient. This will allow a 30 mil clearance from pad to pad. This is
good because at low voltages we will be able to route a 10 mil cooper trace between
two pins with 10 mil clearance. So the decision is 70 mil overall diameter.

Drawing the Footprint
The next step is to draw the three pads for the transistor. Launch BOARD CREATOR,
and start with a new board. Let the size of the board be the default one 6X3. Since the
pins are going to be spaced 100 mil apart, lets set our display grid to 100 mil. Click on
VIEW, then on GRID/CURSOR. Now you have in front of you the REFERENCE
GRID/CURSOR dialog box as shown below.




                  Figure 14.3.1 REFERENCE GRID/CURSOR
                                                                                   293


The cursor grid default is 50 mil. Because we will have to take measurements down to
5 mil in the example we will set it to 5 mil. Click on the down pointing arrow to the
right of the Standard box currently displaying the word Grids. A menu will be pull
down. Select 5 mil.

Next we will set the display grid. Click the Standard box under the display grid to pull
down its menu. Select 100 mil. The setting of 100 mil will help up draw the outline of
the part easily. Click on the Display/Grid box to enable it, and OK the dialog box. As
soon as the dialog box closes the display grid is drawn on the board.

Time to select and place the pads. Select EDIT/PAD TABLE an the PAD TABLE:
BOARD dialog box pops up.




                            Figure 14.3.2 PAD TABLE
294


We need a pad with hole diameter of 35 mil and overall diameter of 70 mil. This table
lists 10 different pad types. The first one is exactly what we need and it is also
selected. Notice the hole box has the diameter of the hole. The component, solder and
inner boxes contain the outer diameter of 70 mil. Click on the other nine pads and
examine their characteristics. When ready to continue click back on pad type #1 and
then the OK button to save the settings and exit.

Drawing the PADS
Now move your cursor somewhere around (1.000,1.000) so that you have lots of room
to move around. Select PAD from the Draw menu. Notice the status bar and its
message. It reads ENTER: Add pad #1, Type =1, ESC:Cancel,
O:Options,(0/Conductor). This means that the first pad we will place will be for pin #1
of the device, and the currently selected pad is type 1. Move the cursor to the
neighborhood of 1,1 and press CTRL + PAGE UP twice to zoom in close. No place
the cursor on (1.000,1.000) and press ENTER. The first pad is drawn and the status
bar now tell us that the next one would be the pad for pin no. 2. Looking at the data
book, pin# 2 is on the right of pin #1. So we need to move 100 mils to the right. here is
a quick way of doing it. Press F to make the cursor snap on the pad you have just
placed. Then press the period key on the key board. This makes the center of pad #1
your relative (0.000,0.000) origin displayed on the right of the menu bar. Now simply
use the right arrow 100 mils to the right and place the second pad by pressing ENTER.
Repeat this and place the third pad too.

Drawing the Outline
Now it's time to draw the outline on the silk screen. Press ESC to stop the
DRAW/PAD command. Select DRAW/LINE. Then click on the status bar and select
layer 0 and the SILK SCREEN mask. As soon as you OK the dialog box the color of
the silk screen (normally yellow) will appear on the right-most end of the menu bar.
Now the question is from where should we start drawing? Examining the data sheet
again I notice that dimension B is the length of the package. Its average length is 392.5
mil, and half of it 196.25 mil. My strategy is as follows. I will start from the center of
pad no.2, I will move out along the width of the device the average of dimension R
(95mil) and then I'll move 196.25 to the right, then up by the dimension C(175mil)
and then continue around to finish the outline. Go ahead and do it. Use the period on
                                                                                    295

every corner to reset your relative origin for measuring convenience. To start drawing
the line you need to press enter, the status bar reminds you of that.

Now let's label the pins. Again from the data-sheet, pin 1 is the gate. So select TEXT
from the DRAW menu, place your cursor under pad 1, between the edge of the cooper
and the outline and press enter. Type G in the STRING box of the dialog box and
press enter. A G appears at the right place but it's too large. Press ESC to stop the
DRAW/TEXT command. Click on the G to select it. It changes color when selected.
Now press U for Update and in the TEXT UPDATE dialog box that appears change
the size to 32 mil. Click OK to make the change effective, and repeat the same
procedure for the other two pins.

Now we need to assign the footprint a reference designator. Looking up the ANSI
Standard help file for reference designator, for transistors the designator is Q. From
the DRAW menu select COMPONENT REF , then move the cursor in the middle of
the package outside the outline and press ENTER. The component ref dialog box
appears with the default designator U1. Replace U1 with Q1 and click Ok to close the
dialog box.

Naming and Saving the Footprint
Finally its time to save our footprint. Click ESC to escape from the last command.
This puts you in the SELECT command which is the default. Move your cursor above
the upper left corner of the outline and select both the outline and the reference
designator by dragging the mouse towards you. Once selected click on FILE and then
on SAVE SYMBOL. The save symbol dialog box appears. We will give it a footprint
name that conforms with standard packaging numbering systems. For this device
Motorolla lists a CASE number, and an Transistor Outline number. We will use the
TO-220AB number because this is standardized through JEDEC and applies to all
manufacturers. The footprint name has to comply with DOS file name convention of
eight characters long. We will name it TO220ABV. The V at the end stands for
vertical. You see, you may want to create another footprint for the same package when
it is installed flat on the board and its metallic tab screwed on it. Then that footprint
will be named TO220ABH, where H is for horizontal. So, go ahead and name your
device and press ENTER to save it.
296

Testing the Footprint
Now it is time to test it. From the FILE menu select LOAD SYMBOL, and type in
TO220ABV. If everything went all right the symbol will appear on the tip of your
cursor. Press CTRL+ PAGE DOWN to zoom out so you can see better. Then move
the outline wherever you want and place it by pressing ENTER.

This concludes this Chapter. Now you know how to create parts, symbols and
footprints. You can use the footprint you have just created for many different parts. By
just looking at the two data-sheets in the help file, you can use this footprint for eight
different parts. So, it pays to take your time and create a perfect footprint because you
do this once and can use it for many parts over and over again. And every time its
drawn its done with the same accuracy you originally put in when you created it.
                                                                                    297



Chapter 15
Creating a SMD Footprint
(Surface Mount Device)
Creating a footprint for a surface mounted device (or SMD) is very similar to the
procedure explained in the last section. Let's try an example. Start-up BOARD
CREATOR and choose New from the FILE menu to begin a clean board. The default
settings will do for this example. Place the cursor at the origin or coordinate
(0.000,0.000) and select the Zoom-in command from the VIEW menu. This will give
us a better working zoom level. Also from the VIEW menu select the Grid command
and adjust the grid snap to 25 mils.

Now we are ready to begin creating the SMD footprint. The footprint that we will be
creating is a standard SO-8 (eight pin) plastic IC package. From the DRAW menu
choose the Pad command and press the letter O to display the pad options. In the pad
options dialog box, choose pad type #9 (which is a 0.060" x 0.025 rectangular pad),
set the layer to layer #1 and set the mask to conductor. Press the OK button to accept
these options. Notice that the bottom status line displays the following information:

        ENTER: Add pad #1, Type=9, ESC: Cancel, O: Options, (1/Conductor)

The status line information tells us that we are about to add pad #1 (or pin #1) of a pad
type #9 on the top conductor layer. Move the cursor to location (1.000,1.000) and
press the ENTER key to place a pad at this location. Notice that the bottom status line
now displays the following:

        ENTER: Add pad #2, Type=9, ESC: Cancel, O: Options, (1/Conductor)

The pin number that will be assigned to the next pad that is placed has been
automatically incremented for you. Therefore, you must pay special attention to this
298

status line information while creating new footprints. Place the remaining seven pads
at the following locations (in the order shown):

                       Location               Pin#
                       (1.000,1.050)          2
                       (1.000,1.100)          3
                       (1.000,1.150)          4
                       (1.200,1.150)          5
                       (1.200,1.100)          6
                       (1.200,1.050)          7
                       (1.200,1.000)          8

Note: The pad spacing and numbering information is normally supplied by the IC
manufacturer. The next step is to show the outline or shape of the footprint by placing
lines on the silk-screen mask. From the DRAW menu choose the Line/Curve
command and press the letter O to display the line options. In the line options dialog
box, select layer #1 and set the mask to silk-screen. Press the OK button to accept
these options. Now, move the cursor to location (0.950,0.975) and press the enter key
to begin the line at this coordinate. Move to location (0.950,1.175) and press ENTER
to place this line on the top silk-screen layer. Continue to place lines by moving to the
following coordinates and pressing the ENTER key:

                       (1.250,1.175)
                       (1.250,0.975)
                       (1.125,0.975)
                       (1.125,1.025)
                       (1.075,1.025)
                       (1.075,0.975)
                       (0.950,0.975)

This completes the outlining of the footprint. The final object that needs to be placed
on this footprint is a component reference. From the DRAW menu, select the
Component Ref command and move the cursor to location (1.050,0.925) and press the
ENTER key. Press the OK button in the Component Reference dialog box to accept
U1 as the component reference for this footprint.
                                                                                     299

The last step is to save this new footprint so that it can be loaded onto a new board at a
later time. From the EDIT menu choose the Select command and move the cursor to
location (0.875,0.850) and press the ENTER key. Now move the cursor to location
(1.325,1.250) and press the ENTER key once more. You should notice that all of the
objects that were just placed to create this new footprint have become highlighted or
selected. From the FILE menu, select the Save Symbol command and enter the desired
name for this new footprint in the save symbol dialog box. Each footprint exists as a
separate file with an extension of PCS.
300
                                                                                  301



Chapter 16
Creating GERBER Photo Plotter File
One of the main objective to create printed circuit board (PCB) using Board Creator is
to fabricate printed circuit board (PCB). All PCB fabricator need the information in a
electronic form to create the mask negatives and drill file. The industry is following
one format very extensively is called GERBER FILE format to create the mask
negatives. The company called GERBER was pioneer in Photo Plot equipment. The
file is ASCII representation of X and Y coordinate of Pads and Lines and is also called
Laser Photo Plot files or simply Photo Plot files. Now there are several companies
manufacture the same equipments using different technology. EIA( Electronic
Industry Association) adapted Gerber file format as the standard format for photo
plotting industry and called RS274D file format. Later they revised the format and
came out with RS274X format. The RS274D file format has only photo-plotting
information such as X and Y co-ordinate for Pads and Lines. Separate file is used for
Aperture information. The RS274X has aperture information embedded in the same
file. Board Creator supports both of these format. Please check with your printed
circuit board (PCB) fabricator company which file format it accepts.

