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					      PN4218/4228 ENGINEERING DESIGN GRAPHICS 2
      SolidWorks Instructional Notes for Teachers




         Lesson 1:
                 Basic Functionality




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                                      PN4218/4228 ENGINEERING DESIGN GRAPHICS 2
                                      SolidWorks Instructional Notes for Teachers
SolidWorks 2001 Teacher Guide




                                         What is SolidWorks?
                                                 SolidWorks is design automation software.

                                                 In SolidWorks, you sketch ideas and experiment
                                                 with different designs to create 3D models.
REPRODUCIBLE




                                                 SolidWorks is used by students, designers,
                                                 engineers and other professionals to produce
                                                 simple and complex parts, assemblies and
                                                 drawings.




                                                                                                                        Lesson 1: Basic Functionality
19




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                                                                                                                        Lesson 1: Basic Functionality
                                         The SolidWorks Model
                                         The SolidWorks model is made up of:
                                                 Parts
REPRODUCIBLE




                                                 Assemblies

                                                 Drawings
SolidWorks 2001 Teacher Guide




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                                      SolidWorks Instructional Notes for Teachers
SolidWorks 2001 Teacher Guide




                                                                                    Part                      Part
REPRODUCIBLE




                                                                                                  Assembly
                                      Drawing                                                                           Drawing




                                                                                                                                  Lesson 1: Basic Functionality
21




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                                                                                                                        Lesson 1: Basic Functionality
                                         Features
                                                 Features are
                                                 the building
                                                 blocks of the
                                                 part.
REPRODUCIBLE




                                                 Features are
                                                 the shapes and
                                                 operations that
                                                 construct the
                                                 part.
SolidWorks 2001 Teacher Guide




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                                      SolidWorks Instructional Notes for Teachers
SolidWorks 2001 Teacher Guide




                                         Examples of Shape Features
                                         Base feature
                                                 First feature in
                                                 part.
REPRODUCIBLE




                                                 Created from a
                                                 2D sketch.

                                                 Forms the
                                                 work piece to




                                                                                                                        Lesson 1: Basic Functionality
                                                 which other
                                                 features are
                                                 added.
23




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                                                                                                                                        Lesson 1: Basic Functionality
                                         Examples of Shape Features
                                         Boss feature
                                                Adds material
                                                to part.
REPRODUCIBLE




                                                Created from
                                                2D sketch.

                                                Must be
                                                attached to the                                                         Boss features
SolidWorks 2001 Teacher Guide




                                                rest of the part.




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                                      SolidWorks Instructional Notes for Teachers
SolidWorks 2001 Teacher Guide




                                         Examples of Shape Features
                                         Cut feature
                                                 Removes
                                                 material from
REPRODUCIBLE




                                                 part.

                                                 Created from a
                                                 2D sketch.

                                                 Must be                                                                Cut features




                                                                                                                                       Lesson 1: Basic Functionality
                                                 attached to the
                                                 rest of the part.
25




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                                                                                                                                  Lesson 1: Basic Functionality
                                         Examples of Shape Features
                                         Hole feature
                                                 Removes
                                                 material from
REPRODUCIBLE




                                                 part.
                                                 Works like a
                                                 more
                                                 intelligent cut
                                                 feature.                                                         Hole features
SolidWorks 2001 Teacher Guide




                                                 Usually
                                                 corresponds to manufacturing process such as
                                                 counter-sink, thread, counter-bore.

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                                         Examples of Operation Features
                                         Fillet feature
                                                                                                                            Fillet features

                                                 Used to round
                                                 off sharp
REPRODUCIBLE




                                                 edges.

                                                 Can remove or
                                                 add material.
                                                     Outside edge
                                                                                                                   Fillet features
                                                 (convex fillet)




                                                                                                                                              Lesson 1: Basic Functionality
                                                 removes material.
                                                        Inside edge (concave fillet) adds material.
27




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                                                                                                                                     Lesson 1: Basic Functionality
                                         Examples of Operation Features
                                         Chamfer
                                         feature
                                                 Similar to a
REPRODUCIBLE




                                                 fillet.

                                                 Bevels an edge
                                                 rather than
                                                 rounding it.
                                                                                                                   Chamfer feature
SolidWorks 2001 Teacher Guide




                                                 Can remove or
                                                 add material.


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SolidWorks 2001 Teacher Guide




                                         Sketched Features
                                                 Shape features have sketches.

                                                 Sketched features are built from 2D profiles.

                                         Operation Features
REPRODUCIBLE




                                                 Operation features do not have sketches.

                                                 Applied directly to the work piece by selecting
                                                 edges or faces.




                                                                                                                        Lesson 1: Basic Functionality
29




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                                                                                                                                                 Lesson 1: Basic Functionality
                                         To Create an Extruded Base Feature:
                                         1. Select a sketch plane.

                                         2. Sketch a 2D profile.

                                         3. Extrude the sketch perpendicular to sketch plane.
REPRODUCIBLE
SolidWorks 2001 Teacher Guide




                                          Sketch the 2D profile                        Extrude the sketch               Resulting base feature


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                                         To Create a Revolved Base Feature:
                                         1. Select a sketch                                                 Centerline
                                            plane.

                                         2. Sketch a 2D
REPRODUCIBLE




                                            profile.

                                         3. Sketch a
                                            centerline.

                                         4. Revolve the




                                                                                                                         Lesson 1: Basic Functionality
                                            sketch around
                                            the centerline.
31




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                                                                                                                                                     Lesson 1: Basic Functionality
                                         Terminology: Document Window
                                         Divided into two                                                               FeatureManager design tree
                                         panels:
                                                 Left panel contains
REPRODUCIBLE




                                                 the FeatureManager®
                                                 design tree.
                                                        Lists the structure of the
                                                        part, assembly or                                                   Graphics Area
                                                        drawing.
SolidWorks 2001 Teacher Guide




                                                 Right panel contains the Graphics Area.
                                                        Location to display, create, and modify a part, assembly or
                                                        drawing.


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                                         Terminology: User Interface
                                       Menu Bar
REPRODUCIBLE




                                      Toolbars                                                                          Drawing
                                                                                                                        document
                                                                                                                        window



                                      Part
                                      document
                                      window




                                                                                                                                      Lesson 1: Basic Functionality
                                                                                                                         Status bar
33




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                                                                                                                            Lesson 1: Basic Functionality
                                         Terminology: PropertyManager
                                                                              PropertyManager
                                                                                                      Confirmation Corner
REPRODUCIBLE




                                                                                    Preview
SolidWorks 2001 Teacher Guide




                                                                                     Handle




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                                         Terminology: Basic Geometry
                                                 Axis - An implied                                                      Axis

                                                 centerline that
                                                 runs through
                                                 every cylindrical                        Plane
REPRODUCIBLE




                                                 feature.
                                                 Plane - A flat 2D
                                                 surface.                                 Origin

                                                 Origin - The
                                                 point where the




                                                                                                                               Lesson 1: Basic Functionality
                                                 three default reference planes intersect. The
                                                 coordinates of the origin are:
                                                 (x = 0, y = 0, z = 0).
35




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                                                                                                                                       Lesson 1: Basic Functionality
                                         Terminology: Basic Geometry
                                                 Face      – The
                                                 surface or “skin”                                     Vertex           Edge
                                                 of a part. Faces
                                                 can be flat or
REPRODUCIBLE




                                                 curved.
                                                 Edge     – The
                                                 boundary of a                                    Edge

                                                 face. Edges can                                                               Faces

                                                 be straight or
SolidWorks 2001 Teacher Guide




                                                 curved.
                                                 Vertex                 – The corner where edges meet.


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                                         Features and Commands
                                         Base feature
                                                 The Base feature is the first feature that is created.
REPRODUCIBLE




                                                 The Base feature is the foundation of the part.

                                                 The Base feature geometry for the box is an
                                                 extrusion.

                                                 The extrusion is named Base-Extrude.




                                                                                                                        Lesson 1: Basic Functionality
37




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                                                                                                                                                    Lesson 1: Basic Functionality
                                         Features and Commands
                                         Features used to
                                         build the box are:
REPRODUCIBLE




                                                 Extruded Base feature
                                                                                                             1. Base Feature    2. Fillet Feature
                                                 Fillet feature

                                                 Shell feature

                                                 Extruded Cut feature
SolidWorks 2001 Teacher Guide




                                                                                                             3. Shell Feature   4. Cut Feature



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                                         Features and Commands
                                         To create the extruded base
                                         feature for the box:
                                                 Sketch a rectangular profile on a
REPRODUCIBLE




                                                 2D plane.

                                                 Extrude the sketch.

                                                 Extrusions are always perpendicular to the sketch
                                                 plane.




                                                                                                                        Lesson 1: Basic Functionality
39




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                                                                                                                                 Lesson 1: Basic Functionality
                                         Features and Commands
                                         Fillet feature
                                                 The fillet feature rounds the
                                                 edges or faces of a part.
REPRODUCIBLE




                                                 Select the edges to be rounded.
                                                 Selecting a face rounds all the
                                                                                                                        Fillet
                                                 edges of that face.

                                                 Specify the fillet radius.
SolidWorks 2001 Teacher Guide




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                                         Features and Commands
                                         Shell feature
                                                 The shell feature removes
                                                 material from the selected face.
REPRODUCIBLE




                                                 Using the shell feature creates a
                                                 hollow box from a solid box.

                                                 Specify the wall thickness for the
                                                 shell feature.




                                                                                                                        Lesson 1: Basic Functionality
41




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                                                                                                                        Lesson 1: Basic Functionality
                                         Features and Commands
                                         To create the extruded cut
                                         feature for the box:
                                         1. Sketch the 2D circular profile.
REPRODUCIBLE




                                         2. Extrude the 2D Sketch profile
                                            perpendicular to the sketch
                                            plane.
                                         3. Enter Through All for the end
SolidWorks 2001 Teacher Guide




                                            condition.
                                         4. The cut penetrates through the
                                            entire part.

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                                         Dimensions and Geometric
                                         Relationships
                                                 Specify dimensions and geometric relationships
                                                 between features and sketches.
REPRODUCIBLE




                                                 Dimensions change the size and shape of the part.

                                                 Mathematical relationships between dimensions
                                                 can be controlled by equations.

                                                 Geometric relationships are the rules that control




                                                                                                                        Lesson 1: Basic Functionality
                                                 the behavior of sketch geometry.

                                                 Geometric relationships help capture design intent.
43




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                                                                                                                        Lesson 1: Basic Functionality
                                         Dimensions
                                                 Base-Extrude
                                                 depth = 50 mm

                                                 Boss-Extrude
REPRODUCIBLE




                                                 depth = 25 mm




                                         Mathematical relationship:
SolidWorks 2001 Teacher Guide




                                                 Boss-Extrude depth = Base-Extrude depth ÷ 2



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                                         Geometric Relationships

                                                                                                                        Vertical
                                                                                               Horizontal
REPRODUCIBLE




                                                                                                                                           Parallel

                                                                                              Intersection




                                                                                                                                                      Lesson 1: Basic Functionality
                                                          Tangent


                                                                                               Concentric                      Perpendicular
45




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                                                                                                                                    Lesson 1: Basic Functionality
                                         To Start SolidWorks:
                                         1. Click the Start button                                           on Windows task bar.

                                         2. Click Programs.

                                         3. Click the SolidWorks 2001 folder.
REPRODUCIBLE




                                         4. Click the SolidWorks 2001
                                            application.
SolidWorks 2001 Teacher Guide




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                                         The SolidWorks Window
REPRODUCIBLE




                                                                                                                        Lesson 1: Basic Functionality
47




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                                                                                                                         Lesson 1: Basic Functionality
                                         To Create a New File Using a
                                         Document Template:
                                         1. Click New                           on the Standard toolbar
                                         2. Select a
REPRODUCIBLE




                                            document
                                            template:
                                                        Part
                                                                                                          Tutorial Tab
                                                        Assembly
                                                        Drawing
SolidWorks 2001 Teacher Guide




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                                         Document Templates
                                                Document Templates control the units, grid, text,
                                                and other settings for the model.

                                                The Tutorial document templates are required to
REPRODUCIBLE




                                                complete the exercises in the SolidWorks 2001
                                                Getting Started book.

