D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
1
FEMAP Tutorial 2: Plate with a Hole
Now that we have constructed a few simple models in FEMAP, we may move on to
structures a little more complicated. In this tutorial we will model the picture above in
order to familiarize you with more of FEMAP’s modeling tools. We will only create the
plate and the hole that the rod passes through. Then, we will constrain the hole to
simulate the presence of the rod (assuming it will not deform or bend). We will specify
four types of information for the plate:
Constitutive – What the model is comprised of (materials, properties)
Geometry – The shape of the model
Boundary conditions – Loads and constraints acting on the model
Compatibility – How the elements fit together
Don’t forget to save the model under different filenames as you complete major
sections. When you are finished, you should have seven or eight files of the model at the
different stages of its construction to avoid having to start from a clean slate in order to
change one aspect of it.
Here is another useful feature to use. Click on the tiny square right above the time in the
bottom, right hand corner of the screen that says ‘Off’. This will turn on a window that
will pop-up and provide information about a specific entity when you move your mouse
over that entity. For instance, if you click on ‘Off’ and then select node, when you move
the mouse over the nodes on the screen, they will become highlighted. In addition, if you
move your mouse over one node, it will tell you its Node ID # and its Coordinates. This
can be useful to find information about a specific curve, element, or node.
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
2
File.New
File.Save As…(FemapTut2)
Define the workspace…See Tutorial 1
Define Material Group…See Tutorial 1
Define Property Set…See Tutorial 1
One change from Tutorial 1: Element Property Type: Plate (check)
Model Geometry
The plate that will be created involves more complicated geometry than the previous
rod/beam and base example. We will begin by creating the plate.
Part 1: Plate
Geometry.Point…
X(0) Y(0) Z(0) OK Here we create points that
X(4) Y(0) Z(0) OK will become the plate, as
X(8) Y(0) Z(0) OK is shown below
X(12) Y(0) Z(0) OK
X(0) Y(3) Z(0) OK
X(4) Y(3) Z(0) OK
X(8) Y(3) Z(0) OK
X(12) Y(3) Z(0) OK
X(0) Y(6) Z(0) OK
X(4) Y(6) Z(0) OK
X(8) Y(6) Z(0) OK
X(12) Y(6) Z(0) OK
Cancel
View.Autoscale.All (or Press Ctrl – A ) Autoscale the screen to fit the model.
Geometry.Curve – Line.Points…
Create Line From Points.(Select the first and second endpoint for the line using the
mouse)
OK
Repeat until rectangular plate has been drawn using the points created. Your screen
should resemble the picture below. Superelements are numbered for reference.
Cancel V1
Y
10.
9.5
9.
8.5
8.
7.5
7.
6.5
6.
5.5
5.
4.5
1 2 3
4.
3.5
3.
2.5
2.
1.5
1.
0.5
0.
4 5 6
-0.5
-1.
-1.5
-2.
-2.5
-3.
-3.5
-4.
Y -4.5
-5.
-5.5
Z X -6.
-6.5
-7.
-7.5
-8.
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
3
Fillets
Now the corners will be filleted. This command takes a sharp corner where two line
segments intersect and creates a smooth curve of a specified radius. Creating fillets in a
model is a valuable skill when attempting to reduce stress concentrations.
BEFORE AFTER
Center of Fillet When selecting the curves to be filleted,
select them by placing the mouse inside the
radius of the fillet that will be formed (dotted
line in schematic), allowing the program to
highlight the curve. Then click to select it.
This tells the program where the center of
the fillet should be.
Modify.Fillet… (or Press Ctrl-F)
Curve 1 (Select top horizontal side of “superelement” 1 by moving the mouse near
the curve. It is important to keep the crosshair inside “superelement” 1 at least 0.5
units away from the curve being selected.)
Curve 2 (Select left vertical side of “superelement” 1 by moving the mouse near the
curve. It is important to keep the crosshair inside “superelement” 1 at least 0.5 units
away from the curve being selected.)
Radius(2)
Trim Curve 1 (check)
Trim Curve 2 (check)
OK
Repeat with superelements 3,4, and 6
Part 2: The Cutout
Now that we have the plate created, we may draw a cutout in the plate that will not be
meshed, creating a hole in the structure.