Photo-plotter Set-Up
       Use this command to generate a report of the photo-plotting set-up
       requirements for the current board. This report will list the draw and flash
       aperture assignments used to generate the printed output. To use this
       command, the current print device must be a photo-plotter type device.

       Notice! This report is generated based on the current print queue set-up
       parameters. If you change the print device, or the print queue parameters after
       making this report, then print your masks, the report may not be valid. Print
       your masks first, then run this report.
302

One Step Photo-plot Creation
      To create Photo Plot files, go to FILE Pull-down menu and select Photo
      Plotter. After software prepares the initial set up information, you will see the
      following Dialog Box.




                       Figure 16-1. Photo plotting setup

      This dialog-box allows you to queue up to ten different mask specifications to
      be plotted. To enable or disable a queue slot for plotting, click on the queue
      number. All the queued items that show the enable check-mark by its queue
      number will be plotted when you press the OK button.

Plotting has many options to choose from:
      Separate files:
      If checked, a separate file will be generated for each queued entry. Otherwise,
      a single file will contain the output of all the queued entries. The print file
      names are constructed by using the base file name of the board and adding
      extensions of "G01", "G02", etc. for as many files as required. This option
                                                                              303

allows you to create each separate file for each mask. For example there will
be separate file for Conductor mask, Silk screen mask, solder mask and so on.
Each file will have a extension G01, G02, G03 etc. The separate file option is
useful when you want to see each mask for accuracy purpose using View
Creator. Creating one file makes it easier to send to printed circuit board (PCB)
Fabricator.

Film size:
This is the size of the film, not the board size Usually film size is one (1) inch
larger in all four directions than printed circuit board (PCB) size.




Method:
Specifies how to process the queued items. Use DIRECT/TILE for one mask
per sheet. If a mask will not fit on a single sheet, it will be printed on multiple
sheets (tiled). PANELS will print as many masks on a single sheet as will fit.
This can greatly reduce the cost of photo-plotting. If COMPOSITE is selected,
all the queued items will be printed as a single print. This is useful if you want
to print multiple layers as a single image.
304

      Layer:
      Selects the PC board layer to be used in making the film.




      Mask
      Selects the type of mask to be printed.




      Show PAD
      When queuing a Show PAD for printing or plotting, you will have three
      options: No, Solid and PAD + Hole. When you get your printed out put you
      can see effect of this options.

      When you selecting NO in show PAD options program doesn’t print PAD on
      your currently selected layer same thing when you select SOLID program
      show you SOLID PADs in print layer and When you select PAD + Hole
      options program give you actual hole size of the PAD you used on PCB file by
      selecting this options you can get PAD + Hole in your print file.
                                                                            305

Oversize
This is used for solder, paste, and power-plane masks. It specifies the amount
to increase the diameter of pads/cut-outs when they are plotted. The industry
normal is 10%.

Mirror
Allows the print image of the mask to be mirrored about the X or Y axis.
Allowable values are: NONE, RIGHT-TO-LEFT, TOP-TO-BOTTOM, or
BOTH AXIS. The default is None and make sure NONE is selected unless you
want to be mirrored for any other reason.




Offset X/Y
Allows you to specify an offset to be applied to the image when the plot is
generated. The plot will be shifted by this amount when it is output. There is
usually no need to apply an offset. The default is 0.0 and make sure it is 0.0,
unless you want to offset for any other reason.

Banner
If checked, the configured banner along with the mask layer number, mask
type, and time/date stamp will be printed just outside the bottom board area.

Border
If checked, a rectangular border will be printed outside the board area.

Targets
If checked, alignment marks (targets) will be printed just outside the board area
at each corner of the board.
306

       Negative
       This is used for solder, paste, and power-plane masks. If you need the plot file
       in a reverse image.

       Set the plotting parameters as desired for each queued slot. Make sure that all
       the queued items you want to plot at this time have the enable check mark
       showing. Press OK to start. If you need to interrupt creating files once it has
       started, press the CANCEL key.

       If you do not want to plot at this time, but you want to save the settings, press
       the CLOSE button. This allows you leave the dialog box without canceling the
       setting changes.

       For most boards, you only need to define the plotting parameters you want to
       use once. The plotting parameters are saved as part of the board data when the
       board is saved to a file.

Gerber File Format

       274X (RS274X)
       This type of format has aperture information embedded in the photo-plot files.

       274D (RS274d)
       This is a older format and it does not put aperture information in the photo-
       files.

Aperture List File
Board Creator creates Aperture file regardless you choose RS274D or RS274X file
format. The extension for this file is .APT.

The following is an example of an aperture list that was generated by Board Creator
for the demonstration PC board called demo.pcb:
                                                                             307

     *** Aperture List for DEMO ***

     PAD DEFINITIONS          FLASH CODE
     ===============          ==========

     ROUNDED   50 50 D10
     ROUNDED   62 62 D11
     RECTANGLE 62 62 D12
     RECTANGLE 54 300 D13

       LINE DRAW WIDTHS           FLASH CODE
       ================          ==========

             5 (mils)                   D14
             10 (mils)                  D15
             25 (mils)                  D16

Excellon Drill File
     Beside Photo-Plot files ( Extension G01, G02 ) and Aperture File ( Extension
     APT) printed circuit board (PCB) Fabricator also needs Excellon Drill File (
     Extension EXL).Go to REPORT menu and select Excellon Drill File The
     following Dialog Box will show.
308

      This report will list the coordinate of each hole on the board and the size of the
      hole. You can specify the location of the coordinate system origin for the
      report.

      The following is a partial list of Drill file created by Board Creator for
      DEMO.PCB

             %
             T01
             X008Y005X013Y005X018Y005X023Y005X024Y0065X025Y0
             08X025Y009X025Y01X025Y011X025Y012X025Y013X025Y0
             14X025Y015X025Y016X025Y017X025Y018X025Y019X025Y
             02X025Y021X025Y022X025Y023X025Y024X025Y025X025Y
             026X025Y027X022Y027X022Y026X022Y025X022Y024X022
             Y023X022Y022X022Y021X019Y021X019Y022X019Y023X01
             9Y024X019Y025X019Y026X019Y027X017Y027X017Y026X0
             17Y025X017Y024X017Y023X017Y022X017Y021X014Y021X
             014Y022X014Y023X014Y024X014Y025X014Y026X014Y027
             X012Y027X012Y026X012Y025X012Y024X012Y023X012Y02
             2X012Y021X009Y021X009Y022X009Y023X009Y024X009Y0
             25X009Y026X009Y027X01Y027X007Y027X007Y026X007Y0
             25X007Y024X007Y023X007Y022X007Y021X004Y021X004Y
             022X004Y023X004Y024X004Y025X004Y026X004Y027X005
             Y027X005Y017X004Y017X004Y016X004Y015X004Y014X00
             4Y013X004Y012X004Y011X007Y011X007Y012X007Y013X0
             07Y014X007Y015X007Y016X007Y017X009Y017X009Y016X
             009Y015X009Y014X009Y013X009Y012X009Y011X012Y011
             X012Y012X012Y013X012Y014X012Y015X012Y016X012Y01
             7X014Y017X014Y016X014Y015X014Y014X014Y013X014Y0
             12X014Y011X017Y011X017Y012X017Y013X017Y014X017Y
             015X017Y016X017Y017X019Y017X019Y016X019Y015X019
             Y014X019Y013X019Y012X019Y011X022Y011X022Y012X02
             2Y013X022Y014X022Y015X022Y016X022Y017X02Y017X02
             05Y016X021Y015X0205Y014X02Y013X024Y013X0235Y018
             X024Y019X0235Y023X024Y024X02Y0245X0205Y0255X031
             Y026X031Y027X031Y025X031Y024X031Y023X031Y022X03
             1Y021X031Y02X031Y019X031Y018X031Y017X031Y016X03
                                                309