                                                The templates are located in the Tutorial tab on the
                                                New SolidWorks Document dialog box.




                                                                                                                        Lesson 1: Basic Functionality
                                                Document properties are saved in templates.
49




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                                                                                                                        Lesson 1: Basic Functionality
                                         Document
                                         Properties
                                                 Accessed through
                                                 the Tools, Options
                                                 menu.
REPRODUCIBLE




                                         Document properties
                                         control many settings,
                                         including:
                                                 Units: English (inches) or Metric (millimeters)
SolidWorks 2001 Teacher Guide




                                                 Grid/Snap Settings
                                                 Colors, Material Properties and Image Quality

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                                         System Options
                                                 Accessed through
                                                 the Tools, Options
                                                 menu.
                                                 Allow you to
REPRODUCIBLE




                                                 customize your work
                                                 environment.
                                         System options control:
                                                 File locations




                                                                                                                        Lesson 1: Basic Functionality
                                                 Performance
                                                 Spin box increments
51




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                                                                                                                        Lesson 1: Basic Functionality
                                         Multiple Views of a Document
                                                 Drag the
                                                 horizontal
                                                 and vertical
                                                 split con-
REPRODUCIBLE




                                                 trols to view
                                                 4 panes.

                                                 Set the view
                                                 and display
                                                 options.
SolidWorks 2001 Teacher Guide




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                                         Creating a 2D
                                         Sketch:                                                                         Sketch Tool

                                         1. Select a sketch
                                            plane. The default
REPRODUCIBLE




                                            sketch plane is
                                            Plane1.                                                      Sketch Origin
                                                                                                                         Rectangle Tool
                                         2. Click Sketch
                                            on the Sketch
                                            toolbar.




                                                                                                                                          Lesson 1: Basic Functionality
                                         3. Click Rectangle                                 on the Sketch Tools toolbar.

                                         4. Move the pointer to the Sketch Origin.
53




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                                                                                                                                         Lesson 1: Basic Functionality
                                         Creating a 2D
                                         Sketch:                                                                        Sketch Tool

                                         5. Click the left
                                            mouse button.
REPRODUCIBLE




                                         6. Drag the pointer
                                                                                                       Sketch Origin
                                            up and to the                                                               Rectangle Tool
                                            right.

                                         7. Click the left
SolidWorks 2001 Teacher Guide




                                            mouse button
                                            again.



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                                         Adding Dimensions
                                                 Dimensions specify the size of the model.

                                         To create a dimension:                                                               Text Location
REPRODUCIBLE




                                         1. Click Dimension    on
                                            the Sketch Relations
                                            toolbar.                                                                    2D Geometry


                                         2. Click the 2D geometry.

                                         3. Click the text location.




                                                                                                                                              Lesson 1: Basic Functionality
                                         4. Enter the dimension
                                            value.
55




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         Lesson 2:
                 The 40-Minute Running
                 Start



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                                          Features and Commands
                                          Base Feature
                                                  The first feature that is created.
                                                  The foundation of the part.
REPRODUCIBLE




                                                  The workpiece to which everything else is
                                                  attached.
                                                  The base feature geometry for the box is an




                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                  extrusion.
                                                  The extrusion is named Base-Extrude.
                                                  Tip: Keep the base feature simple.
 71




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                                                                                                                                                  Lesson 2: The 40-Minute Running Start
                                          To Create an Extruded Base Feature:
                                          1. Select a sketch plane.

                                          2. Sketch a 2D profile.

                                          3. Extrude the sketch perpendicular to sketch plane.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




                                           Sketch the 2D profile                        Extrude the sketch               Resulting base feature


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                                          Features Used to Build Tutor1
REPRODUCIBLE




                                                      1. Base Extrude                       2. Boss Extrude                         3. Cut Extrude




                                                                                                                                                     Lesson 2: The 40-Minute Running Start
                                                                              4. Fillets                                 5. Shell
 73




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                                                                                                                         Lesson 2: The 40-Minute Running Start
                                          Extruded Boss Feature
                                                  Adds material to the part.
                                                  Requires a sketch.

                                          Extruded Cut Feature
REPRODUCIBLE




                                                  Removes material from the part.
                                                  Requires a sketch.

                                          Fillet Feature
 SolidWorks 2001 Teacher Guide




                                                  Rounds the edges or faces of a part to a specified
                                                  radius.

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                                          Shell Feature
                                                  Removes material from the
                                                  selected face.

                                                  Creates a hollow block from
REPRODUCIBLE




                                                  a solid block.

                                                  Very useful for thin-walled,
                                                  plastic parts.
                                                                                                                         Shell Feature




                                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                  You are required to specify a
                                                  wall thickness when using the shell feature.
 75




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                                                                                                                         Lesson 2: The 40-Minute Running Start
                                          View Control
                                          Magnify or reduce the view of a model in the
                                          graphics area.
                                                     Zoom to Fit – displays the part so that it fills the
REPRODUCIBLE




                                                     current window.
                                                     Zoom to Area – zooms in on a portion of the view
                                                     that you select by dragging a bounding box.
                                                     Zoom In/Out – drag the pointer upward to zoom
 SolidWorks 2001 Teacher Guide




                                                     in. Drag the pointer downward to zoom out.
                                                     Zoom to Selection – the view zooms so that the
                                                     selected object fills the window.

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                                          Display Modes
                                          Illustrate the part in various display modes.
REPRODUCIBLE




                                                                                                                                        Lesson 2: The 40-Minute Running Start
                                          Wireframe                       Hidden in Gray                        Hidden Lines   Shaded
                                                                                                                  Removed
 77




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                                                                                                                                      Lesson 2: The 40-Minute Running Start
                                          Standard Views
                                                                               Isometric
                                                                                 View
REPRODUCIBLE




                                                                                                              Top View




                                                            Back View                Left View              Front View   Right View
 SolidWorks 2001 Teacher Guide




                                                                                                           Bottom View


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                                          View Orientation
                                          Changes the view display to correspond to
                                          one of the standard view orientations.
                                                     Front                                                       Top
REPRODUCIBLE




                                                     Right                                                       Left

                                                     Bottom                                                      Back




                                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                     Isometric                                                   Normal To (selected
                                                                                                                 plane or planar face)
 79




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                                                                                                                         Lesson 2: The 40-Minute Running Start
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          View Orientation
                                          The views most
                                          commonly used
                                          to describe a
REPRODUCIBLE




                                          part are:
                                                  Top View

                                                  Front View




                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                  Right View

                                                  Isometric View
 81




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                                                                                                                         Lesson 2: The 40-Minute Running Start
                                          Default Planes
                                                  Plane1, Plane2,
                                                  and Plane3

                                          Correspond to the
REPRODUCIBLE




                                          standard principle
                                          drawing views:
                                                  Plane1 = Front or
                                                  Back view
 SolidWorks 2001 Teacher Guide




                                                  Plane2 = Top or Bottom view
                                                  Plane3 = Right or Left view

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                                          Isometric View
                                          Displays the part with height, width, and
                                          depth equally foreshortened.
                                                  Pictorial rather than
REPRODUCIBLE




                                                  orthographic.

                                                  Shows all three dimensions –
                                                  height, width, and depth.




                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                  Easier to visualize than
                                                  orthographic views.
 83




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                                                                                                                                         Lesson 2: The 40-Minute Running Start
                                          Section View
                                                  Displays the internal structure
                                                  of a model.

                                                  Requires a section cutting
REPRODUCIBLE




                                                  plane.




                                                                                                                         Section Plane
 SolidWorks 2001 Teacher Guide




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                                          The Status of a Sketch
                                                  Under defined
                                                         Additional dimensions or relations are
                                                         required.
                                                         Under defined sketch entities are blue (by
                                                         default).
REPRODUCIBLE




                                                  Fully defined
                                                         No additional dimensions or relationships
                                                         are required.
                                                         Fully defined sketch entities are black (by
                                                         default).




                                                                                                                         Lesson 2: The 40-Minute Running Start
                                                  Over defined
                                                         Contains conflicting dimensions or
                                                         relations, or both.
                                                         Over defined sketch entities are red (by
                                                         default).
 85




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                                                                                                                         Lesson 2: The 40-Minute Running Start
                                          Geometric Relations
                                                  Geometric relations are the rules that control the
                                                  behavior of sketch geometry.

                                                  Geometric relations help capture design intent.
REPRODUCIBLE




                                                  Example: The sketched circle is
                                                  concentric with the circular edge
                                                  of the extruded boss feature.

                                                  In a concentric relation, selected
 SolidWorks 2001 Teacher Guide




                                                  entities have the same center
                                                  point.



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                                          Geometric Relations
                                                  The SolidWorks default name for
                                                  circular geometry is an Arc#.

                                                  SolidWorks treats circles as 360°
REPRODUCIBLE




                                                  arcs.




                                                                                                                         Lesson 2: The 40-Minute Running Start
 87




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         Lesson 3:
                 Assembly Basics




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                                         Features Used to Build Tutor2
REPRODUCIBLE




                                                                   1. Base Extrude                                         2. Fillet




                                                                                                                                         Lesson 3: Assembly Basics
                                                                        3. Shell                                        4. Cut Extrude
107




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                                                                                                                         Lesson 3: Assembly Basics
                                         Sketch for Cut Feature
                                                 Sketch is composed of two curves.
                                                        Convert Entities creates the outside curve.
                                                        Offset Entities creates the inside curve.
REPRODUCIBLE




                                                 Rather than drawing the outlines by hand, they are
                                                 “copied” from existing geometry.

                                                 This technique is:
                                                        Fast and easy– select the face and click the tool.
SolidWorks 2001 Teacher Guide




                                                        Accurate – sketch entities are “cloned” directly from existing
                                                        geometry.
                                                        Intelligent – if the solid body changes shape, the sketch
                                                        updates. Automatically.


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                                         Convert Entities
                                                 Copies one or more curves into the active sketch
                                                 by projecting them onto the sketch plane.

                                                 Curves can be:
REPRODUCIBLE




                                                        Edges of faces
                                                        Entities in other sketches

                                                 Easy and fast
                                                        Select the face or curve.




                                                                                                                        Lesson 3: Assembly Basics
                                                        Click the              tool.
109




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                                                                                                                                       Lesson 3: Assembly Basics
                                         To Create the Outside Curve:
                                         1. Select the sketch plane.

                                         2. Open a new sketch.                                                          Sketch Plane


                                         3. Select the face or curves you
REPRODUCIBLE




                                            want to convert. In this case,
                                            select the face.

                                         4. Click Convert Entities                                        on
                                            the Sketch toolbar.
SolidWorks 2001 Teacher Guide




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                                         Creating the Outside Curve:
                                         5. Outside edges of face are
                                            copied into the active sketch.

                                         6. Sketch is fully defined – no
REPRODUCIBLE




                                            dimensions needed.




                                                                                                                        Lesson 3: Assembly Basics
111




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                                                                                                                        Lesson 3: Assembly Basics
                                         To Create the Inside Curve:
                                         1. Click Offset Entities   on
                                            the Sketch toolbar. The
                                            PropertyManager opens.
REPRODUCIBLE




                                         2. Select one of the converted
                                            entities.

                                         3. Move the cursor to the inside
                                            of the converted entities.
SolidWorks 2001 Teacher Guide




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                                         Creating the Inside Curve:
                                         4. The system generates a preview
                                            of the resulting offset. Because
                                            the Chain option was selected,
                                            the offset goes all the way around
REPRODUCIBLE




                                            the contour.

                                         5. Type the distance value. You can
                                            do this by simply typing. The
                                            pointer does not have to be inside the
                                            PropertyManager.




                                                                                                                        Lesson 3: Assembly Basics
                                         6. Press Enter. This updates the preview to reflect
                                            the offset distance.
113




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                                                                                                                        Lesson 3: Assembly Basics
                                         Creating the Inside Curve:
                                         7. Press Enter again (or click OK) to complete the
                                            command.

                                         8. The resulting sketch is fully defined.
REPRODUCIBLE




                                         9. There is only one dimension. It
                                            controls the offset distance.
SolidWorks 2001 Teacher Guide




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                                         Tutor Assembly
                                         The Tutor assem-
                                         bly is comprised of
                                         two parts:
REPRODUCIBLE




                                                 Tutor1 (created in
                                                 Lesson 2)

                                                 Tutor2 (created in
                                                 this lesson)




                                                                                                                        Lesson 3: Assembly Basics
115




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                                                                                                                        Lesson 3: Assembly Basics
                                         Assembly Basics
                                                 An assembly contains two or more parts.