Geometry.Curve – Circle.Center…
X(2) Y(3) Z(0) The circle will provide the
OK curved part of the D-shaped
Radius(1.5) cutout
OK
Cancel
Geometry.Curve – Line.Project Points…
X(1.5) Y(5.5) Z(0) This vertical line will form
OK the vertical side of the D-
X(1.5) Y(0.5) Z(0) shaped cutout
OK
Cancel
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
4
Trimming
Trimming is a powerful command that cuts curves you have drawn at the points they
intersect with other curves. This helps you to define complex geometries. Depending on
where you select the curve to be trimmed, part of the curve will remain and part of it will
be removed from the model. To trim, you must have two or more curves: the cutting
curves and the curves being trimmed. The following commands trim the vertical line first
(first the bottom of the line and then the top of the line,) and then we will trim the circle.
Modify.Trim (or Press Ctrl – I )
Entity Selection – Select Curve(s) to use as Cutting Edges (Select circle) This specifies the circle as
OK the cutting line.
Trim Curve (Select the bottom of the vertical line outside the circle using the
mouse – as indicated by the arrow below)
OK
Selecting near the bottom of the line fills in the
‘remove near fields’
Entity Selection – Select Curve(s) to use as Cutting Edges.(Select circle) This specifies the circle as
OK the cutting line.
Trim Curve (Select the top of the vertical line outside the circle using the mouse -
as indicated by the arrow below)
OK
This forms the D-shaped
cutout. Now we must
remove the remaining part
of the circle.
Entity Selection – Select Curve(s) to use as Cutting Edges.(Select vertical line through
circle) This specifies the vertical line as the cutting edge.
OK
Trim Curve (Select the left side of the circle – as indicated by the arrow below )
OK
The trimming resulted in a two edged-
sword for the circle.
I am not exactly sure what Brian Mente
meant by this line. Correct as you see
fit.
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
5
Entity Selection – Select Curve(s) to use as Cutting Edges. (Select vertical line of the D,
as well as top and bottom half of arc of the D – as indicated by the arrow below)
OK
This command is more for
aesthetic value for the
model.
Trim Curve (Select the horizontal line running through the center of the D)
OK
Cancel
The model should now appear as follows, without the number labels:
V1
1 2 3
4 5 6
Y
Z X
Creating the Mesh
Now that the shape of the model has been created, we can subdivide the ‘superelements’
to create our mesh. Previously the ‘Mesh.Between…’ command was used, but now the
geometry of superelements 1 and 4 are too complicated for that command to be effective.
Thus, a new approach will be taken. Boundary surfaces will be created, and the program
will automatically mesh them using our specifications .
First, the ‘Break’ command must be used to ensure that each superelement is bounded by
the intersecting curves.
Modify.Break… (or Press Ctrl – K)
Entity Selection – Select Curves to Break (Select vertical side of D-shaped cutout)
OK
Locate – Enter Location to Break At
X(1.5) Y(3) Z(0) The single line has now
OK been broken into two lines
Cancel
Now the boundary surfaces can be defined to mesh these complicated sections. The
boundaries of each superelement must form a single, enclosed loop for the mesh
command to be accomplished.
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
6
Geometry.Boundary Surface.From Curves…
Entity Selection – Select Curves on a Closed Boundary
(Select the eight curves that bound superelement 1)
OK
Repeat with Superelement 3, 4, and 6
Cancel
Now the size, shape, and properties of the mesh must be determined on these
superelements.
Mesh.Mesh Control.Size On Surface…
Entity Selection – Select Surfaces to Set Mesh Size
(Select superelements 1,3,4 and 6)
0.3 is chosen to determine that there will be
OK
ten elements along the vertical sides of the
Automatic Mesh Sizing
superelements, which have a length of .3
Element Size (0.3)
Surface Interior Mesh Growth.Growth Factor(1.0) (check) This will ensure that all
OK elements are roughly the
Cancel same size.
Mesh.Geometry.Surface…
Entity Selection – Select Surfaces to Mesh
(Select superelements 1,3,4 and 6)
OK
Property(Select 1/4” Steel)
OK Now mesh superelements 2
and 5 using the technique
Mesh.Between… (or Control – B) learned in Tutorial 1.