1Y015X031Y014X031Y013X031Y012X031Y011X031Y01X03
1Y009X031Y008X0325Y005X0375Y0065X039Y005X0405Y0
09X042Y0095X0435Y0105X045Y0145X045Y0155X045Y016
5X045Y0175X045Y0185X045Y0195X045Y0205X045Y0215X
045Y0225X045Y0235X042Y0235X042Y0225X042Y0215X04
2Y0205X042Y0195X042Y0185X042Y0175X042Y0165X042Y
0155X042Y0145X0375Y0145X036Y013X036Y0165X04Y017
X043Y0205X043Y022X048Y0225X05Y0225X05Y0235X05Y0
215X05Y0205X05Y0195X05Y0185X05Y0175X05Y0165X05Y
0155X05Y0145X053Y0145X053Y0155X053Y0165X053Y017
5X053Y0185X053Y0195X053Y0205X053Y0215X053Y0225X
053Y0235X051Y026X051Y0205X047Y02X048Y0175X047Y0
145X037Y0215X037Y0235X04Y025X021Y01X0205Y009X02
Y008X01Y017M30

---------------------------------------------
Measured from LOWER-LEFT corner
237 total drill holes, 1 different sizes.
T01 = 31 mil diameter hole
310
                                                                                     311



Chapter 17
HOW to Section for Board Creator
How to Rotate Object on the PC Board
Board Creator allows you to Rotate the Part ( Object, or Footprint ) in the increment of
90 Degrees. Firsr select the Part and then without moving the mouse, Press and Hold
the left mouse button to pick up the part, but do n't move the part. Continue to hold the
left mouse button and Press F10 or Key O. Keep pressing F10 or key O untill you get
your desired position and orientation.

Moving Part from One Layer to Another Layer
PART on the PC board can be moved from one layer to another by Cutting, Copying
and Pasting sequence. When a PART (or PARTS) is cut or copied, it is placed into
paster buffer. Select the Paste and the bottom status line will display the following
information:

       ENTER: Paste, ESC: Cancel, O: Mask, F10: Rotate

According to the bottom status line information, pressing the letter O will allow you to
specify the destination mask of where the pasted objects will be placed. Press the letter
O while pasting objects on your board. The layer where the pasted objects will be
placed can be selected from the Paste:Destination Mask dialog box. Here mask really
represent Layer rather than mask. This will be easy with the example, if two PADSs
have been cut, one PAD was on the conductor mask of Layer 1 and the other PAD was
on the solder mask of Layer 1. When the Paste command was selected and the letter O
was pressed, Layer 2 was selected as the destination layer. Now the one PAD will be
pasted to the conductor mask of Layer 2 and the other PAD will be pasted to the solder
mask of Layer 2. Only the layer changes for the pasted items, not the mask.

If Layer zero is selected as the destination layer, then the pasted objects will appear
exactly as they did before they were cut or copied. If a layer (other than Layer zero ) is
312

selected, then all of the items (that were cut or copied) will be pasted to that specific
layer.

An alternative method for moving objects from one layer to another would be to select
and update each individual object in order to change the layer or mask that the object
is currently on. However, this can be a very time consuming method for moving
objects from one layer to another.

Rotating and Mirroring a Footprint
Use Load Symbol command from File menu to select desired footprint. While the
footprint is still on cursor, the status Line shows as follows

       ENTER: Add Symbol, ESC: Cancel, F10: Rotate, O: Back/Front

At this time you have few options. Place the footprint as you see it, rotate it or Mirror
it. By pressing Enter Or left click of the mouse, the footprint will get placed on the
board as it is. Press F10 to Rotate it or Press 'O" to Mirror it.

F10 function key rotates the footprint in 90 Degree increment. "O" key puts the
footprint on the back side of the board. This will also switch silk screen on the back
side of the board also. Once the footprint has been placed on the board, you can not
mirror the footprint.

Note : If you are creating the board from Logic Creator, create mirror footprint for the
components you want on the back side of the board.

Importing a Gerber File
       Importing a Gerber file is accomplished in several steps. First, you will need
       to obtain the aperture list that was used to generate the Gerber plot files that
       you are going to import. Without the aperture list, BOARD CREATOR will
       not know what size pads and lines to use while importing the Gerber file. The
       following is a sample of the type of information that will be found in an
       aperture list:
                                                                                  313

              Flash Code Pad Definition

              D10 0.062" ROUNDED
              Dl l 0.050" ROUNDED
              D12 0.062" x 0.062" RECTANGULAR
              D13 0.030t x 0.300" RECTANGULAR
              D14 0.040" x 0.100" ELLIPTICAL

Step 1:
       The above aperture table information needs to be in a format that can be used
       by BOARD CREATOR. In order for BOARD CREATOR to use this
       information, it must be included in a printer configuration file (or PCF file).
       The printer configuration file that can be used by BOARD CREATOR for
       importing Gerber files is gerber.pcf. This file will be located in the directory
       c:\cktcrt. Using the above aperture list information, add the following
       information to the gerber.pcf file (using a text or ASCII editor):

               D15 0.005"
               D16 0.010"
               D17 0.025"
               D18 0.100"

              Flash Code Line Width

              PAD FLASH ROUNDED 62 62 "D10*\13\\10\"
              PAD FLASH ROUNDED 50 50 "D11*\13\\10\"
              PAD FLASH RECTANGLE 62 62 "D12*\13\\10\"
              PAD FLASH RECTANGLE 30 300 "D13*\13\\10\"
              PAD FLASH ELLIPSE 40 100 "D14*\13\\10\"
              WIDTH 5 "D15*\13\\10\"
              WIDTH 10 "D16*\13\\10\"
              WIDTH 25 "D17*\13\\10\" WIDTH 100 "D18*\13\\10\"

Note: You may want to delete all of the existing pad and line width definitions in the
gerber.pcf file so that you do not duplicate any of the flash code definitions.
314

Step 2:
      The next step will be to enter the pad definitions (from the aperture list) into
      the System Pad Table of BOARD CREATOR. First, copy your BOARD
      CREATOR configuration file (bc32.cfg) to a temporary file. One way to do
      this is to start-up a DOS shell and type the following at the DOS prompt:

             CD\CKTCRT (and press ENTER)
             Next, type the following at the DOS prompt:
             COPY bc32.cfg bc32.tmp (and press ENTER)

      This is done so that you can easily restore your original System Pad Table
      definitions when you have finished importing the Gerber files. To modify the
      System Pad Table to include the pad definitions that are used in the Gerber
      plot files, select Edit System Pad Table from the FILE/Preferences menu.
      Enter each pad definition (from the aperture list) in the System Pad Table.

      The above dialog box shows the first pad (from the aperture list) entered in the
      System Pad Table as pad #1. Enter the next pad's definition (from the aperture
      list) as pad #2 and so on. After you have finished entering all of the pad
      definitions, we can begin importing the Gerber

Summary:
      This is a short summary of the steps that will take place when BOARD
      CREATOR imports a Gerber file. When BOARD CREATOR encounters a
      flash code (for example D10) in the Gerber plot file, it searches the printer
      configuration file (gerber.pcf) for a matching flash code. If the flash code is
      found, the size and shape of the pad (0.062" ROUNDED) is determined from
      the PAD FLASH definition. Next, the System Pad Table is searched for a pad
      definition that matches this same pad size and shape and BOARD CREATOR
      places one on the PC board.

Step 3:
      Select Paths/Options from the FILE/Preferences menu and select the printer
      configuration file gerber.pcf by pressing the Plotter PCF button. This will
      contain the aperture list information that we entered in Step 1.
                                                                                  315

Step 4:
     The Gerber plot files will need to be converted to a format that can be used by
     the BOARD CREATOR program. As mentioned earlier, the Import ASCII
     command converts files that are in another format to an update list. This update
     list is then used to create a board in BOARD CREATOR. To convert the
     Gerber plot files, select Import ASCII from the I/O menu.

     Enter the name of the Gerber plot file that represents the top conductor mask in
     the From field and enter the name that you will be giving to converted (update
     list) file in the To field. Note: Use the extension upd when naming the
     converted files. Select the Gerber option in the above dialog box and press the
     OK button to accept this information. The following dialog box will appear
     allowing you to assign the layer and mask type that this Gerber plot file
     represents:

     Repeat this step in order to import (or convert) each Gerber plot file to a
     separate update list file and assign the appropriate layer and mask type to each
     Gerber file (in the above dialog box). Note: Only use the Convert flashes
     (pads) option (in the above dialog box) on one of the Gerber plot files that
     represents a conductor mask. Otherwise, you will have pads stacked on top of
     each other when this board is generated.

Step 5:
     After you have finished importing (or converting) the Gerber plot files to
     update list files, we can begin re-creating each layer of the board one at a time.
     Select New from the FILE menu and define a new board that will be large
     enough to handle the imported board. Refer to the section "CREATING A
     NEWFILE" for more information about defining a new board. Next, select the
     Update from LOGIC CREATOR command from the I/O menu and choose one
     of the converted update list files (upd) that was created by the Import ASCII
     command in Step 4. When this layer has finished drawing, select the Update
     from EZ-LOGIC command again and choose the next upd file. Repeat this last
     step until all of the layers have been selected.

     Note: The text that will appear when the Gerber plot files are imported is not
     really text. The text will be made up of line segments because text is drawn in
316

       a Gerber plot file. Simply delete this pseudo text and replace it with real text.
       Also, there is no component information contained in a Gerber plot file,
       therefore, there are no true footprints on this imported board. They are simply
       silk-screen lines and pads. You will need to delete these pseudo footprints and
       replace them with real ones.