                                                 In an assembly, parts are referred to as
                                                 components.
REPRODUCIBLE




                                                 Mates are relationships that align and fit
                                                 components together in an assembly.

                                                 Components and their assembly are directly
                                                 related through file linking.
SolidWorks 2001 Teacher Guide




                                                 Changes in the components affect the assembly.

                                                 Changes in the assembly affect the components.

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                                         To create the Tutor assembly:
                                         1. Open a new
                                            assembly
                                            document
                                            template.
REPRODUCIBLE




                                         2. Open
                                                 Tutor1.
                                         3. Open
                                                 Tutor2.




                                                                                                                        Lesson 3: Assembly Basics
                                         4. Tile the three
                                            windows
                                            horizontally.
117




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                                                                                                                        Lesson 3: Assembly Basics
                                         Creating the Tutor assembly:
                                         5. Drag and
                                            drop the part
                                            icons into
                                            the assembly
REPRODUCIBLE




                                            document.
SolidWorks 2001 Teacher Guide




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                                         Assembly Basics
                                                 The first component placed into an
                                                 assembly is fixed.

                                                 A fixed component cannot move.
REPRODUCIBLE




                                                 If you want to move a fixed component,
                                                 you must Float (unfix) it first.

                                                 Tutor1 is added to the FeatureManager design
                                                 tree with the symbol (f).




                                                                                                                        Lesson 3: Assembly Basics
                                                 The symbol (f) indicates a fixed component.
119




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                                                                                                                        Lesson 3: Assembly Basics
                                         Assembly Basics
                                                 Tutor2 is added to the FeatureManager
                                                 design tree with the symbol (-).

                                                 The symbol (-) indicates an
REPRODUCIBLE




                                                 underdefined component.

                                                 Tutor2 is free to move and rotate.
SolidWorks 2001 Teacher Guide




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                                         Manipulating
                                         Components
                                                    Move Component – translates
                                                    (moves) the selected
REPRODUCIBLE




                                                    component according to its
                                                    available degrees of freedom.




                                                                                                                        Lesson 3: Assembly Basics
121




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                                                                                                                        Lesson 3: Assembly Basics
                                         Manipulating
                                         Components
                                                    Rotate Component – rotates the
                                                    selected component according
REPRODUCIBLE




                                                    to its available degrees of
                                                    freedom.
SolidWorks 2001 Teacher Guide




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                                         Degrees of Freedom: There are Six
                                                 They describe
                                                 how an object is
                                                 free to move.
REPRODUCIBLE




                                                 Translation
                                                 (movement)
                                                 along X, Y, and Z
                                                 axes.

                                                 Rotation around




                                                                                                                        Lesson 3: Assembly Basics
                                                 X, Y, and Z axes.
123




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                                                                                                                                             Lesson 3: Assembly Basics
                                         Mate Relationships
                                                 Mates relationships align and fit together
                                                 components in an assembly.

                                                 The Tutor assembly requires three mates to fully
REPRODUCIBLE




                                                 define it. The three mates are:

                                                 Coincident between the top                                                          Edges
                                                 back edge of Tutor1 and the
                                                 edge of the lip on Tutor2.
SolidWorks 2001 Teacher Guide




                                                                                                                        Tutor1

                                                                                                                                 Tutor2


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                                         Mate Relationships
                                                 Second Mate: Coincident mate
                                                 between the right face of Tutor1
                                                 and the right face of Tutor2.
REPRODUCIBLE




                                                 Third Mate: Coincident mate
                                                 between the top face of Tutor1 and
                                                 the top face of Tutor2.




                                                                                                                        Lesson 3: Assembly Basics
125




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                                                                                                                        Lesson 3: Assembly Basics
                                         Mates and Degrees of Freedom
                                                 The first mate
                                                 removes all but
                                                 two degrees of
                                                 freedom.
REPRODUCIBLE




                                                 The remaining
                                                 degrees of
                                                 freedom are:
                                                        Movement along the
SolidWorks 2001 Teacher Guide




                                                        edge.
                                                        Rotation around the edge.




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                                         Mates and Degrees of Freedom
                                                 The second mate removes one
                                                 more degree of freedom.

                                                 The remaining degree of
REPRODUCIBLE




                                                 freedom is:
                                                        Rotation around the edge.




                                                                                                                        Lesson 3: Assembly Basics
127




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                                                                                                                        Lesson 3: Assembly Basics
                                         Mates and Degrees of Freedom
                                                 The third mate removes last
                                                 degree of freedom.

                                                 No remaining degrees of
REPRODUCIBLE




                                                 freedom.

                                                 The assembly is fully defined.
SolidWorks 2001 Teacher Guide




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                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 The switchplate requires two
                                                 fasteners.
REPRODUCIBLE




                                                 Create the fastener.

                                                 Create the switchplate-
                                                 fastener assembly.




                                                                                                                        Lesson 3: Assembly Basics
129




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                                                                                                                                Lesson 3: Assembly Basics
                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 The switchplate-fastener assembly
                                                 requires three mates to be fully defined. The three
REPRODUCIBLE




                                                 mates are:

                                                 First Mate: Concentric
                                                 mate between the
                                                 cylindrical face of the
                                                 fastener and the
SolidWorks 2001 Teacher Guide




                                                 cylindrical face of the
                                                 switchplate.                                                           Faces




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                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 Second Mate: Coincident                                      Faces
                                                 mate between the flat
REPRODUCIBLE




                                                 circular back face of the
                                                 fastener and the flat
                                                 front face of the
                                                 switchplate.




                                                                                                                        Lesson 3: Assembly Basics
131




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                                                                                                                                Lesson 3: Assembly Basics
                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 Third Mate: Parallel
                                                 mate between the flat                                                  Faces
REPRODUCIBLE




                                                 cut face of the
                                                 fastener and the flat
                                                 top face of the
                                                 switchplate.
                                                 The switchplate-
SolidWorks 2001 Teacher Guide




                                                 fastener assembly is
                                                 fully defined.



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                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 The cdcase-storagebox assembly requires
                                                 three mates to be fully defined. The three mates are:
REPRODUCIBLE




                                                 First Mate: Coincident
                                                 between the inside bottom
                                                 face of the storagebox
                                                 and the bottom face of the
                                                 cdcase.




                                                                                                                                Lesson 3: Assembly Basics
                                                                                                                        Faces
133




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                                                                                                                                             Lesson 3: Assembly Basics
                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 Second Mate: Coincident
                                                 mate between the inside                                                  Inside back face
REPRODUCIBLE




                                                 back face of the
                                                 storagebox and the back
                                                 face of the cdcase.

                                                                                                                  Faces
SolidWorks 2001 Teacher Guide




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                                         Additional Mate Relationships for
                                         Exercises and Projects
                                                 Third Mate: Distance mate
                                                 between the inside left face of
REPRODUCIBLE




                                                 the storagebox and the left
                                                 face of the cdcase.

                                                 Distance = 1cm.
                                                                                                                        Faces
                                                 Good job! Now, would you like
                                                 to do this 24 more times?




                                                                                                                                Lesson 3: Assembly Basics
                                                 No!
135




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                                                                                                                        Lesson 3: Assembly Basics
                                         Local Component Pattern
                                                 A local component pattern
                                                 is a pattern of components
                                                 in an assembly.
REPRODUCIBLE




                                                 The local component
                                                 pattern copies the Seed
                                                 Component.

                                                 The Seed Component in this
                                                 example is the cdcase.
SolidWorks 2001 Teacher Guide




                                                 This eliminates the work of adding and mating
                                                 each cdcase individually.


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                                         To Create a Local Component
                                         Pattern:
                                         1. Click Insert,
                                            Component
REPRODUCIBLE




                                            Pattern.

                                         2. Click Define your
                                            own pattern.

                                         3. Click Arrange in
                                            straight lines.




                                                                                                                        Lesson 3: Assembly Basics
                                         4. Click Next.
137




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                                                                                                                        Lesson 3: Assembly Basics
                                         Creating a Local Component Pattern:
                                         5. Select the cdcase
                                            as the Seed
                                            Component.
REPRODUCIBLE




                                         6. Select the front
                                            edge of the storage
                                            box for Along Edge/
                                            Dim.

                                         7. Spacing = 1cm
SolidWorks 2001 Teacher Guide




                                         8. Instances = 25

                                         9. Click Finish.

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                                         More to Explore: The Hole Wizard
                                         What determines
                                         the size of the
                                         hole?
REPRODUCIBLE




                                                 The size of the
                                                 fastener

                                                 The desired amount
                                                 of clearance




                                                                                                                        Lesson 3: Assembly Basics
                                                        Normal
                                                        Close
                                                        Loose
139




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         Lesson 4:
                 Drawing Basics




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                                          Engineering Drawings
                                          Drawings communicate three things about
                                          the objects they represent:
                                                  Shape – Views communicate the shape of an
REPRODUCIBLE




                                                  object.

                                                  Size – Dimensions communicate the size of an
                                                  object.

                                                  Other information – Notes communicate non-




                                                                                                                         Lesson 4: Drawing Basics
                                                  graphic information about manufacturing
                                                  processes such as drill, ream, bore, paint, plate,
                                                  grind, heat treat, remove burrs, etc.
 157




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                                                                                                                         Lesson 4: Drawing Basics
                                          Sample Engineering Drawing
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          General Drawing Rules – Views
                                                  The general characteristics of an object will
                                                  determine what views are required to describe its
                                                  shape.
REPRODUCIBLE




                                                  Most objects can be described using three
                                                  properly selected views.
                                                         Sometimes you can use fewer.
                                                         However, sometimes more are needed.




                                                                                                                         Lesson 4: Drawing Basics
 159




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                                                                                                                         Lesson 4: Drawing Basics
                                          Drawing Views
                                          Why do we need three
                                          views?
                                                  The Front and Top views of
REPRODUCIBLE




                                                  both parts are identical.

                                                  The Right side view is
                                                  necessary to show the
                                                  characteristic shape.
 SolidWorks 2001 Teacher Guide




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                                          Drawing Views: When Three is not
                                          Enough
                                                  Three standard views do not fully describe the
                                                  shape of the cut-out in the angled face.
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
 161




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                                                                                                                         Lesson 4: Drawing Basics
                                          Drawing Views: When Three is too
                                          Many
                                                  The Right side view is unnecessary.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          Dimensions
                                          There are two kinds of
                                          dimensions:
                                                  Size dimensions – how big is
REPRODUCIBLE




                                                  the feature?                                                             Size Dimensions


                                                  Location dimensions – where
                                                  is the feature?




                                                                                                                                               Lesson 4: Drawing Basics
                                                                                                                         Location Dimensions
 163




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                                                                                                                         Lesson 4: Drawing Basics
                                          General Drawing Rules – Dimensions
                                                  For flat pieces, give
                                                  the thickness
                                                  dimensions in the
                                                  edge view, and all
REPRODUCIBLE




                                                  other dimensions in
                                                  the outline view.
 SolidWorks 2001 Teacher Guide




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                                          General Drawing Rules – Dimensions
                                                  Dimension
                                                  features in
                                                  the view
                                                  where they
REPRODUCIBLE




                                                  can be seen
                                                  true size and
                                                  shape.

                                                  Use diameter dimensions for circles.

                                                  Use radial dimensions for arcs.




                                                                                                                         Lesson 4: Drawing Basics
 165




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                                                                                                                                    Lesson 4: Drawing Basics
                                          General Drawing Rules – Dimensions
                                                  Omit unnecessary dimensions.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




                                                                 This                                                    Not This



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                                          Dimension Guidelines – Appearance
                                                  Place dimensions away from the profile lines.

                                                  Allow space between individual dimensions.

                                                  A gap must exist between the profile lines and the
REPRODUCIBLE




                                                  extension lines.

                                                  The size and style of leader line, text, and arrows
                                                  should be consistent throughout the drawing.