Node And Element Options.Property(1..1/4” Steel)
Mesh Size.#Nodes.Dir1(11)
Mesh Size.#Nodes.Dir2(11)
OK
X(4) Y(0) Z(0) OK
X(8) Y(0) Z(0) OK
X(8) Y(3) Z(0) OK
X(4) Y(3) Z(0) OK
Mesh.Between… (or Control – B)
Node And Element Options.Property(1..1/4” Steel)
Mesh Size.#Nodes.Dir1(11)
Mesh Size.#Nodes.Dir2(11)
OK
X(4) Y(3) Z(0) OK
X(8) Y(3) Z(0) OK
X(8) Y(6) Z(0) OK
X(4) Y(6) Z(0) OK
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
7
You should have a complete mesh that resembles the following picture:
V1
Y
Z X
Now we must combine our superelements into one structure to satisfy our compatibility
requirement. To apply compatibility, the “Check Coincident Nodes” command is used,
which combines nodes that occupy the same location (“coinciding” in the same place).
By combining these nodes, the superelements are then ‘connected’ by these shared nodes.
If you neglect to do combine the nodes, it will be easy to notice that in the analysis
results, the model will be disjointed along those boundaries.
Tools.Check.Coincident Nodes…
Entity Selection.Select All
OK
OK to specify additional range of nodes to merge? Yes
Entity Selection.Select All
OK
Options.Merge Coincident Entities(check)
OK
Loads and Constraints
In this example, we will be constraining the hole to represent the presence of the rod, and
we will apply tensile loads in different directions.
Create a constraint set
Model.Constraint.Set… (or Shift-F2)
Title(ConstraintSet1)
OK
Specify the constraints
Specifying the constraints along a geometric feature of a model can be useful while
selecting nodes along the side can be tedious.
Model.Constraint.On Curve…
Entity Selection.(Select the four curves that make up the D-shaped cutout)
OK
Create Constraints on Geometry.DOF.Fixed(check)
OK
Cancel
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
8
Create a load set
We will now create a single active load set that will consist of two separate applied
loads. As long as a another new load set is defined (ex. LoadSet2, making this the active
set) or the active load set is not reset, all loads applied to the model will be placed under
LoadSet1. These loads will also be defined along curves of the model.
Model.Load.Set… (or Control-F2)
Title(LoadSet1)
OK
Specify the loading
Model.Load.On Curve…
Entity Selection.(Select the four curves that make up the right side of the model) As shown below
V1
1
2
3
4
Y
Z X
OK
(Select Force Per Length off of the list of choices)
Load.FX.Value(1000)
OK
Cancel
Model.Load.On Curve…
Entity Selection.(Select the identical four curves that make up the left side of the
model)
OK
(Select Force Per Length off of the list of choices)
Load.FX.Value(-1000)
OK
Cancel
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
9
Model Analysis
CAEFEM performs analysis using FEMAP generated models. We will export our model
to CAEFEM and command it to perform our choice of the type of analysis. CAEFEM
will automatically import the results back into FEMAP.
File.Export.Analysis Model… (or Press Ctrl – T)
Export To.CAEFEM(check)
OK
OK to save model? Yes
The CAEFEM analysis window will now automatically open. The following section
refers to commands in this window.
Constraint Set (Select ConstraintSet1)
LoadSet (Select LoadSet1)
Analysis Options
Run
Results Generation.Linear Static(check)
OK
Post-Processing
Post-Processing allows us to view the stress contours and displacements on our model.
These contours and displacements are the results generated from the CAEFEM analysis.
View.Select… (or Press F5)
Deformed Style.Deform(check)
Contour Style.Contour(check)
Deformed and Contour Data…
Output Vectors.Deformation(1..Total Translation)
Output Vectors.Contour(7033..Plt Top vonMises)
OK
OK
Let’s imagine that this particular steel has
View.Options… (or Press F6) been known to fail at stress levels over
Category.PostProcessing(check) 6750. We may adjust the contouring on the
Options(Select Countour/Criteria Levels on list) model to show red regions when the stress
Level Mode (Select 3..User Defined) is at or above this level. You must set the
Maximum(7200) maximum value for a small percentage
Apply greater than 6750 so that all red regions
OK will indicate failure.
D:\Docstoc\Working\pdf\d0c5347f-48f1-4fc2-9e2e-c4c7b8ac9464.doc
10
The final model should look similar to this:
V1
L1 7200.
C1
6750.
6300.
5850.
1000. 1000. 5400.
1000. 4950.
1000.
4500.
1000. F 1000.
F 4050.
1000. F 1000.
F 3600.
1000. 1000.
F 3150.
1000. F 1000.
F
2700.
F
1000. 1000.
2250.
1000. 1000.
1800.
1350.
Y
900.
Z X 450.
Output Set: CAEFEM (C:1 L:1)
Deformed(0.00163): Total Translation 0.
Contour: Plt Top vonMises