       The PC board may appear to be partially off of the screen when it is imported
       into BOARD CREATOR. If this happens, simply choose the Change All
       command from the EDIT menu and use the shift option to move the entire PC
       board a certain distance in the x and/or y direction.


Creating New Footprints
Footprints are created using the board editor (BOARD CREATOR). First, select a
New board under the FILE pull down menu. The default board size and settings will
do. Next, select DRAW/PAD and press the letter O to display the Pad Options.
Choose a pad (1-10) that matches the one you wish to use on your footprint. If you do
not find a pad with the size and shape that you require, re-define one of the pad's
dimensions under SYSTEM/EDIT SYSTEM PAD TABLE. Note: pad numbers 1, 3, 7
and 9 are commonly used in all the DIP, DB Connectors, and discrete component
footprints, so we suggest that you do not redefine these pads. When you have selected
a pad, you may begin placing the pads on the board with the proper pad spacing
required for your footprint. The first pad that is placed will be pin #1, the second will
be pin #2, and so on. The pin number will be automatically incremented for you, so
you will want to place the pads in the order that they are numbered on your footprint.

When you have finished placing pads, you will need to add a COMPONENT
REFerence selected from the DRAW pull down menu. (Add U1 as a component
reference to an IC, R1 to a resistor, C1 to a capacitor, and so on.) You may finish your
footprint by outlining its shape by selecting Line/Curve from the DRAW menu and
place these lines on the silkscreen mask. Finally, EDIT/SELECT the entire footprint
that you have just created and FILE/SAVE SYMBOL and name your footprint. This
footprint will be saved to a DOS file with an extension PCS.
                                                                                  317



Chapter 18
Using the Automatic Router
What is the Auto-Router?
The Auto-Router is the module of the CIRCUIT CREATOR system, that automates
the routing of the printed circuit board. The Auto-Router needs a PCB file with all the
footprints placed where you want them and the schedule lines to show on the board.
Then it picks up from there and automatically routes the board for you.
In this Chapter we will start with a board that is already prepared for routing. It is
called rtdemo1.pcb, and is shipped with CIRCUIT CREATOR Pro. Figure 17-1 is a
snap-shot of it.




      Figure 18.1 The rtdemo1.pcb Board Prepared for the Auto-Router

Go ahead and load it into BOARD CREATOR and examine how the component
footprints are placed on the board. Notice that enough space was left between and
318

around each component for the Auto-Router to route the copper track and also place
vias if needed. Do not change anything on this board at this time. Notice how the ICs
are aligned and how the descrete components are placed symmetrically to produce a
balanced looking board. When you are done with your examination exit BOARD
CREATOR without saving.

Now let’s route this board. Double click the Router icon to start the program. The
dialog box of figure 17-2 appears.




                 Figure 18.2 The Route:Board File Dialog Box

Select rtdemo1.pcb and press OK. Then the “Route:Setup” dialog box appears (figure
17-3).
                                                                                 319




                    Figure 18.3 The Route:Setup Dialog Box

We are not going to change any of the default settings for this example. Press OK, and
sit back and enjoy the Auto-Router doing all the work. On the right hand side of your
screen a double bar graph displays graphically the progress of the Router. Figure 17-4
shows a snap-shot of the Auto-Router at work.
320




                 Figure 18.4 The Auto-Router Doing its “Magic”

After the Auto-Router is done, it saves the routed PCB under the same file name.
Therefore in this case if we run BOARD CREATOR, and load rtdemo1.pcb we will
have the finished board. A snap-shot of the routed board is shown in figure 17-5. The
Router also produces the text file router.log, which summarizes the actions of the
Auto-Router. A copy of the log file produced during routing or rtdemo1.pcb follows.

              ROUTE CREATOR: PCB Autorouter, Version 3.0
              Input file: C:\CKTCRT\RTDEMO1.PCB

              Grid size 122 x 92, memory                        required=23312
              free=2050784
              Schedule   size  113,  memory                     required=1469,
              free=2003680
              Queue    size   701,  memory                      required=6309,
                                          321

free=2003680
Void type=0
Void type=0
Void type=0
Void type=0
Void type=0
Void type=0
Void type=0
Void type=0

Horizontal layer...:   1
Vertical layer.....:   2
Clearance line-line:   10
Clearance via-line.:   10
Clearance via-pad..:   10
Routing area (mils):   0,0 to 6000,4500
Routing grid..... x:   50, y: 50
Routing via pad #..:   1
Routing line width.:   10

-------------------Pass--------Total-
Pass.......... Setup
Pads.......... 228
Vias.......... 0,    0
Segments...... 0,    0
Length (mils). 0,    0
Time (sec).... 2.00,     2.00

-------------------Pass-------Total-
Pass.......... 1
Scheduled..... 113, 113
Attempted..... 65, 65
Made.......... 64, 64
Vias.......... 0,    0
Segments...... 183, 183
Length (mils).40959, 40959
Time (sec).... 2.00, 4.00
322

      -------------------Pass------Total-
      Pass.......... 2
      Scheduled..... 49, 113
      Attempted..... 17,   82
      Made.......... 16,   80
      Vias.......... 17,   17
      Segments...... 45, 228
      Length (mils). 14600, 55559
      Time (sec)....      1.00,     5.00

      ------------------------------Pass-----Total-
      Pass..........      3
      Scheduled.....      33,   113
      Attempted.....      33,   115
      Made..........      33,   113
      Vias..........      53,   70
      Segments...... 125,       353
      Length (mils). 63891, 119450
      Time (sec).... 19.00, 24.00

      Input file C:\CKTCRT\RTDEMO1.PCB renamed        to
      C:\CKTCRT\RTDEMO1.bak
      Routed PCB file is C:\CKTCRT\RTDEMO1.PCB
      All scheduled routes complete!

      -End-
                                                                                   323




                          Figure 18.5 The Routed Board

Let’s take a look at the log file and see what we can learn from it. At the beginning we
have information about the memory requirements of rtdemo1.pcb and the available
RAM of the computer system we used. Then a listing of the four passes it took the
Router to route the board and what was done during each pass.

The setup pass is for reading the PCB file and setting up the auto-Router. During this
pass it was found that we have a total of 228 pads in this file. No vias or copper track
segments were placed. It took the Router 2 seconds to do the setup pass.

During the first pass 113 copper tracks were scheduled, 65 were attempted and 64
were made. No vias were placed, 183 copper segments were placed, with total length
of 40,959 mils, or 40.959 inches. It took the Router 3 seconds to do the first pass.

During pass no.2, 49 tracks were scheduled, 17 were attempted, and 16 were made.
324

Seventeen vias were placed, 45 copper track segments were placed, with total length
of 14,600 mils or 14.6 inches. It took the Router 1 second to do the second pass.

During the third pass, 33 copper tracks were scheduled, and all were made. Fifty-three
vias were placed, 125 copper segments were placed totaling 63,891 mils or 63.891
inches. It took the Router 19 seconds to do the third pass.

Under the total column you can see the totals for this board. The total number of
scheduled copper tacks was 113. It took the Router 115 attempts to route them! (I
know it would have taken me many more attempts for sure). It placed a total of 70
vias, and 353 copper segments totaling 119.45 inches. It took the Router 25 seconds to
complete this routing! (It would have taken me half a day).




             Figure 18.6: The Reports Menu of BOARD CREATOR

This valuable information is always saved in the file router.log. When your run the
next Router session the new file will replace this one. If you would like to save this
information I suggest renaming this file to rtdemo1.log, so that you can easily
recognize it later on.

The Router also automatically creates a backup file of the original pre-routed file. The
name of the file is the same with the extension “BAK” (rtdemo1.bak). Therefore if
                                                                                  325

you would like to recover the original pre routed file you can rename the
“rtdemo1.bak” to something else with the extension “.PCB” so that you can load it
into BOARD CREATOR; for example: rtdemo1a.pcb.

Summary of Auto-routing
Here are the steps you need to follow to automatically route your board:

       1. Run BOARD CREATOR, and import the update list from LOGIC
          CREATOR.
       2. Move the footprints of the parts and place them the way you want the
          board to physically look. In placing the components leave enough spacing
          between them so that the Auto-Router will have room to place vias as
          needed.
       3. Run the Check/Schedule... command from the Reports menu (fig. 17-6)
          so that the schedule lines will appear on the screen. Now look for any
          schedule lines connecting parts that can be “untangled”. For example if you
          have 8 lines connecting straight from one IC to a neighboring one, and
          swapping the position of the IC’s will help, go ahead and do it. At this
          stage we are preparing the board to satisfy the physical constrains that we
          place on the design while at the same time having in mind what will aid the
          Auto-Router do the most efficient routing. Physical constrains that you
          may have are the location of connectors on the board, components
          requiring heat sinks, components requiring mechanical support on chassis
          or other modules, isolation of digital circuitry from analog circuitry, etc.
       4. Define how many layers the board is going to have, and identify each layer.
       5. Re-size the dimensions of the board (length and width).
       6. Now your board is ready for the Auto-Router to do its job. Save the board.
       7. Start the Auto-Router by double clicking its icon.
       8. Click on the file you have just prepared for routing, and then select OK.
       9. Change the Auto-router’s defaults if needed and run it.
       10. Now sit back and enjoy the view. You will see the Auto-Router at work,
           routing your board. On the right hand side of your screen a double bar
326

           graph displays graphically the progress of the Router.
       11. When the Router is done you can open your file using BOARD CREATOR
           and see the finished product.