                                                  Display only the number of decimal places




                                                                                                                         Lesson 4: Drawing Basics
                                                  required for manufacturing precision.
 167




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                                                                                                                         Lesson 4: Drawing Basics
                                          Drawing Appearance – Not Good
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          Drawing Appearance – Much Better
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
 169




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                                                                                                                         Lesson 4: Drawing Basics
                                          What is a Drawing Template?
                                                  A Drawing Template is the foundation for drawing
                                                  information.

                                          A drawing template specifies:
REPRODUCIBLE




                                                  Sheet (paper) size

                                                  Orientation - Landscape or Portrait

                                                  Sheet Format
 SolidWorks 2001 Teacher Guide




                                                         Borders
                                                         Title block
                                                         Data forms and tables such as bill of materials or revision
                                                         history


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                                          Drawing Templates Choices in
                                          SolidWorks
                                                  Standard SolidWorks drawing template

                                                  Tutorial drawing template
REPRODUCIBLE




                                                  Custom template

                                                  No template




                                                                                                                         Lesson 4: Drawing Basics
 171




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                                                                                                                           Lesson 4: Drawing Basics
                                          To Create a New Drawing Using a
                                          Document Template:
                                          1. Click New                           on the Standard toolbar
                                          2. Click the
REPRODUCIBLE




                                             Tutorial
                                             tab.
                                                                                                            Drawing Icon
                                          3. Double-
                                                                                              Tutorial Tab
                                             click the
                                             drawing
 SolidWorks 2001 Teacher Guide




                                             icon.                                                          Preview




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                                          Sample Drawing Template
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
 173




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                                                                                                                         Lesson 4: Drawing Basics
                                          Edit Sheet vs. Edit Sheet Format
                                          There are two modes in the drawing:
                                                  Edit Sheet
                                                         This is the mode you use to make detailed drawings
                                                         Used 99+% of the time
REPRODUCIBLE




                                                         Add or modify views
                                                         Add or modify dimensions
                                                         Add or modify text notes

                                                  Edit Sheet Format
 SolidWorks 2001 Teacher Guide




                                                         Change the title block size and text headings
                                                         Change the border
                                                         Incorporate a company logo
                                                         Add standard text that appears on every drawing


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                                          Title Block
                                                  Contains vital part and/or assembly information.

                                                  Each company can have a unique version of a title
                                                  block.
REPRODUCIBLE




                                                  Typical title block information includes:
                                                    Company name                                     Material & Finish
                                                    Part number                                      Tolerance
                                                    Part name                                        Drawing scale
                                                    Drawing number                                   Sheet size




                                                                                                                           Lesson 4: Drawing Basics
                                                    Revision number                                  Revision block
                                                    Sheet number                                     Drawn By/Checked By
 175




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                                                                                                                         Lesson 4: Drawing Basics
                                          To Edit the Title Block:
                                          1. Right-click in
                                             the graphics
                                             area, and
                                             select Edit
REPRODUCIBLE




                                             Sheet Format
                                             from the
                                             shortcut
                                             menu.
 SolidWorks 2001 Teacher Guide




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                                          Editing the Title Block:
                                          2. Zoom in on the
                                             title block.
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
 177




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                                                                                                                         Lesson 4: Drawing Basics
                                          Editing the Title Block:
                                          3. Right-click the note that
                                             says <COMPANY
                                             NAME>, and select
                                             Properties from the
REPRODUCIBLE




                                             shortcut menu.
 SolidWorks 2001 Teacher Guide




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                                          Editing the Title Block:
                                          4. Enter your school name
                                             in the Note text area of
                                             the dialog box.
REPRODUCIBLE




                                          5. Set the text justification
                                             to Center.
                                          6. Select the Font button
                                             to change the size and
                                             style of the text font.




                                                                                                                         Lesson 4: Drawing Basics
                                          7. Click OK.
 179




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                                                                                                                         Lesson 4: Drawing Basics
                                          Editing the Title Block:
                                          8. Position the
                                             note so it is
                                             centered in the
                                             space.
REPRODUCIBLE




                                          Tip: If you do not want
                                          to change the
                                          properties of the text
                                          (its font, size, etc.),
                                          only what it says,
 SolidWorks 2001 Teacher Guide




                                          simply double-click the
                                          text in the title block and edit it.




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                                          Customizing the Part Name
                                          Advanced Topic
                                                  The name of the part or assembly shown on the
                                                  drawing changes with every new drawing.
REPRODUCIBLE




                                                  It is not very efficient to have to edit the sheet
                                                  format and the title block each time you make a
                                                  new drawing.
                                                  It would be nice if the title block would
                                                  automatically be filled in with the name of the part




                                                                                                                         Lesson 4: Drawing Basics
                                                  or assembly that is shown on the drawing.
                                                  This can be done.
 181




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                                                                                                                         Lesson 4: Drawing Basics
                                          Editing the Part Name:
                                          Advanced Topic
                                          1. Click Note    on the
                                             Annotation toolbar, or
REPRODUCIBLE




                                             click Insert,
                                             Annotations, Note.
                                          2. Click the Link to
                                                  Property button                              .
 SolidWorks 2001 Teacher Guide




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                                          Editing the Part Name:
                                          Advanced Topic
                                          3. Choose SW-File Name
                                             from the list of
REPRODUCIBLE




                                             properties, and click
                                             External model
                                             reference.

                                          4. Click OK to add the property.




                                                                                                                         Lesson 4: Drawing Basics
 183




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                                                                                                                         Lesson 4: Drawing Basics
                                          Editing the Part Name:
                                          Advanced Topic
                                          5. On the Properties
                                             dialog, set any other
REPRODUCIBLE




                                             text properties such as
                                             justification, or font.
                                          6. Click OK to apply the
                                             changes and close the
                                             dialog.
 SolidWorks 2001 Teacher Guide




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                                          Editing the Part Name:
                                          Advanced Topic
                                          7. Results.
                                                  Currently the title block
REPRODUCIBLE




                                                  shows the text of the
                                                  property. However, when
                                                  the first view is added to
                                                  the drawing, that text
                                                  will change to become
                                                  the file name of the referenced part or assembly.




                                                                                                                         Lesson 4: Drawing Basics
 185




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                                                                                                                         Lesson 4: Drawing Basics
                                          Switching to Edit Sheet Mode:
                                          1. Right-click in
                                             the graphics
                                             area, and select
                                             Edit Sheet from
REPRODUCIBLE




                                             the shortcut
                                             menu.
                                          2. This is the
                                             mode you must
                                             be in when you
 SolidWorks 2001 Teacher Guide




                                             make drawings.




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                                          Detailing Options
                                          Dimensioning Standards
                                                  Dimensioning standards determine things such as
                                                  arrowhead style and dimension text position.
REPRODUCIBLE




                                                  The Tutorial drawing template uses the
                                                  ISO standard.

                                                  ISO stands for International
                                                  Organization for Standardization.




                                                                                                                         Lesson 4: Drawing Basics
                                                  ISO is widely used in European
                                                  countries.
 187




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                                                                                                                         Lesson 4: Drawing Basics
                                          Detailing Options
                                          Dimensioning Standards
                                                  ANSI is widely used in the United
                                                  States.
REPRODUCIBLE




                                                  ANSI stands for American National
                                                  Standards Institute.

                                                  Other standards include BSI (British Standards
                                                  Institution) and DIN (Deutsche Industries-Normen).
 SolidWorks 2001 Teacher Guide




                                                  Customize the drawing template to use the ANSI
                                                  standard.


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                                          Detailing Options
                                          Setting the dimensioning standard:
                                          1. Click Tools,
                                             Options.
REPRODUCIBLE




                                          2. Click the Document
                                             Properties tab

                                          3. Click Detailing.

                                          4. Select ANSI from




                                                                                                                         Lesson 4: Drawing Basics
                                             the Dimensioning
                                             standard list.
 189




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                                                                                                                         Lesson 4: Drawing Basics
                                          Detailing Options
                                          Setting the dimension font:
                                          1. Click Tools,
                                             Options.
REPRODUCIBLE




                                          2. Click the
                                             Document
                                             Properties tab

                                          3. Click Dimensions.
 SolidWorks 2001 Teacher Guide




                                          4. Click the Font button.

                                          5. Make the desired changes and click OK.

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                                          Saving a Custom Drawing Template:
                                          1. Click File, Save As...

                                          2. From the Save as type:
                                             list, click Drawing
REPRODUCIBLE




                                             Template.
                                                  The system automati-
                                                  cally jumps to the
                                                  directory where the
                                                  templates are
                                                  installed.




                                                                                                                         Lesson 4: Drawing Basics
                                          3. Click                   to create a new folder.
 191




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                                                                                                                         Lesson 4: Drawing Basics
                                          Saving a Custom Drawing Template:
                                          4. Name the new folder
                                             Custom.
                                          5. Browse to the
REPRODUCIBLE




                                             Custom folder.
                                          6. Enter ANSI-MM-
                                             SIZEA for the file
                                             name.
                                          7. Click Save.
 SolidWorks 2001 Teacher Guide




                                                  Drawing templates have the suffix *.drwdot



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                                          Creating a Drawing – General
                                          Procedure
                                          1. Open the part or assembly you wish to detail.
                                          2. Open a new drawing of the desired size.
REPRODUCIBLE




                                          3. Add views. Usually three standard views plus any
                                             specialized views such as detail, auxiliary, or
                                             section views.
                                          4. Insert the dimensions and arrange the dimensions
                                             on the drawing.




                                                                                                                         Lesson 4: Drawing Basics
                                          5. Add additional sheets, views and/or notes if
                                             required.
 193




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                                                                                                                                                    Lesson 4: Drawing Basics
                                          To Create Three Standard Views:
                                          1. Click Standard 3
                                                                                                                               Drawing View 2
                                                  Views                .
                                                                                                                                   Drawing View 3
                                          2. Select Tutor1
REPRODUCIBLE




                                             from the Window                                                             Drawing View 1

                                             menu.

                                          3. Click the graphics
                                             area of the part
 SolidWorks 2001 Teacher Guide




                                                  The drawing window
                                                  reappears with the three views of the selected
                                                  part.


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                                          Working with Drawing Views
                                                  To select a view, click the view boundary. The view
                                                  boundary is displayed in green.

                                                  Drawing views 2 and 3 are aligned with view 1.
REPRODUCIBLE




                                                  Drag Drawing View1 (Front). Drawing View 2 (Top)
                                                  and Drawing View 3 (Right) move, staying aligned
                                                  to Drawing View1.

                                                  Drawing View 3 can only be dragged left or right.




                                                                                                                         Lesson 4: Drawing Basics
                                                  Drawing View 2 can only be dragged up or down.
 195




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                                                                                                                         Lesson 4: Drawing Basics
                                          Working with Drawing Views
                                                  Hidden line representation.
                                                         Hidden in Gray is usually used in
                                                         orthographic views.
                                                         Hidden Lines Removed is usually
REPRODUCIBLE




                                                         used in isometric views.



                                                  Tangent edge display.
                                                         Right-click inside the view border.
 SolidWorks 2001 Teacher Guide




                                                         Select Tangent Edges, Tangent
                                                         Edges Removed from the shortcut
                                                         menu.




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                                          Dimensioning Drawings
                                                  The dimensions used to create the part can be
                                                  imported into the drawing.

                                                  Dimensions can be added manually using the
REPRODUCIBLE




                                                  Dimension tool                           .

                                          Associativity
                                                  Changing the values of imported dimensions will
                                                  change the part.




                                                                                                                         Lesson 4: Drawing Basics
                                                  You cannot change the values of manually
                                                  inserted dimensions.
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                                                                                                                         Lesson 4: Drawing Basics
                                          To Import Dimensions
                                          into the Drawing:
                                          1. Click Model Items     on the
                                             Annotation toolbar, or click
                                             Insert, Model Items.
REPRODUCIBLE




                                          2. Click the Dimensions check
                                             box.

                                          3. Click the Import items into all
                                             views check box.
 SolidWorks 2001 Teacher Guide




                                          4. Click OK.



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                                          Manipulating Dimensions
                                                  Moving dimensions:
                                                         Click the dimension text.
                                                         Drag the dimension to the desired location.
                                                         To move a dimension into a different view, press and hold the
REPRODUCIBLE




                                                         Shift key while you drag it.