Route Creator Reference
This section provides user reference information for using the ROUTE CREATOR
program.

What is an Autorouter?
Before using the auto-router, please take a few moments to read the following sections
to familiarize yourself with just what the auto-router does. An understanding of what the
auto-router expects and what it produces will help you in making it work for you. The
auto-router reads an BOARD CREATOR PC board file, accepts specifications from the
user, routes the board per the specifications, and writes a new BOARD CREATOR
board file. Note that the router inputs and outputs a board file of the same format. This
allows the same board file produced by one router run to be used as input to another
router run. Also, this allows a router run to be interrupted and restarted again at a later
time.

The PC board file that is read by the auto-router is made into a backup file by changing
its extension to "BAK". If anything goes wrong during a router run, or you are not
pleased with the results of a run, the board file may be restored from the backup file.
The new board file, containing the results of the routing, has the same name as the input
file. For example, if you route the board "MYBOARD.PCB", this file is renamed to
"MYBOARD.BAK" and the newly routed board file is named "MYBOARD.PCB".

Each run of the router creates a new log file named "ROUTE CREATOR.LOG". This
file lists statistics of the router run and other important information. To view the
contents of this file, use the DOS TYPE command, or print the file.

Preparation
To prepare a PC board for auto-routing, the following sections offer guidelines which
will greatly help the auto-router complete its task efficiently. These guidelines not only
apply to the auto-routing, they are equally good for manual layout as well.
                                                                                    327

Respect the Routing Grid
The auto-router uses a "routing grid" which is normally set to a spacing of 50 or 25 mils
and is measured from the board origin. When at all possible, components should be
placed on the board so that the pads of the components correspond to the routing grid.
Normally, the cursor grid in the BOARD CREATOR editor is set to 50 mils, and this
will happen automatically.




                         Figure 18.7 : Typical Routing Grid

Components and lines may be off-grid; however, it is expected that the majority of
components are on the routing grid. Components, such as the fingers of an edge
connector or the pins of an odd shaped component, may not fall exactly on the routing
grid. This is OK, and routes made to the pads will connect to the true center of the pad.
However, components that can be placed exactly on the routing grid should be placed
exactly on the routing grid.




                       Figure 18.8 : Component Placement
328

Good Component Placement
Proper placement of the components on the PC board is critical if a high degree of
completion is expected from the auto-router (or by hand layout). Some basic rules of
good placement are as follows:

Place components which connect together close to each other.

Align the pads of connecting components such that the connections may be made by
lines which are near horizontal or near vertical on the board.

Place components on the board so that they form rows and columns. Pads should align
with other pads horizontally and vertically. Do not stagger pads with respect to other
components.

When possible, spread out the components on the board. Use the available board area.
Do not jam a lot of components into a small area and then leave large open areas in
other sections of the board.

Route Widest Lines First
If you are routing a board with mixed line widths, such as a board with wide power and
ground lines, route the widest lines first. It is good practice to review each router run
with the BOARD CREATOR editor. Make adjustments as necessary, with the editor,
before making the next router run.

Indicate Void Areas
Use the DRAW/VOID AREA command in the BOARD CREATOR editor to mark
areas on the board that the auto-router is not allowed to use. Normally, a small margin
around the edge of the board is voided. Also, you may want to specify void areas around
edge connectors, holes, and other mechanically limiting devices.

The Routing Schedule
A "routing schedule" tells the auto-router which points on the board are to be connected.
A board must have a routing schedule before it can be auto-routed. Normally, a
routing schedule is generated with the BOARD CREATOR CHECK/SCHEDULE
command on the REPORTS menu.. If necessary, a routing schedule may be entered
directly with the BOARD CREATOR editor, by drawing "schedule lines" between
                                                                                     329

points that are to be routed. The lines must be drawn on the schedule mask. In either
case, the following describes how a routing schedule is represented on a PC board.




                          Figure 18.9 : Routing Schedule

A routing schedule is represented by lines on the "SCHEDULE" mask (any layer) of
the board. Each line on the schedule layer represents two points that are to be
connected by the auto-router. Schedule lines may freely cross other routing lines. This
is why these lines are sometimes referred to as a "rat's nest". Only the end points are
significant. The width of each schedule line specifies the width used to route the actual
connection.

When the auto-router makes a connection between two scheduled points, the actual
routing path is added to the board. The corresponding schedule line for this route is
deleted. If the auto-router attempts to route a scheduled line, but for some reason cannot
make the connection, the scheduled line is left on the board.

Please note that a routing schedule does not always have to be complete. That is, it
does not have to represent everything that is "un-routed" on the board. You may limit
the schedule to just what you want the auto-router to work on. You may work in any
combination of routing and manual editing.

Scheduling a Board
The BOARD CREATOR CHECK/SCHEDULE command on the REPORTS menu is
used to automatically generate a routing schedule for a board which has net names
assigned to its part pins.. If the board was created from an LOGIC CREATOR update
list file, or one of the supported import formats, the net names were assigned when the
board was created. If a board does not have net names, you must either assign the net
330

names or draw the routing schedule manually with the BOARD CREATOR editor.

The BOARD CREATOR schedule command will prompt you for the default line width
to be used in generating the schedule, and the name and width of any nets that have
special widths, such as power and ground.

Any schedule lines already on the board will be deleted before the new schedule is
generated. The new schedule lines will be added on the schedule mask of layer one of
the board. The ends of the schedule lines indicate the points that are to be connected by
the auto-router. Only points on the board which are not already connected will be
scheduled. All connections which are already made will be left exactly as they are.

Nets which are assigned to power planes, such as the power and ground nets for boards
with internal power planes, will not be scheduled for routing. Since these pads connect
directly to the required power plane, no additional routing is required.

Once a board is scheduled, you may proceed directly to the ROUTE CREATOR
program to auto-route the board.

A word of caution! If you make changes to a PC board after a schedule has been made,
the schedule may no longer be valid. If the placement of a board changes, or net
assignments are changed, make sure you reschedule the board before running the auto-
router.

Routing Controls
The following is an explanation of each of the router options.

Horizontal & Vertical
       Layers
       These two options specify the two layers of the board to use for routing new
       connections, and the predominant routing direction on each of those layers. This
       does not mean that only two layer boards may be routed. It means that only two
       specific layers of the board may be used during a single routing run. Boards with
       more than two signal layers are routed by making additional routing runs, and
       selecting different layers during each run.
                                                                                      331

       The horizontal and vertical layer must be two different layers.

Single Layer Routing
If you want to route only one layer, or you are routing a single-sided board, then specify
the layer you want to route on by its layer number. Enter zero (0) for the other layer. No
routing will be attempted on the zero layer.

Clearances
The clearance values specify the minimum distance allowed between the given items.
For example, a line-to-line clearance of 10 mils will cause the router to add new lines
with a separation of at least 10 mils from any other line. The distance is from edge to
edge (not center to center).

Routing Limit Area
The routing limit area represents the limits of the area on the board where routing is
allowed. The auto-router will only route within this area. By default, this is set to the
entire area of the board. For very large boards or test routing, you may wish to route the
board in sections. This is done by setting the area to different portions of the board, and
making multiple router runs. This option also controls how much computer memory is
required to route a board. For very large boards, you may not have enough memory to
route the entire board all at once. In this case, route the board by making several routing
runs, each of which is limited to a specific section of the board.

Routing Grid
The routing grid is the grid spacing to be used by the router. The default value is 50
mils. It is suggested you use a value of 50 or 25 mils. At first, you might think a 25 mil
grid would double the effective routing area of the board. This is not really true. On a 25
mil grid, a via will make the adjacent grids (25 mils away) unusable, except by its own
net. There is actually very little improvement in routing completion rates by using a 25
versus a 50 mil grid. The routing time and memory requirements are much larger!

Via Pad Type
This option specifies the pad number (shape) for vias added by the auto-router. This is
the pad number as defined by the BOARD CREATOR editor (numbers 1 - 25). The
default value is the via number last specified by the BOARD CREATOR editor for this
board.
332

Blind/Buried Vias
If the two specified routing layers could be used to route blind or buried vias, this option
will be available. If this option is selected (with an X), then only blind/buried vias will
be routed. These vias will connect only between the two routing layers. If this option is
off (no X), then regular vias will be routed. Regular vias will not go through all layers of
the board.

Tap In
If "tap-in" is checked, then the router is allowed to make connections by "tapping in" to
existing lines. This improves routing efficiency, and is desirable as long as the
technology you are using allows it.

Routing Line Width
This option specifies the width of lines to be routed by the auto-router. Only one width
per router run is allowed. The default value is the line width last specified by the
BOARD CREATOR for this board. Only scheduled lines which match the routing
line width option will be attempted during a single routing run.

Routing Passes
These options specify the router strategies to be applied during this router run. The
routing pass types are listed in order of increasing routing difficulty. Each router pass
may specifically enable or disable the routing of 45 degree lines. An X by an option
indicates it is enabled. The options enabled by default have proven to be very effective
in general purpose routing. For a given board, only experimenting on your own, and
experience in using the router will prove the most effective method for a particular
board. The strategies are always performed in order of easiest to most difficult. The
exact internal strategies represented by each routing pass option are considered
proprietary.

       Cancel
       Select this button to exit the router without attempting to route the current board.

       OK
       Begin Routing Select this button to begin routing the current board per the
       current control settings. Select this option after all the settings are set as desired.
                                    333

Help (H)
     Route Creator - General Help
     File Name
     Done Routing
     Horizontal & Vertical Layers
     Clearances
     Routing Limit Area
     Routing Grid
     Routing Line Width
     Via Pad Type
     Routing Passes
     Blind/Buried Vias
     Tap-In
     Ok, Begin Routing
     Cancel
334
                                                                                  335



Chapter 19
View Creator - General Help
File Menu
     The "file menu" provides commands for loading photo-plotter files, printer set-
     up, displaying program version information, running a DOS shell, and for
     exiting the program. You normally start and end an VIEW CREATOR session
     by using commands on this menu.

File - Open (Ctrl+O)
     Use this command to load a photo-plotter output file for viewing. Upon
     loading a file, the program will automatically display the file in the display
     window.

     Select the file to be loaded from the dialog-box that appears. If the name of the
     file that you want to view is in the list-box, you may press ENTER twice or
     double click with the mouse to directly make the selection.

     After loading a file, you may want to use the VIEW/SHOW OPTIONS
     command to select which "sub-plots" you want to view, the display colors, and
     the plot you want to appear on the top of the display.

File - Photoplotter Setup (I)
     Use this command to setup the Photoplotter configuration to control the photo-
     plotter "film" size and useable film area when a photo- plotter file is displayed.

     Always select the device and page size that corresponds to the actual photo-
     plotter device that will be used to eventually print your files. This will allow
     you to view the plots on the screen so you can verify that they are within the
     limits of the actual film's (page) useable area.
336

      Film Size
      This is the size of the film, not the board size Usually film size is one (1) inch
      larger in all four directions than printed circuit board (PCB) size.




      Crosshairs
      If clicked, You can see “+” sing on print image you have opened by using
      View Creator program. This command is usefull to check the co-ordinate on
      print image.

File - Exit (Alt+X)
      Use this command to exit the program.

View Menu
      Use the commands on this menu to control the view area, position, and scale of
      the current photo-plot that is being displayed.

View Menu - Application Colors
      Use this command to configure the colors for the program windows, such as
      the color of the rulers, status line, etc.

View - Show Options (M)
      Use this command to select the plots within the current photo-plotter file that
      will be displayed. Also, the color of each plot as well as the plot that will
      appear on top, and the film (background) color can be. specified.
                                                                             337

     A dialog-box will appear. Set the fields to the desired values and press OK.
     The current file will be redisplayed per the new settings.

View - Absolute/Local ( . )
     Use this command to toggle between an "absolute" or "local" cursor. The
     current cursor position is shown in the upper-right corner of the window.
     Absolute mode displays the position measured from the upper-left corner of
     the film area. Local mode displays the relative distance from the point the
     cursor was at when local mode was selected. Local mode is good for
     measuring distance between items, and the width of items. When in local mode
     the display of the cursor value is highlighted (reversed) on the screen.

     To use this command effectively, you must use the "." hot-key (period) to
     activate the command. If you use the mouse to select the command from the
     menu, the cursor will not be in the position you want to use as your local
     origin.

View - Pan Up (Pgup)
     Use this command to pan the drawing "up". The pan direction refers to the
     change in the view, not the direction that the photo-plotter film appears to
     move. For example, panning "up" indicates that you want to view more of the
     area toward the top edge of the film.

View - Pan Down (Pgdn)
     Use this command to pan the display view "down". For more detail, refer to
     the PAN UP command.

View - Pan Left (Shift+<)
     Use this command to pan the photo-plotter film view "left". For more detail,
     refer to the PAN UP command.

View - Pan Right (Shift+>)
     Use this command to pan the photo-plotter film view "right". For more detail,
     refer to the PAN UP command.
338

View - Pan Center (Nunlock+#5)
      Use this command to pan the point at the current cursor location to the center
      of the display area.

View - Zoom Home (Ctrl+Home)
      Use this command to view the upper-left corner of a photo-plotter file at the
      standard zoom and scale.

View - Zoom In (Ctrl+Pgup)
      Use this command to zoom in on the photo-plotter film display. Objects in the
      view will appear bigger and more detailed; however, you will be able to see
      less area of the film.

View - Zoom Out (Ctrl+Pgdn)
      Use this command to zoom out on the photo-plotter film display. Objects in the
      view will appear smaller and less detailed; however, you will be able to see
      more area of the film.

View - Redraw (Ctrl+R)
      Use this command to redraw the current display using the current view area
      and zoom settings.

Help Menu
Context/Index - F1
      This option gives you the index of the help manual. Move your mouse pointer
      above the word you need help on. If the arrow changes to a pointing hand then
      help is available, and you can access it by clicking on that word.

      This is the most important feature of the HELP menu. It allows you to get
      direct help on the specific command you are interested by highlighting the
      command and then pressing F1.
                                                                             339

Using Help
     This is a tutorial on how to use the help menu of VIEW CREATOR. Please go
     through this tutorial as many times as you need. It will help you became a

About View Creator (H)
     Use this command to display the copyright notice and current version/release
     number of the program.
340
                                      341



Appendix
CIRCUIT CREATOR "Hot-Keys"

Logic Creator Hot-Keys
The FILE MENU (Alt+F)
    OPEN                Ctrl+O
    New                 Ctrl+N
    Save                Ctrl+S
    Save As             Ctrl+A
    Hierachy            Push+
    Hierachy            Pop-
    Print               Ctrl+P
    Setup Printer       I
    Exit                Alt+X, or X
    Files               Alt+F #1
                        Alt+F #2
                        Alt+F #3
                        Alt+F #4

The DRAW Menu (Alt+D)
    Wire                W
    Net Name            N
    Port                P
    Bus                 B
    Line                L
    Text                T
342

The EDIT Menu (Alt+E)
      Format                      E
      Undo                        F2
      Cut                         Shift+Del
      Copy                        C
      Paste                       Shift+Ins
      Delete                      Del
      Update                      U
      Select                      S
      Unselect                    Z
      Select Trace                R
      Break Line                  Ctrl+B

Library Menu
      Freshen                     F
      Add Part by Library         A
      Add Part by Name            J
      Libraries                   Alt+L

      First Character of Library Name also you can define your own at configuring
      library in preferance menu.

VIEW Menu
      Sheet                       V
      Grid                        G
      Pan Up                      PgUp
      Pan Down                    PgDn
      Pan Right                   Shift+>
      Pan Left                    Shift+<
      Zoom In                     Ctrl+PgUp
      Zoom Out                    Ctrl+PgDn
      Zoom Home                   Ctrl+Home
      Redraw                      Ctrl+R
                                        343

The REPORTS Menu
    Status                Q
    Design Check          D
    Formal                Y
    Back Annotate         K

The HELP Menu
    Context & Index       F1
    Using Help            Alt+H U
    Abour Logic Creator   H

Board Creator Hot Keys
The FILE MENU
    Open                  Ctrl+O
    New                   Ctrl+N
    Save                  Ctrl+S
    Save As               Ctrl+A
    Load Symbol           Ctrl+L
    Save Symbol           Ctrl+V
    Print                 Ctrl+P
    Setup Printer         I
    Exit                  Alt+X, or X
    Files                 Alt+F #1
                          Alt+F #2
                          Alt+F #3
                          Alt+F #4

The EDIT Menu
    Board Format          E
    Undo                  F2
    Cut                   Shift+Del
    Copy                  C
    Paste                 Shift+Ins
    Delete                Del
344

      Update           U
      Select           S
      Unselect         Z
      Toggle Layer     F9
      Trace Net        Alt+E R
      Change All       Alt+E H
      Edit PAD Table   Alt+E P
      Component/Flat   Space Bar
      Break Line       B

The DRAW Menu
      Component Ref    N
      Pad              P
      Line/Curve       L
      Text             T
      Solid Area       D
      Void Area        V
      Region Pour      R
      Arc              A

The View Menu
      Layer/Masks      M
      Grid/Cursor      G
      Pan Up           PgUp
      Pan Down         PgDn
      Pan Right        Shift+>
      Pan Left         Shift+<
      PanPoint         F4
      PanCenter        NumLock + #5
      Locate           K
      Snap to Pad      F
      Zoom Home        Ctrl+Home
      Zoom In          Ctrl+PgUp
      Zoom Out         Ctrl+Pgdn
      Redraw           Ctrl+R
                                   345

The HELP Menu
   Context & Index       F1
   Using Help            Alt+H U
   About Board Creator   H
346
                                                                               347



Frequently
Asked Questions
Q.   If you initially create a PCB board file from LOGIC CREATOR and then
     make changes to the schematic, how do I update my BOARD CREATOR PCB
     file without losing the work already done on my board ?
A.   When you have finished making changes to your schematic in LOGIC
     CREATOR, select the Formal/Export command from the REPORTS menu and
     generate a new PCB Update list. This will create an update list file with the
     extension upd. The update list contains part and net list information about the
     schematic. Next, under the IO pull down menu in BOARD CREATOR there is
     an option to Update from LOGIC CREATOR where you select the update list
     file generated from LOGIC CREATOR. This will update the your PCB design
     respecting component placement and any routes you may have completed.