                                                  Deleting dimensions:
                                                         Click the dimension text, and then press the Delete key.

                                                  Flipping the arrows:
                                                         Click the dimension text.




                                                                                                                         Lesson 4: Drawing Basics
                                                         A green dot appears on the dimension
                                                         arrows.
                                                         Click the dot to flip the arrows in or out.
 199




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                                                                                                                         Lesson 4: Drawing Basics
                                          Finish the Drawing
                                                  Position the
                                                  views.

                                                  Arrange the
REPRODUCIBLE




                                                  dimensions by
                                                  dragging them.

                                                  Set hidden line
                                                  removal and
                                                  tangent edge
 SolidWorks 2001 Teacher Guide




                                                  display.




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                                          Associativity
                                                  Changing a dimension on the
                                                  drawing changes the model
                                                         Double-click the dimension text.
                                                         Enter a new value.
REPRODUCIBLE




                                                         Rebuild.

                                                  Open the part. The part reflects
                                                  the new value.

                                                  Open the assembly. The
                                                  assembly also reflects the new




                                                                                                                         Lesson 4: Drawing Basics
                                                  value.
 201




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                                                                                                                         Lesson 4: Drawing Basics
                                          Multi-sheet Drawings
                                          Drawings can contain more than one sheet.
                                                  The first drawing sheet contains Tutor1.
REPRODUCIBLE




                                                  The second drawing sheet contains the Tutor
                                                  assembly.

                                                  Use the B-size landscape (11” x 17”) drawing
                                                  Sheet Format.
 SolidWorks 2001 Teacher Guide




                                                  Add 3 standard views.

                                                  Add an Isometric view of the assembly. The
                                                  Isometric view is a named view.

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                                          Three View Drawing of Assembly
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
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                                                                                                                           Lesson 4: Drawing Basics
                                          Named Views
                                                  A named view shows the part or assembly in a
                                                  specific orientation.

                                                  Examples of named views are:
REPRODUCIBLE




                                                         Standard Views such as Front, Top or Isometric view.
                                                         User-defined view orientations that were created in the part or
                                                         assembly.
                                                         The current view in a part or assembly.
 SolidWorks 2001 Teacher Guide




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                                          To Insert a Named View:
                                          1. Click Named View                                     , or click Insert, Drawing
                                             View, Named View.

                                          2. Click inside the border of an existing
REPRODUCIBLE




                                             view.
                                                  Important: Do not click directly on
                                                  one of the parts in the assembly.
                                                  Doing so will create a named view of
                                                  that specific part.




                                                                                                                               Lesson 4: Drawing Basics
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                                                                                                                         Lesson 4: Drawing Basics
                                          Inserting a Named View:
                                          3. A list of named views appears in
                                             the PropertyManager.
                                                  Select the desired view, in this
                                                  case, Isometric, from the list.
REPRODUCIBLE




                                          4. Place the view in the desired
                                             location on the drawing.
 SolidWorks 2001 Teacher Guide




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                                          Isometric View Added to Drawing
REPRODUCIBLE




                                                                                                                         Lesson 4: Drawing Basics
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                                                                                                                         Lesson 4: Drawing Basics
                                          Specialized Views
                                          Detail View – used to show
                                          enlarged view of something.

                                          1. Click  , or click Insert,
                                             Drawing View, Detail.
REPRODUCIBLE




                                          2. Sketch a circle in the
                                             “source” view.
                                          3. Position the view on
                                             drawing.
 SolidWorks 2001 Teacher Guide




                                          4. Edit the label to change scale.
                                          5. Import dimensions or drag them into view.

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                                          Specialized Views
                                          Section View – used to show internal
                                          aspects of object.

                                          1. Click  , or click Insert
                                             Drawing View, Section.
REPRODUCIBLE




                                          2. Sketch line in the “source”
                                             view.

                                          3. Position the view on drawing.




                                                                                                                         Lesson 4: Drawing Basics
                                          4. Section view is automatically crosshatched.

                                          5. Double-click section line to reverse arrows.
 209




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         Lesson 5:
                 Design Tables




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                                          Families of Parts
                                                  Many times parts
                                                  come in a variety
                                                  of sizes.
REPRODUCIBLE




                                                  This is called a
                                                  family of parts.

                                                  It is not efficient to
                                                  build each version
                                                  individually.




                                                                                                                         Lesson 5: Design Tables
                                                  Design Tables
                                                  simplify making families of parts.
 225




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                                                                                                                         Lesson 5: Design Tables
                                          Design Table Overview
                                                  Design Tables are used to create different
                                                  configurations of a part.

                                                  What is a Configuration?
REPRODUCIBLE




                                                         A configuration is a way to create a family of similar parts
                                                         within one file.
                                                         Each configuration represents one version of the part.

                                                  Design Tables automatically change the
                                                  dimensions and features of an existing part to
 SolidWorks 2001 Teacher Guide




                                                  create multiple configurations. The configurations
                                                  control the size and shape of a part.


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                                          Design Table Overview
                                                  Design Tables can                                                      Center hole suppressed
                                                  control the state of
                                                  a feature.
REPRODUCIBLE




                                                  The state of a
                                                  feature can be
                                                  suppressed or
                                                  unsuppressed (also
                                                  called resolved). A suppressed feature is not
                                                  rebuilt or displayed.




                                                                                                                                                  Lesson 5: Design Tables
                                                  Design Tables requires Microsoft Excel
                                                  application.
 227




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                                                                                                                                         Lesson 5: Design Tables
                                          Design Tables Require:
                                                                                                        Dimension and/or Feature names
                                                                                                        or special keywords
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




                                                                   Configuration names                                   Values

                                          Tip: Rename features and dimensions before
                                               creating a design table.

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                                          Rename Features and Dimensions
                                                 Feature and Dimension names used in a Design
                                                 Table should be renamed to better describe their
                                                 function.
REPRODUCIBLE




                                                 Which is easier to understand?
                                                         D1@Cut-Extrude1
                                                         Width@Oval_Slot




                                                                                                                         Lesson 5: Design Tables
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                                                                                                                         Lesson 5: Design Tables
                                          To Rename a Feature:
                                          1. Click-pause-click on Base-
                                             Extrude in the FeatureManager
                                             design tree (do not double-click).
REPRODUCIBLE




                                                 Tip: Instead of the click-pause-click
                                                 technique, you can select the feature, and
                                                 then press the function key F2.

                                          2. The feature name is highlighted in
                                             blue, ready to be edited.
 SolidWorks 2001 Teacher Guide




                                          3. Type the new name, Box, and press Enter.




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                                          Rename the Other Features Used in
                                          the Design Table
                                                 Rename Boss-Extrude1 to Knob.

                                                 Rename Cut-Extrude1 to
REPRODUCIBLE




                                                 Hole_in_knob.
                                                 Rename Fillet1 to
                                                 Outside_corners.




                                                                                                                         Lesson 5: Design Tables
 231




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                                                                                                                         Lesson 5: Design Tables
                                          To Display Feature Dimensions:
                                                 Right-click the
                                                 Annotations
                                                 folder, and
                                                 select Show
REPRODUCIBLE




                                                 Feature
                                                 Dimensions
                                                 from the
                                                 shortcut
                                                 menu.
 SolidWorks 2001 Teacher Guide




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                                          To Hide All the Feature
                                          Dimensions for a
                                          Selected Feature:
                                                 Right-click the feature in the
REPRODUCIBLE




                                                 FeatureManager design tree,
                                                 and select Hide All Dimensions
                                                 from the shortcut menu.




                                                                                                                         Lesson 5: Design Tables
 233




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                                                                                                                         Lesson 5: Design Tables
                                          To Hide Individual Dimensions:
                                                 Right-click the
                                                 dimension, and
                                                 select Hide from
                                                 the shortcut
REPRODUCIBLE




                                                 menu.
 SolidWorks 2001 Teacher Guide




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                                          To Display Dimension Names:
                                          1. Click Tools,
                                             Options.

                                          2. Click General
REPRODUCIBLE




                                             on the System
                                             Options tab.

                                          3. Click Show
                                             dimension
                                             names.




                                                                                                                         Lesson 5: Design Tables
                                          4. Click OK.
 235




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                                                                                                                         Lesson 5: Design Tables
                                          To Rename a Dimension:
                                          1. Display the dimension.
                                                         Either double-click the
                                                         feature to display its
                                                         dimensions.
REPRODUCIBLE




                                                         Or, right-click the
                                                         Annotations folder, and
                                                         select Show Feature
                                                         Dimensions.

                                          2. Right-click the 70mm
 SolidWorks 2001 Teacher Guide




                                             diameter dimension,
                                             and select Properties
                                             from the shortcut
                                             menu.

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                                          Renaming Dimensions:
                                          3. In the Dimension Properties
                                             dialog box, select the text in
                                             the Name box and type in a
                                             new name, knob_dia.
REPRODUCIBLE




                                                 knob_dia@Sketch2 is
                                                 automatically displayed in the
                                                 Full Name box.

                                          4. Click OK.




                                                                                                                         Lesson 5: Design Tables
 237




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                                                                                                                         Lesson 5: Design Tables
                                          Rename these Dimensions:
                                                 Height of the box to
                                                 box_height.
                                                 Width of the box to
REPRODUCIBLE




                                                 box_width.
                                                 Diameter of the hole
                                                 in the knob to
                                                 hole_dia.
 SolidWorks 2001 Teacher Guide




                                                 Radius of outside
                                                 corners to
                                                 fillet_radius.

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                                          Design Intent
                                                 The depth of the Knob
                                                 should always be equal to
                                                 the depth of the Box (the
                                                 base feature).
REPRODUCIBLE




                                                 The Knob should always
                                                 be centered on the Box.

                                                 Dimensions alone are not
                                                 always the best way to
                                                 capture design intent.




                                                                                                                         Lesson 5: Design Tables
 239




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                                                                                                                         Lesson 5: Design Tables
                                          Linking Values
                                                 The Link Values command relates dimensions to
                                                 each other through shared variable names.

                                                 If the value of one linked dimension is modified,
REPRODUCIBLE




                                                 then all of the linked dimensions are modified.

                                                 Link Values is excellent for making feature
                                                 dimensions equal to each other.

                                                 This is an important tool for capturing design
 SolidWorks 2001 Teacher Guide




                                                 intent.




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                                          Examples of Uses for Link Values
                                                 The thickness
                                                 of the square
                                                 and the two
                                                 tabs is always
REPRODUCIBLE




                                                 equal.

                                                 The width of
                                                 both slots is
                                                 always equal.




                                                                                                                         Lesson 5: Design Tables
 241




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                                                                                                                         Lesson 5: Design Tables
                                          Link the Depth of the Box to the
                                          Depth of the Knob:
                                          1. Display the
                                             dimensions.
REPRODUCIBLE




                                          2. Right-click on
                                             the depth
                                             dimension for
                                             the Box, and
                                             select Link
 SolidWorks 2001 Teacher Guide




                                             Values from the
                                             shortcut menu.



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                                          Linking the Box to the Knob:
                                          3. Type Depth in the
                                             Name text box and
                                             then click OK.
REPRODUCIBLE




                                          4. Right-click on the
                                             depth dimension for the
                                             Knob, and select Link
                                             Values from the shortcut
                                             menu.




                                                                                                                         Lesson 5: Design Tables
 243




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                                                                                                                         Lesson 5: Design Tables
                                          Linking the Box to the Knob:
                                          5. Select Depth
                                             from the list, and
                                             click OK.
                                          6. Both dimensions
REPRODUCIBLE




                                             have the same name and value.
                                          7. Rebuild the part to
                                             update the geometry.
                                          Tip: Use the CTRL key to select
                                          several dimensions at the same
 SolidWorks 2001 Teacher Guide




                                          time and link them in one step.




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                                          Geometric Relations
                                          Relate geometry through physical
                                          relationships such as:
                                                 Concentric
REPRODUCIBLE




                                                 Coradial

                                                 Midpoint

                                                 Equal




                                                                                                                         Lesson 5: Design Tables
                                                 Collinear

                                                 Coincident
 245




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                                                                                                                         Lesson 5: Design Tables
                                          Examples of Geometric Relations
                                                 The Sketch Fillet tool
                                                 automatically creates
                                                 one radial dimension
                                                 and 3 Equal relations.
REPRODUCIBLE




                                                 Changing the dimension
                                                 changes all 4 fillets.