Q.   Does the BOARD CREATOR have DXF output ?
A.   Yes, Under the IO pull down menu in BOARD CREATOR select Export
     ASCII and DXF will be one of the output formats.

Q.   How can I add or change the pen widths defined in my pen carousel and pen
     speed for my particular pen plotter ?
A.   In order to add or change any printer/plotter options such as init strings
     (including pen speed), draw commands (including pen widths), you must edit
     the printer configuration file (or PCF file). The PCF files are in ASCII format
     and can be edited using any text editor. To change the pen speed of a pen
     plotter, you will need to modify the init string:

                           init "IN;PU;SP 0;VS 20;\13\\10\"

     Where VS 20 sets the pen speed of the plotter. Refer to the reference manual
     included with your pen plotter for recommended pen speed values. To add pen
348

      width definitions (as in the case of a pen carousel), add the following similar
      information to the printer/plotter configuration file (PCF):

                     WIDTH x "SP y;"

      Where x is the width of the pen (in mils) and y is the position of the pen in the
      pen carousel.

Q.    Is there any way to modify a region pour (i.e. break lines or update individual
      lines) after the copper has been put in place ?
A.    The region pour is placed as one component, which makes it very easy to
      select and remove if you need to make modifications on your PCB design.
      However, you can remove individual lines of the region pour if needed.

      There are several options that can be used when selecting objects: touching,
      bound by, flat, or component. To configure these options, choose the Select
      command from the EDIT menu and then press the letter O for options.
      Touching - when an area is selected, any object touching that "marked" area
      will also become selected.

      Bound by - only the objects completely bound by the "marked" area will
      become selected.

      Component - the entire component (or footprint) will be selected when any
      part of the component is selected.

      Flat - the Flat mode is very unique in that it allows you to edit, update, or
      move individual objects that belong to a component (or footprint) without
      selecting the entire component.

Q.    The region pour feature in BOARD CREATOR should fill as a solid area and
      not cross hatched.
A.    If you require that the region pour fills as a solid area, simply set the line width
      of the line used in the copper pour slightly greater than the x and y step. This
      will cause the lines to overlap giving the appearance of a solid area of copper.
                                                                               349

Q.   How do I relate footprints in BOARD CREATOR to the pins on my symbols
     in LOGIC CREATOR ?
A.   The symbols in LOGIC CREATOR contain the physical pin numbers on the
     symbol itself. Similarly, the footprints in BOARD CREATOR have pin
     numbers assigned to each pad used on the footprint.

Q.   How do I create a new footprint in BOARD CREATOR ?
A.   Footprints are created using the board editor (BOARD CREATOR). First
     select a New board under the FILE pull down menu. The default board size
     and settings will do. Next, select Pad from the DRAW menu and choose a pad
     (1-25) with the dimensions that you wish to use on your footprint. To display
     the pad options, press the letter O on the keyboard after selecting the Pad
     command. If you do not find a pad with the size and shape that you require,
     re-define one of the pad's dimensions by selecting Edit System Pad Table from
     the SYSTEM menu. (Note: pad types 1, 3, 7 and 9 are commonly used in all
     the DIP, DB Connectors, and discrete component footprints, so we suggest that
     you do not redefine these pads.) When you have selected a pad type, you may
     begin placing the pads on the board (with the proper pad spacing as required
     for your footprint) by simply clicking the right mouse button. The first pad
     that is placed will be assigned pin #1, the second will be pin #2, and so on.
     The pin number will be automatically incremented as you place the pads,
     therefore, you will want to place the pads in the order that they are numbered
     for your footprint. When you have finished placing pads, you will need to add
     a component reference by selecting Component Ref from the DRAW pull
     down menu. (Add U as a component reference to an IC, R to a resistor, C to a
     capacitor, and so on.) You may finish your footprint by outlining its shape by
     selecting Line/Curve from the DRAW menu and place these lines on the
     silkscreen mask. Finally, you will need to select the entire footprint that you
     have just created and select Save Symbol from the FILE menu and name your
     footprint. This footprint will be saved to a file with an extension PCS.

Q.   When I try to do Create from LOGIC CREATOR in BOARD CREATOR I get
     the error message "cannot open .log" ?
A.   This error message will occur when the path names configured for BOARD
     CREATOR are incomplete. Under the SYSTEM menu choose Paths/Options
350

      and check the path name configured for Drawing, Scratch, and Check Point.
      This path name must be complete. A valid path is as follows:

             C:\BOARD CREATOR\PCB\

      The path name must also be terminated with a backslash (\).

Q.    I get the error "part not recognized" on a part that I created when I try to
      generate reports in LOGIC CREATOR. I know my part and symbol are in the
      libraries. What should I do ?
A.    Check the part definition for your part using Symbol Creator. You may not
      have defined enough pins for your part in the MaxPin# field. The number you
      enter in this field must be greater than or equal to the largest pin number on
      your symbol. For instance, the part PHONEJK (a RJ-11 phone jack) uses a
      symbol that has four pins (pins 2, 3, 4, and 5). The part definition will need to
      show that this part has five pins since the largest pin number on the symbol is
      five. When you generate an UPDATE list with the PHONEJK part on your
      schematic, five pins will be listed for this part (however, pin #1 will be
      assigned as a NC pin).

Q.    How do I delete a connect dot in LOGIC CREATOR ?
A.    Selecting objects in LOGIC CREATOR is very similar to selecting objects in
      BOARD CREATOR. You have several SELECT options:
      Bound by - means that only the objects completely bound by the marked area
      will be selected.
      Touching - means that any object touching the marked area will be selected.
      Therefore, in order to delete a connect dot, choose the Bound By option as your
      select mode option and mark an area around the connect dot. Once the connect
      dot has been selected, press the DEL key.

Q.    When I run Check/Schedule in BOARD CREATOR I get the following error
      message:
                                                                                  351

     Note!
     ===================
     Routes not complete
     132
              What am I doing wrong ?
A.   This is not an error message. This message is telling you that based on your
     net list, you (or the auto-router) will need to connect 132 pairs of pads together
     in order to complete this design. A route is complete when two pads are
     connected (or joined together) by placing lines on a conductor mask. These
     routed lines result in a copper track on the finished PC board.

Q.   How do I move a group of items from one layer to another in BOARD
     CREATOR?
A.   This is accomplished using the Cut and Paste options. First select the items
     you wish to move. Next, select Cut from the EDIT pull down menu. These
     items will be stored in the "paste buffer". Now select Paste from the EDIT pull
     down menu and a box will appear showing you the area of the objects to be
     pasted. Before you "click" the left mouse button (or hit <ENTER>) to place the
     objects, press the letter O on the keyboard and you will be able to select the
     layer/mask that the objects will be "pasted" to.

Q.   Every once in a while I see a message appear that says "saving to checkpoint"
     file. What is this?
A.   LOGIC CREATOR and BOARD CREATOR have an auto-backup feature that
     periodically saves your current drawing or PC board to a check-point or
     backup file in case of a power loss. You can specify how often this backup
     occurs by selecting Paths/Options from the SYSTEM menu in both LOGIC
     CREATOR and BOARD CREATOR. The number entered for the checkpoint
     is in seconds. Entering a zero (0) will disable this feature. If a power loss is
     encountered, when you try to load your work again, you will be prompted that
     a checkpoint file exists and if you want to load this backup file instead.

Q.   When plotting Gerber in BOARD CREATOR, it always says "making sheet 1
     of 2". I know that I have selected a large enough film size to fit my board on.
     What am I doing wrong ?
352

A.    You never want to make two or more "plot" files for a single layer/mask when
      creating Gerber plots. First, check the "actual" size of your board. This is
      determined by selecting Board Format in the EDIT menu. The "width" (which
      is the horizontal measurement) and the "length" (which is the vertical
      measurement) are entered in this dialog box. This is your board size. The
      second problem that occurs while plotting Gerber is that a one inch border is
      added to all the sides of your board. Therefore, you will need to add two
      inches to your board's dimensions when selecting a film size. Finally, the film
      sizes defined in the Gerber configuration file (PCF) are oriented (L x W)
      whereas the dimensions of your board are (W x L). For example, if your
      board's dimensions are 6" x 9", you will need to select a film size that is larger
      than 11" x 8".

Q.    How do I rotate a footprint ?
A.    To rotate a footprint, it must first be selected. Once the footprint is selected,
      place the cursor in the selected area and press and hold the left mouse button.
      Continue holding the left mouse button and with the other hand press the F10
      key or the letter O to rotate the footprint in ninety degree increments.

      Rectangular pads of a footprint will only rotate when there is a pad defined in
      the PAD TABLE that has the opposite dimensions of the pad used on the
      footprint. For example, let's say a footprint is using a pad type # 9 (which is a
      20 x 60 rectangular pad with a 0.031 diameter hole). In order to rotate this
      footprint and also have the pads to appear as if they had rotated, there would
      need to be a pad (let's say Pad # 10) defined as 60 x 20 rectangular with a
      0.031 diameter hole. When the footprint is rotated, BOARD CREATOR
      automatically replaces the pad with a another pad having the exact opposite
      dimension. If such a pad does not exist, the pad in the footprint will appear to
      have not been rotated.