                                                 This technique is better
                                                 than having 4 radial
 SolidWorks 2001 Teacher Guide




                                                 dimensions.




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                                          Examples of Geometric Relations
                                                 Two features.

                                                 Making the circle
                                                 for the boss
REPRODUCIBLE




                                                 Coradial with the
                                                 edge of the base
                                                 ensures that the
                                                 boss will always be
                                                 the correct size
                                                 regardless of how                                                       Or




                                                                                                                              Lesson 5: Design Tables
                                                 the base changes.
 247




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                                                                                                                         Lesson 5: Design Tables
                                          To Center the Knob on the Box:
                                          1. Right-click the Knob
                                             feature, and select Edit
                                             Sketch from the
                                             shortcut menu.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          Centering the Knob on the Box:
                                          2. Delete the linear
                                             dimensions.

                                          3. Notice the circle is blue,
REPRODUCIBLE




                                             indicating it is under
                                             defined.

                                          4. Drag the circle to one side.
                                             Without dimensions to
                                             locate it, it is free to move.




                                                                                                                         Lesson 5: Design Tables
                                          5. Click   , and sketch a
                                             diagonal Centerline.
 249




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                                                                                                                         Lesson 5: Design Tables
                                          Centering the Knob on the Box:
                                          6. Click Add Relations                                      .

                                          7. Select the centerline and the
                                             point at the center of the circle.
REPRODUCIBLE




                                                         Note: If the centerline is still
                                                         highlighted when the Add Geometric
                                                         Relations dialog box opens, the line
                                                         will automatically appear in the
                                                         Selected Entities list and you do not
                                                         have to select it again.
                                                         If you select the wrong entity, right-
 SolidWorks 2001 Teacher Guide




                                                         click in the graphics area, and select
                                                         Clear Selections.




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                                          Centering the Knob on the Box:
                                          8. Click Midpoint, and then
                                             click Apply and Close.

                                          9. The circle will now stay
REPRODUCIBLE




                                             centered on the Box
                                             feature.




                                                                                                                         Lesson 5: Design Tables
 251




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                                                                                                                         Lesson 5: Design Tables
                                          Centering the Knob on the Box:
                                          10. Click Rebuild    to exit
                                              the sketch and rebuild
                                              the part.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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                                          To Insert a New Design Table:
                                          1. Position the part in the lower right hand corner of
                                             the graphics area

                                          2. Click Tools, Options.
REPRODUCIBLE




                                          3. On the System Options tab, under the heading
                                             General, make sure the option Edit design tables
                                             in a separate window is not selected

                                          4. Click OK.




                                                                                                                         Lesson 5: Design Tables
                                          5. Click Insert, New Design Table.
 253




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                                                                                                                         Lesson 5: Design Tables
REPRODUCIBLE
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                                          Inserting a New Design Table:
                                                 An Excel worksheet is displayed in the part
                                                 document window.
                                                 Excel toolbars replace the SolidWorks toolbars.
REPRODUCIBLE




                                                 By default, the first configuration is named First
                                                 Instance. You can (and should) change this to
                                                 something more meaningful.




                                                                                                                         Lesson 5: Design Tables
 255




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                                                                                                                                             Lesson 5: Design Tables
                                          Review of a Design Table’s Format:

                                                                                                       Dimension and/or Feature names
                                                                                                       or special keywords go in this row.
REPRODUCIBLE




                                                                                                                         Values go here.
 SolidWorks 2001 Teacher Guide




                                                                    Configuration names
                                                                    go in this column.




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                                          Inserting a New Design Table:
                                          1. Double-click the box_width dimension.
                                                 The full dimension name is
                                                 inserted into cell B2. The
                                                 dimension value is inserted
REPRODUCIBLE




                                                 into cell B3.
                                                 The next cell, C2, is
                                                 automatically selected.

                                          2. Double-click the
                                                 box_height




                                                                                                                         Lesson 5: Design Tables
                                                 dimension.
 257




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                                                                                                                           Lesson 5: Design Tables
                                          Inserting a New Design Table:
                                          3. Repeat this process for knob_dia, hole_dia,
                                             fillet_radius, and Depth.
                                                         Note: Since the depth dimensions of the Knob and the Box are
                                                         linked together, you only need one of them in the design table.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




                                          Excel tip: Dimension names tend to be very long. Use the Excel
                                          command Format Cells, and click Wrap Text on the Alignment tab.



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                                          Inserting a New Design Table:
                                          1. Enter new configuration names in column A:
                                                         Replace First Instance with blk1.
                                                         Fill cells A4 through A6 with blk2, blk3, and blk4.
REPRODUCIBLE




                                          2. Fill in the dimension values as shown below.




                                                                                                                         Lesson 5: Design Tables
 259




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                                                                                                                         Lesson 5: Design Tables
                                          To Close the Excel Worksheet:
                                          1. Click in the graphics area outside the worksheet.

                                          2. The system builds
                                             the configurations.
REPRODUCIBLE




                                          3. Click OK.
                                                 The Design Table is
                                                 embedded and
                                                 stored in the part document.
 SolidWorks 2001 Teacher Guide




                                          4. Save the part document.




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                                          To View Part Configurations:
                                          1. Click the Configuration-
                                             Manager tab     at the
                                             bottom of the Feature-
                                             Manager window.
REPRODUCIBLE




                                                 The list of configurations
                                                 is displayed.

                                          2. Double-click each
                                             configuration.




                                                                                                                         Lesson 5: Design Tables
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                                                                                                                         Lesson 5: Design Tables
                                          Viewing Part Configurations:
                                          3. The part is automatically rebuilt using the
                                             dimension values from the design table.
REPRODUCIBLE
 SolidWorks 2001 Teacher Guide




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         Lesson 6:
                 Revolve and Sweep
                 Features



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                                         Revolve Feature Overview
                                                 A Revolve feature is created by rotating a 2D
                                                 profile sketch around a centerline.

                                                 The profile sketch must contain the centerline.
REPRODUCIBLE




                                                 The profile sketch cannot cross the centerline.




                                                                                                                                  Lesson 6: Revolve and Sweep Features
                                                                       Good                       Good                  No Good
277




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                                                                                                                                     Lesson 6: Revolve and Sweep Features
                                         To Create a Revolve Feature:
                                         1. Select a sketch plane.                                                      Centerline


                                         2. Sketch a 2D profile.

                                         3. Sketch a centerline.
REPRODUCIBLE




                                                        The centerline must be in the sketch
                                                        with the profile. It cannot be in a
                                                        separate sketch.
                                                        The profile must not cross the
                                                        centerline.
SolidWorks 2001 Teacher Guide




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                                         Creating a Revolve Feature:
                                         4. Click Revolved Boss/Base                                               .

                                         5. Specify the angle of rotation and
                                            click OK.
REPRODUCIBLE




                                                        The default angle is 360°, which is right
                                                        99+% of the time.




                                                                                                                        Lesson 6: Revolve and Sweep Features
279




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Creating a Revolve Feature:
                                         6. The sketch is revolved around
                                            the centerline creating the
                                            feature.
REPRODUCIBLE
SolidWorks 2001 Teacher Guide




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                                         Sketching Arcs – 3 Point Arc
                                                 A 3 Point Arc creates an arc through three points –
                                                 the start, end and midpoint.

                                         To Create a 3 Point Arc:
REPRODUCIBLE




                                         1. Click 3 Pt Arc                              on the Sketch Tools toolbar.
                                         2. Point to the arc start location and
                                            click the left mouse button.




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         3. Move the pointer to the arc to the end
                                            location.
                                         4. Click the left mouse button again.
281




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Creating a 3 Point Arc:
                                         5. Drag the arc midpoint to
                                            establish the radius and
                                            direction (convex vs.
                                            concave).
REPRODUCIBLE




                                         6. Click the left mouse button a
                                            third time.
SolidWorks 2001 Teacher Guide




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                                         Sketching Arcs – Tangent Arc
                                                 The Tangent Arc tool creates
                                                 an arc that has a smooth                                               Not tangent
                                                 transition to an existing sketch
                                                 entity.
REPRODUCIBLE




                                                 Saves the work of sketching an                                         Tangent
                                                 arc and then manually adding
                                                 a geometric relation to make it
                                                 tangent.




                                                                                                                                      Lesson 6: Revolve and Sweep Features
                                                                                                                        Not tangent
                                                 Start point of the arc must
                                                 connect to an existing sketch
                                                 entity.
283




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                                                                                                                                             Lesson 6: Revolve and Sweep Features
                                         To Create a Tangent Arc:
                                         1. Click Tangent Arc     on the                                                  Arc is tangent
                                            Sketch Tools toolbar.                                                         to existing line

                                         2. Point to the arc start
REPRODUCIBLE




                                            location, and click the left
                                            mouse button.

                                         3. Drag to create the arc.                                                     Arc is tangent
                                                                                                                        to existing arc
                                                        The arc angle and radius values
                                                        are displayed on the pointer
SolidWorks 2001 Teacher Guide




                                                        when creating arcs.

                                         4. Click the left mouse button.


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                                         Pointer Feedback
                                                 As you sketch, the pointer provides feedback and
                                                 information about alignment to sketch entities and
                                                 model geometry.
REPRODUCIBLE




                                                                             Horizontal                         Midpoint

                                                                             Vertical                           Intersection

                                                                             Parallel                           End or Vertex




                                                                                                                                Lesson 6: Revolve and Sweep Features
                                                                             Perpendicular                      On

                                                                             Tangent
285




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                                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Inferencing
                                                 Dotted lines appear when you
                                                 sketch, showing alignment                                                     Orange

                                                 with other geometry.
REPRODUCIBLE




                                                 This alignment information is
                                                 called inferencing.                                                    Blue



                                                 Inference lines are two different colors: orange
                                                 and blue.
                                                        Orange inference lines capture and add a geometric relation
SolidWorks 2001 Teacher Guide




                                                        such as Tangent.
                                                        Blue lines show alignment and serve as an aid to sketching,
                                                        but do not actually capture and add a geometric relation.



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                                         Ellipse Sketch Tool
                                                 Used to create the sweep section for the handle of
                                                 the candlestick.

                                                 An Ellipse has two axes:
REPRODUCIBLE




                                                        Major axis, labeled A at the right.
                                                        Minor axis labeled B at the right.

                                                 Sketching an ellipse is a two-
                                                 step operation, similar to sketching a 3 Point Arc.




                                                                                                                        Lesson 6: Revolve and Sweep Features
287




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         To Sketch an Ellipse:
                                         1. Click Tools, Sketch Entity, Ellipse.
                                                        Tip: You can use Tools, Customize to add the Ellipse tool
                                                        to the Sketch Tools toolbar.
REPRODUCIBLE




                                         2. Position the pointer at the center of the ellipse.

                                         3. Click the left mouse
                                            button, and then move the
                                            pointer horizontally to
                                            define the major axis.
SolidWorks 2001 Teacher Guide




                                         4. Click the left mouse button
                                            a second time.


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                                         Sketching an Ellipse:
                                         5. Move the pointer vertically to
                                            define the minor axis.
REPRODUCIBLE




                                         6. Click the left mouse button a
                                            third time. This completes
                                            sketching the ellipse.




                                                                                                                        Lesson 6: Revolve and Sweep Features
289




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Fully Defining an Ellipse
                                         Requires 4 pieces of information:
                                                 Location of the center:
                                                        Either dimension the center or locate
                                                        it with a geometric relation such as
REPRODUCIBLE




                                                        Coincident.
                                                 Length of the major axis.
                                                 Length of the minor axis.
                                                 Orientation of the major axis.
                                                        Even though the ellipse at the right is
SolidWorks 2001 Teacher Guide




                                                        dimensioned, and its center is
                                                        located coincident to the origin, it is
                                                        free to rotate until the orientation of
                                                        the major axis is defined.


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                                         More About Ellipses
                                                 The major axis does not have to be
                                                 horizontal.
                                                 You can dimension half the major and/
                                                 or minor axis.
REPRODUCIBLE




                                                        It is like dimensioning the radius of a circle
                                                        instead of the diameter.

                                                 You do not have to use a
                                                 geometric relation to orient the




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                                 major axis.
                                                        A dimension works fine.
291




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Trimming Sketch Geometry
                                                 The Trim tool                         is used to delete a sketch
                                                 segment.

                                                 The segment is deleted up to its intersection with
REPRODUCIBLE




                                                 another sketch entity.

                                                 The entire sketch segment is deleted if it does not
                                                 intersect any other sketch entity.
SolidWorks 2001 Teacher Guide




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                                         To Trim a Sketch Entity:
                                         1. Click Trim    on the
                                            Sketch Tools toolbar.
                                         2. Position the pointer
                                            over the sketch
REPRODUCIBLE




                                            segment.
                                         3. The segment that will
                                            be trimmed is high-




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                            lighted in red.
                                         4. Click the left mouse
                                            button to delete the
                                            segment.
293




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                                                                                                                                  Lesson 6: Revolve and Sweep Features
                                         Sweep Overview
                                                 The Sweep feature is created                                           Section
                                                 by moving a 2D profile along
                                                 a path.
REPRODUCIBLE




                                                 A Sweep feature is used to
                                                                                                                           Path
                                                 create the handle on the
                                                 candlestick.

                                                 The Sweep feature requires
                                                 two sketches:
SolidWorks 2001 Teacher Guide




                                                        Sweep Path
                                                        Sweep Section




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                                         Sweep Overview – Rules
                                                 The sweep path is a set of sketched curves
                                                 contained in a sketch, a curve, or a set of model
                                                 edges.
REPRODUCIBLE




                                                 The sweep section must be a closed contour.

                                                 The start point of the path must lie on the plane of
                                                 the sweep section.




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                                 The section, path or the resulting solid cannot be
                                                 self-intersecting.
295




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Sweep Overview – Tips
                                                 Make the sweep path first. Then make the section.

                                                 Create small cross sections away from other part
                                                 geometry.
REPRODUCIBLE




                                                 Then move the sweep section into position by
                                                 adding a Coincident or Pierce relation to the end
                                                 of the sweep path.
SolidWorks 2001 Teacher Guide




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                                         To Create the Sweep Path:
                                         1. Open a sketch on
                                            Plane1 (Front).
                                         2. Sketch the Sweep
REPRODUCIBLE




                                            path using the Line
                                            and Tangent Arc
                                            sketch tools.

                                         3. Dimension as




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                            shown.

                                         4. Close the sketch.
297




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                                                                                                                                     Lesson 6: Revolve and Sweep Features
                                         To Create the Sweep Section:
                                         1. Open a sketch on Plane3 (Right).

                                         2. Sketch the Sweep section using
                                            the Ellipse sketch tool.
REPRODUCIBLE




                                         3. Add a Horizontal relation between
                                            the center of the ellipse and one
                                            end of the major axis.
                                                                                                                        Horizontal
                                         4. Dimension the major and minor
SolidWorks 2001 Teacher Guide




                                            axes of the ellipse.




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                                         Creating the Sweep Section:
                                         5. Add a Coincident relation
                                            between the center of the
                                            ellipse and the endpoint                                       Coincident
                                            of the path.
REPRODUCIBLE




                                         6. Close the sketch.




                                                                                                                        Lesson 6: Revolve and Sweep Features
299




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         To Sweep the Handle:
                                         1. Click Sweep                              on the Features
                                            toolbar.

                                         2. Select the Sweep path sketch.
REPRODUCIBLE




                                         3. Select the Sweep section sketch.

                                         4. Click OK.
SolidWorks 2001 Teacher Guide




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                                         Sweeping the Handle – Results
REPRODUCIBLE




                                                                                                                        Lesson 6: Revolve and Sweep Features
301




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                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         Extruded Cut with Draft Angle
                                                 Creates the opening for a candle in the top of the
                                                 candlestick.
                                                 Same process as extruding a boss except it
                                                 removes material instead of adding it.
REPRODUCIBLE




                                                 Draft tapers the shape.
                                                 Draft is important in molded,
                                                 cast, or forged parts.
                                                        Example: Ice cube tray – without
SolidWorks 2001 Teacher Guide




                                                        draft it would be very hard to get
                                                        the ice cubes out of the tray.
                                                        Find other examples.



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                                         To Create the Cut:
                                         1. Open a sketch on the top face of the
                                            candlestick.
REPRODUCIBLE




                                         2. Sketch a circular profile
                                            Concentric to the circular face.




                                                                                                                        Lesson 6: Revolve and Sweep Features
                                         3. Dimension the circle.
303




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                                                                                                                               Lesson 6: Revolve and Sweep Features
                                         Creating the Cut:
                                         4. Click Extruded Cut                                      on the Features toolbar.

                                         5. End Conditions:
                                                        Type = Blind
REPRODUCIBLE




                                                        Depth = 25mm
                                                        Draft = On
                                                        Angle = 15°

                                         6. Click OK.
SolidWorks 2001 Teacher Guide




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                                         Extruding the Cut– Results
REPRODUCIBLE




                                                                                                                        Lesson 6: Revolve and Sweep Features
305




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                                                                                                                                             Lesson 6: Revolve and Sweep Features
                                         Fillet Feature
                                                 Fillets are used to smooth the edges of the
                                                 candlestick.

                                         Selection Filters
REPRODUCIBLE




                                                 Help in selecting the correct geometry.

                                                 Click               to turn on Selection Filter toolbar.

                                                 Use the Edge selection filter                                          .
SolidWorks 2001 Teacher Guide




                                                 Pointer changes appearance                                                 when filter is
                                                 active.


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                                         Filleting the Edges – Results



                                                                                                                        Fillets
REPRODUCIBLE




                                                                                                                                  Lesson 6: Revolve and Sweep Features
307




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                                                                                                                                  Lesson 6: Revolve and Sweep Features
                                         Best Practice – Keep it Simple
                                                 Do not use a sweep feature
                                                 when a revolve or extrude will
                                                 work.
REPRODUCIBLE




                                                 Sweeping a circle along a
                                                 circular path appears to give the                                      Revolve

                                                 same result as a revolve feature.

                                                 However, the revolve feature:
SolidWorks 2001 Teacher Guide




                                                        Is mathematically less complex
                                                        Is easier to sketch – one sketch vs. two                        Sweep




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         Lesson 7:
                 Loft Features




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                                         Loft Feature Overview
                                                 Blends multiple profiles together.

                                                 A Loft feature can be a base, boss, or cut.

                                         To Create a Simple Loft Feature:
REPRODUCIBLE




                                         1. Create the planes required for
                                            the profile sketches
                                                 Each sketch should be on a
                                                 different plane.




                                                                                                                        Lesson 7: Loft Features
321




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                                                                                                                        Lesson 7: Loft Features
                                         Creating a Simple Loft Feature:
                                         2. Sketch a profile on
                                            the first plane.
                                         3. Sketch the remaining
                                            profiles on their
REPRODUCIBLE




                                            corresponding
                                            planes.
                                         4. Click Loft   on the
                                            Features toolbar.
SolidWorks 2001 Teacher Guide




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                                         Creating a Simple Loft Feature:
                                         5. Select each profile.

                                         6. Examine the preview
                                            curve.
REPRODUCIBLE




                                         7. Click OK.




                                                                                                                        Preview curve




                                                                                                                                        Lesson 7: Loft Features
323




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                                                                                                                        Lesson 7: Loft Features
                                         Additional Information About Lofts:
                                                 Neatness counts!
                                                        Select the profiles in order.
                                                        Click corresponding points on each profile.
                                                        The vertex closest to the selection point is used.
REPRODUCIBLE




                                                 A preview curve connecting
                                                 the profiles is displayed.

                                                 Review the curve in order to
                                                 address adjustments.
SolidWorks 2001 Teacher Guide




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                                         Neatness Counts!
                                         Unexpected results occur when you don’t pick corresponding
                                         points on each profile.
REPRODUCIBLE




                                                                                                                        Lesson 7: Loft Features
325




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                                                                                                                        Lesson 7: Loft Features
                                         Neatness Counts!
                                         Rebuild errors can occur if you select the
                                         profiles in the wrong order.
REPRODUCIBLE
SolidWorks 2001 Teacher Guide




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                                         To Create an Offset Plane:
                                         1. Select Plane1.

                                         2. Click     on the Reference Geometry toolbar, or
                                            click Insert, Reference Geometry, Plane.
REPRODUCIBLE




                                                                                                                        Lesson 7: Loft Features
                                         3. Click Offset for Step 1 of 2.
                                         4. Click Next.
327




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                                                                                                                        Lesson 7: Loft Features
                                         Creating an Offset Plane:
                                         5. Enter 25mm for
                                            Distance.

                                         6. Look at the preview
REPRODUCIBLE




                                            on the screen to
                                            verify that the offset
                                            is going in the correct
                                            direction.
                                                 If it is not, click Reverse direction.
SolidWorks 2001 Teacher Guide




                                         7. Click Finish.



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                                         Creating an Offset Plane – Results
REPRODUCIBLE




                                                                                                                        Lesson 7: Loft Features
329




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                                                                                                                        Lesson 7: Loft Features
                                         Setting up the Planes
                                         Additional offset planes are required.

                                                 Plane5 is offset 25mm
                                                 from Plane4.
REPRODUCIBLE




                                                 Plane6 is offset 40mm
                                                 from Plane5.

                                                 Verify the positions of the
                                                 planes.
SolidWorks 2001 Teacher Guide




                                                        Click View, Planes.
                                                        Double-click the planes to see
                                                        their offset dimensions.



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                                         Sketch the Profiles
                                                 The Base-Loft feature is created with 4 profiles.

                                                 Each profile is on a separate plane.

                                         To Create the First
REPRODUCIBLE




                                         Profile:
                                         1. Open a sketch on Plane1.

                                         2. Sketch a square.




                                                                                                                        Lesson 7: Loft Features
                                         3. Exit the sketch.
331




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                                                                                                                        Lesson 7: Loft Features
                                         Best Practice
                                         There is a better way to sketch a centered square:
                                         1. Sketch a rectangle.
                                         2. Sketch a centerline from
                                            corner to corner.
REPRODUCIBLE




                                         3. Relate the centerline to the
                                            origin with a Midpoint
                                            relation. This keeps the
                                            rectangle centered.
SolidWorks 2001 Teacher Guide




                                         4. Add an Equal relation to one horizontal and one
                                            vertical line. This makes the rectangle a square.
                                         5. Dimension one side of the square.

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                                         Sketch the Remaining Profiles:
                                         1. Open a sketch on Plane4.

                                         2. Sketch a circle and dimension it.

                                         3. Exit the sketch.
REPRODUCIBLE




                                         4. Open sketch on Plane5.

                                         5. Sketch a circle whose
                                            circumference is coincident with
                                            the corners of the square.




                                                                                                                        Lesson 7: Loft Features
                                         6. Exit the sketch.
333




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                                                                                                                                  Lesson 7: Loft Features
                                         To Copy a Sketch:
                                         1. Select Sketch3 in the FeatureManager design
                                            tree or graphics area.

                                         2. Click Copy                              on the Standard
REPRODUCIBLE




                                            toolbar.

                                         3. Select Plane6 in the
                                            FeatureManager design tree or
                                            graphics area.
SolidWorks 2001 Teacher Guide




                                         4. Click Paste                             .                                   Sketch4

                                                 A new sketch, Sketch4, is created on Plane6.


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                                         More About Copying Sketches
                                                 External relations are deleted.
                                                 For example, when you copied Sketch3, the
                                                 geometric relations locating the center and
                                                 defining the circumference were deleted.
REPRODUCIBLE




                                                 Therefore, Sketch4 is underdefined.
                                                 To fully define Sketch4, add a Coradial relation
                                                 between the copied circle and the original.
                                                 If you sketch a profile on the wrong plane, move it




                                                                                                                        Lesson 7: Loft Features
                                                 to the correct plane using Edit Sketch Plane. Do
                                                 not copy it.
335




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                                                                                                                        Lesson 7: Loft Features
                                         To Move a Sketch to a Different
                                         Plane:
                                         1. Right-click the sketch in the
                                            FeatureManager design tree.
REPRODUCIBLE




                                         2. Select Edit Sketch Plane from the
                                            shortcut menu.



                                         3. Select a different plane.
SolidWorks 2001 Teacher Guide




                                         4. Click Apply.



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                                         Base-Loft Feature
                                         The Base-Loft feature blends the
                                         4 profiles to create the handle of
                                         the chisel.
REPRODUCIBLE




                                         1. Click Loft                          on the Features toolbar.




                                                                                                                        Lesson 7: Loft Features
337




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                                                                                                                                        Lesson 7: Loft Features
                                         Creating the Base-Loft Feature:
                                         2. Select each profile.
                                                 Click on each sketch in the
                                                 same relative location –
                                                 the right side.
REPRODUCIBLE




                                         3. Examine the preview
                                            curve.
                                                 The preview curve shows
                                                 how the profiles will be
SolidWorks 2001 Teacher Guide




                                                 connected when the loft                                                Preview curve
                                                 feature is created.