Q.    What Is a Thermal Relief ?
A.    When a power layer is printed or plotted, you will have the option to print the
      pads using a thermal relief or as a direct connection to the power layer. A
      power layer can be thought of as a solid sheet of copper dedicated to a single
      net (such as +5V). Pads (and vias) normally pass through the entire board
      including any inner layers such as a power layer. Think of the pads (and vias)
                                                                              353

as tiny metal cylinders (or plugs) inserted throughout your PC board design.
The pads that we want to connect to the power layer need to touch the solid
copper plane of the power layer. For all of the other pads and vias, we will
need to cutout (or remove) a large enough area of copper (in the power layer)
around the pad or via so that it will not be electrically connected to the power
layer. Therefore, we need to enter an oversize amount when printing or
plotting the power layer in order to isolate these pads and vias from the power
layer. Note: A minimum oversize amount of 0.020" is recommended in order
to leave a 0.010" clearance around a pad or via that is not to be connected to
the power layer.

A thermal relief is recommended when the board that you are designing will be
wave soldered. When the components are soldered on your board, the power
layer will act as a heat sink causing the solder to cool very fast on the pads that
are connected directly to the power layer. This may cause cold solder
connections on your board. A cold solder connection occurs when the solder
cools before it has a chance to bond to the metal lead of the component on the
PC board.

A thermal relief is used to reduce the area of copper that is connected to a pad
on the power layer. This will greatly reduce the amount of heat that is
dissipated through the power layer when the components are soldered. The
following is an example of a power layer showing the cutouts (or pads not
connected to the power layer) and thermal reliefs:




           Figure 16.1.1.1: Example of Thermal Reliefs.
354

      In order to view a power layer on the screen in BOARD CREATOR, you must
      be editing an object on that specific layer. For example, let's say that your
      power layer is Layer 2. Select the Line/Curve command from the DRAW
      menu and press the letter 0 to pop-up the Line Options dialog box. Choose
      Layer 2 as the layer that you would like to place the lines and press the OK
      button to accept this choice. When the screen redraws, it will be relative to the
      power layer (Layer 2) on your board and will display the pads as cutouts and
      thermal reliefs.

      Electronic and Electrical Device Reference Designators (ANSI Y32.2-1975)

      Voltage: Used interchangeably with potential. (See "Potential.") Watt: The
      unit of electric power. In a direct current one watt is equal to volts multiplied
      by amperes. In an alternating current the true power in watts is equal to
      effective volts multiplied by effective amperes. Word: In computers, a series
      of one to several bytes. Word length is expressed in bits and bytes, such as a
      2-byte word = a 4-nibble word = a 1 6-bit word. Word length is not standard.
      Electrical Part (Device) Reference Designations
      FROM ANSI Y32.2-1975

             Alarm, audible                    LS
             Amplifier                         AR
             Amplifier, rotating               G
             Annunciator                       DS
             Antenna                           E*
             Arrester, lightning               E*
             Assembly                          A
             Attenuator, fixed                 AT*
             Audible signaling device          LS
             Autotransformer                   T
             Battery                           BT
             Bell, electric                    LS*
             Blower                            B
             Board, terminal                   TB
             Breaker, circuit                  CB*
             Buzzer                            LS*
                                            355

Cable                                 W
Capacitor                             C*
Cell, aluminum or electrolytic        E
Cell,              light-sensitive,   V
photoemissive
Choke                                 L
Circuit breaker                       CB*
Clock                                 M*
Coil, hybrid                          HY
Coil, induction, relay, tuning,       L
operating
Coil. repeating Computer              A
Connector, plug, affixed to end       P
of cable, wire
Connector, receptacle, affixed        J
to wall, chassis, panel
Contact, electrical                   E*
Contactor, electrically operated      K
Contactor, mechanically or            S
thermally operated
Coupler, directional                  DC
Crystal detector                      CR
Crystal diode                         CR
Crystal, piezoelectric                Y
Cutout, fuse                          F
Cutout, thermal                       S
Detector, crystal                     CR
Device, indicating                    DS
Dipole antenna                        E*
Disconnecting device                  S
Earphone                              HT*
Electron tube                         V
Exciter                               G
Fan                                   B
Filter                                FL*
Fuse holder, lamp holder, or          X*
356

      socket
      Fuse                                F*
      Generator                           G*
      Handset                             HS*
      Head,      erasing,    recording,   PU*
      reproducing
      Heater                              HR*
      Horn, howler                        LS*
      Indicator, visual                   DS*
      Inductor                            L
      Instrument                          M
      Insulator                           E*
      Interlock, mechanical               MP
      Interlock, safety, electrical       S
      Jack (see connector, receptacle,    J*
      electrical)
      Junction, coaxial or Repeater       AR
      Junction, hybrid                    HY
      Key, switch                         S
      Lamp, pilot or illuminating         DS
      Lamp, signal                        DS
      Line, delay                         DL*
      Loop antenna                        E*
      Magnet, permanent                   E*
      Meter                               M
      Microphone                          MK*
      Mode transducer                     MT
      Modulator                           A
      Motor                               B*
      Motor-generator                     MG
      Oscillator (excluding electric      Y
      tube used in oscillator)
      Oscilloscope                        M*
      Pad                                 AT
      Pair                                W
      Path, guided, transmission          W
                                        357

Phototube                        V
Pickup, erasing, recording, or   PU
reproducing head
Plug                             P
Potentiometer                    R
Power supply                     PS*
Radio receiver                   RE*
Radio transmitter ff             TR *
Receiver, telephone              HT
Receptacle (fixed connector)     J
Regulator, voltage (except       VR
electron tube)
Relay, electrically operated     K*
contactor or switch
Resistor                         R*
Rheostat                         RF
Selenium cell                    CR
Shunt, relay                     R
Solenoid                         L*
Speaker                          LS
Speed regulator                  S
Subassembly                      A
Switch                           S
Terminal board                   TB*
Terminal strip                   TB*
Test point                       TB
Thermistor                       RT
Thermocouple                     TC*
Thermostat                       S
Timer                            M
Transducer                       MT
Transformer                      T*
Transistor                       Q*
Transmission path                W
Tube, electron                   V*
Varistor, symmetrical            RV
358

             Voltage regulator (except an R
             electron tube)
             waveguide (tee or wye)       CP
             Waveguide                    W
             Winding                      L*
             Wire                         W*

      * Those parts marked with an asterisk(*) are also approved in the Federal Item
      Identification
      Guide Cataloging Handbook H6-1.

      The preceding list is not the complete list of devices shown in ANSI
      Y32.2-1975. This listing contains more commonly used parts. This listing or
      ANSI Y32.2-1975 does not contain device function designations for power
      switchgear, industrial control, and industrial equipment. For
      these function designations, please consult:

      American National Standard Manual and Station Control, Supervisory and
      Associated Telemetering Equipment, C37.2-1970.
      NEMA Standard, Industrial Controls ICS-1970 (R1975)
      Joint Industrial Council Electrical Standards for Mass Production Equipment,
      EMP-1-1967 and General Purpose Machine Tools, EGP-1-1976

      Military Standard, Designations for Electric Power Switch Devices and
      Industrial Control Devices, MIL STD 27.

Control-Device Designations
Brake relay               BR              Magnetic clutch               MC
Control relay             CR              Manual                        MN
Control relay manual      CRH             Overload relay                OL
Control relay master      CRM             Pushbutton                    PB
Down                      D               Reverse                       R
Disconnect switch         DISC            Rheostat                      RH
Electron tube             ET              Switch                        S
Flow switch               FLS             Solenoid                      SOL
Float switch              FS              Selector switch               SS
                                                                                   359

Instantaneous overload        IOL            Transforrner                  T
Limit switch                  LS             Time delay relay              TR
Motor starter                 M              Reactor                       X
Magnetic brake                MB

Abbreviations for Drawings and Technical Publications
Primarily from MIL STD l 2D and other sources where Mil Std 1 2D does not list an
abbreviation.

Adapter                       ADPTR          Anode (electron devices)      A
Aircircuit breaker            ACB            Arrester                      ARSR
Alternating current           AC             Attenuation, attenuator       ATTEN
Alternating current volts     VAC            Audio frequency               AF
Aluminum                      AL             Auto frequency control        AFC
American Society of                          Automatic gain control        AGC
Mechanical Engineers          ASME           Base (electron device)        B
Ammeter                       AMM            Battery                       BTRY
Ampere                        A              Beat-frequency oscillator     BFO
Amplifier                     AMPL           Bottom                        BOT
Antenna                       AN
Arrnature                     ARM
Anode                         AD

* The Joint Industrial Council (JIC), "Electrical Standards for Industrial Equipment."
360

ACKNOLEDGEMENT and COMPANY INFORMATION
CIRCUIT CREATOR, LOGIC CREATOR, BOARD CREATOR, ROUTE
CREATOR, SYMBOL CREATOR, and VIEW CREATOR are trademarks of
Advanced Microcomputer Systems, Inc. At various places in this manual, other
products are referenced, using their common names which may be registered
trademarks of other companies. The purpose is for reference only, and no claim to the
trademark is intended.

Specifications are subject to change without notice.

The CIRCUIT CREATOR product is published and marketed by




                     Advanced Microcomputer Systems, Inc.
                           1377 S. Andrew Avenue,
                          Pompano Beach, FL 33069

                      Web Site: www.advancedmsinc.com
                       Email: info@advancedmsinc.com

				
DOCUMENT INFO