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                                         Creating the Base-Loft Feature:
                                         4. The sketches are listed in the Profiles
                                            box.
REPRODUCIBLE




                                                 The Up/Down arrows are used to
                                                 rearrange the order of the profiles.




                                                                                                                        Lesson 7: Loft Features
339




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                                                                                                                        Lesson 7: Loft Features
                                         Creating the Base-Loft Feature:
                                         5. Click OK.
REPRODUCIBLE
SolidWorks 2001 Teacher Guide




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                                         A Second Loft Feature Creates the
                                         Bit of the Chisel:
                                                 The Boss-Loft Feature is composed of two
                                                 profiles: Sketch5 and Sketch6.
REPRODUCIBLE




                                         To Create Sketch5:
                                         1. Select the square face.

                                         2. Open a sketch.

                                         3. Click Convert Entities                                       .




                                                                                                                        Lesson 7: Loft Features
                                         4. Exit the sketch.
341




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                                                                                                                        Lesson 7: Loft Features
                                         To Create Sketch6:
                                         1. Offset Plane7 behind
                                            Plane1.
                                                 Press and hold Ctrl, and
                                                 drag Plane1 to create
REPRODUCIBLE




                                                 the new plane.

                                         2. Double-click Plane7 to
                                            display its offset
                                            dimension.
SolidWorks 2001 Teacher Guide




                                         3. Double-click the dimension, change the value to
                                            200mm, and click Rebuild     .


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                                         To Create Sketch6:
                                         4. Open a sketch on Plane7.

                                         5. Sketch a narrow rectangle.

                                         6. Dimension the rectangle.
REPRODUCIBLE




                                         7. Exit the sketch.




                                                                                                                        Lesson 7: Loft Features
343




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                                                                                                                                            Lesson 7: Loft Features
                                         To Create the Boss-Loft Feature:
                                         1. Click Loft                          on the Features toolbar.
                                         2. Select Sketch5 in
                                            the lower right corner
                                            of the square.
REPRODUCIBLE




                                                                                                                        Sketch6
                                         3. Select Sketch6 in
                                            the lower right corner
                                                                                                                                  Preview
                                            of the rectangle.
                                                                                                                             Sketch5
                                         4. Examine the preview
SolidWorks 2001 Teacher Guide




                                            curve.
                                         5. Click OK.


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                                         Finished Chisel
REPRODUCIBLE




                                                                                                                        Lesson 7: Loft Features
345




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                                                                                                                        Lesson 7: Loft Features
                                         Tips and Tricks
                                         Remember best practices:
                                                 Only two dimensions are
                                                 required for the narrow
REPRODUCIBLE




                                                 rectangle.

                                                 Use a centerline and a
                                                 Midpoint relation to center
                                                 the rectangle.
SolidWorks 2001 Teacher Guide




                                                 This technique eliminates two dimensions and it
                                                 captures the design intent.



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                                         Tips and Tricks
                                                 You do not need
                                                 Sketch5 (the
                                                 sketch with the
                                                 converted edges of
REPRODUCIBLE




                                                 the square face).

                                                 Loft can use the face
                                                 as a profile.

                                                 Select the face near
                                                 the corner.




                                                                                                                        Lesson 7: Loft Features
347




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         Lesson 8:
                 Visualization




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                                         What is
                                         PhotoWorks?
                                         A software application that
                                         creates realistic images from
                                         SolidWorks models.
REPRODUCIBLE




                                         PhotoWorks uses rendering
                                         effects such as:

                                                 Materials                                        Shadows

                                                 Lights                                           Backgrounds




                                                                                                                        Lesson 8: Visualization
363




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                                                                                                                        Lesson 8: Visualization
                                         Shaded Rendering
                                                 The basis for images in
                                                 PhotoWorks.

                                                 Shaded Rendering requires a
REPRODUCIBLE




                                                 material.

                                                 The default material is Polished
                                                 Plastic.
                                         To display the Shaded Rendering:
SolidWorks 2001 Teacher Guide




                                                 Click Render                          on the PhotoWorks toolbar.




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                                         Materials
                                         Materials specify the properties of a
                                         model’s surface.
                                         Properties are:
REPRODUCIBLE




                                                 Color

                                                 Texture

                                                 Reflectance

                                                 Transparency




                                                                                                                        Lesson 8: Visualization
365




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                                                                                                                        Lesson 8: Visualization
                                         Materials
                                         Categorized as:
                                                 Procedural materials – defined by a series of
                                                 steps that determine:
REPRODUCIBLE




                                                        Color
                                                        Reflectance
                                                        Displacement (roughness)

                                                 Texture mapped materials – wraps a 2D image
SolidWorks 2001 Teacher Guide




                                                 around the selected surface(s) of the model.




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                                         Stock Procedural Material – Metal
                                         To apply the Chrome material:

                                         1. Click Materials                                 on the PhotoWorks toolbar.

                                         2. Double-click Stock Procedural.
REPRODUCIBLE




                                         3. Click Metals.

                                         4. Select Chrome.

                                         5. Click Apply, Close.




                                                                                                                         Lesson 8: Visualization
                                         6. Click Render                              .
367




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                                                                                                                        Lesson 8: Visualization
                                         Materials Editor – Chrome
REPRODUCIBLE
SolidWorks 2001 Teacher Guide




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                                         Stock Procedural Material – Brick
                                                 The Primary color determines the brick color.

                                                 The Secondary color determines the mortar color
                                                 between the bricks.
REPRODUCIBLE




                                                 The Pattern scale modifies the size of the bricks.

                                         To customize the properties for Brick:
                                         1. Click Materials                                 on the PhotoWorks toolbar.

                                         2. Double-click Stock Procedural.




                                                                                                                         Lesson 8: Visualization
                                         3. Click Stones, and then click Brick.
369




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                                                                                                                        Lesson 8: Visualization
                                         Customizing the Properties for Brick:
                                         4. Click the Color tab.

                                         5. Click Edit for the Primary color (bricks).

                                         6. Select a color from the color palette, and click OK.
REPRODUCIBLE




                                         7. Click Edit for the Secondary color (mortar).

                                         8. Select a color from the color palette, and click OK.

                                         9. Enter 0.5 in the Pattern scale box.
SolidWorks 2001 Teacher Guide




                                       10. Click Apply, and then click Close.

                                       11. Click Render                               .

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                                         Materials Editor – Brick
REPRODUCIBLE




                                                                                                                        Lesson 8: Visualization
371




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                                                                                                                        Lesson 8: Visualization
                                         Image Background
                                         The portion of the graphics area not
                                         covered by the model.
                                                 Background styles vary in complexity and
REPRODUCIBLE




                                                 rendering speed.

                                                 Background styles controlled by Scene Editor.

                                                 Incorporate advanced rendering effects into a
                                                 PhotoWorks Scene.
SolidWorks 2001 Teacher Guide




                                                        Shadows
                                                        Reflections



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                                         Scene Editor – Clouds
REPRODUCIBLE




                                                                                                                        Lesson 8: Visualization
373




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                                                                                                                        Lesson 8: Visualization
                                         To Change the Background Style
                                         to Clouds:
                                         1. Click Scene    on
                                            the PhotoWorks
REPRODUCIBLE




                                            toolbar.
                                         2. Click the
                                            Background tab.
                                         3. Select Clouds from
                                            the Style list.
SolidWorks 2001 Teacher Guide




                                         4. Enter 2 for Scale.
                                         5. Click OK


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                                         To Save the Image File
                                         1. Click Options                                 on the PhotoWorks toolbar.

                                         2. Click the Image Output
                                            tab.
REPRODUCIBLE




                                         3. Click Render to file.
                                                        The image file name is based
                                                        on the model name.
                                                        The default file type is *.bmp.

                                         4. Enter a file name and click
                                            OK.




                                                                                                                        Lesson 8: Visualization
                                         5. Click Render                              .
375




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                                                                                                                        Lesson 8: Visualization
                                         SolidWorks Animator Application
                                         What is SolidWorks Animator?
                                                 SolidWorks Animator animates and captures
                                                 motion of SolidWorks parts and assemblies.
REPRODUCIBLE




                                                 SolidWorks Animator generates Windows-based
                                                 animations (*.avi files). The *.avi file uses a
                                                 Windows-based Media Player.

                                                 SolidWorks Animator can be combined with
SolidWorks 2001 Teacher Guide




                                                 PhotoWorks.




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                                         Renderer Options
                                         The Renderer affects the quality of the
                                         saved image. There are two options:
                                                 SolidWorks screen
REPRODUCIBLE




                                                 PhotoWorks buffer




                                                                                                                        Lesson 8: Visualization
377




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                                                                                                                         Lesson 8: Visualization
                                         Factors Affecting File Size
                                                 Number of frames per second

                                                 Renderer used
                                                        PhotoWorks buffer creates a larger file than SolidWorks screen
REPRODUCIBLE




                                                 If using PhotoWorks buffer:
                                                        Materials
                                                        Background
                                                        Shadows
                                                        Multiple-light sources
SolidWorks 2001 Teacher Guide




                                                 Video compression

                                                 Key frames

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                                         To Create an Exploded View:
                                         1. Click Open     on the Standard
                                            toolbar, and open the assembly,
                                            Tutor.
REPRODUCIBLE




                                         2. Click Insert, Exploded
                                            View...




                                                                                                                        Lesson 8: Visualization
                                                 The Assembly Exploder
                                                 dialog box appears.
379




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                                                                                                                        Lesson 8: Visualization
                                         Creating an Exploded View:
                                         3. Click New    on the Step
                                            Editing toolbar to begin a
                                            new explode step.
                                                 The dialog box expands to
REPRODUCIBLE




                                                 show selection lists for:
                                                        Direction to explode along
                                                        Components to explode
                                                        Distance
SolidWorks 2001 Teacher Guide




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                                         Creating an Exploded View:
                                         4. Click the flat face on the front
                                            of the Tutor1 component.
                                                 An arrow appears that is
                                                 perpendicular to the selected
REPRODUCIBLE




                                                 face and the name Face of
                                                 Tutor1<1> appears in the
                                                 Direction to explode along list.




                                                                                                                        Lesson 8: Visualization
381




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                                                                                                                        Lesson 8: Visualization
                                         Creating an Exploded View:
                                         5. Select the Tutor1
                                            component.
                                                 The component name
                                                 appears in the Components
REPRODUCIBLE




                                                 to Explode list.

                                         6. Set the Distance to 70mm
                                            and click Apply    on the
                                            Step Editing toolbar.
SolidWorks 2001 Teacher Guide




                                         7. Since there is only one component to explode, this
                                            completes making the exploded view. Click OK to
                                            close the Assembly Exploder dialog box.

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                                         Creating an Exploded View:
                                         8. Results.
                                                 Note: Exploded views are
                                                 related to and stored in
                                                 configurations. You can
REPRODUCIBLE




                                                 only have one exploded
                                                 view per configuration.




                                                                                                                        Lesson 8: Visualization
383




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                                                                                                                        Lesson 8: Visualization
                                         Collapsing an Exploded View:
                                                 Right-click in the FeatureManager design tree, and
                                                 select Collapse from the shortcut menu.

                                         To Explode an Existing Exploded
REPRODUCIBLE




                                         View:
                                         1. Switch to the ConfigurationManager.
                                         2. Expand the configuration that contains the
SolidWorks 2001 Teacher Guide




                                            exploded view.
                                         3. Right-click the exploded view, and select Explode
                                            from the shortcut menu.

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