Exercise 1 - Analyzing a Solid Part

SAVE OFFLINE

Exercise 1 – Analyzing a Solid Part

Introduction In this exercise, you perform a linear stress analysis of a lower control arm using the following process:  Set Femap Preferences to use millimeters as the Geometry

Scale Factor and to use the extended metal alloy material database and other settings.  Import a Parasolid solid.  Assign a material and a property to the control arm.  Apply Constraints and Loads to the geometry.  Mesh the control arm.  Create an Analysis Set and submit to NX Nastran to complete the analysis.  Display the results. The preferences and units used in this exercise are: Solid Geometry Scale Factor: Millimeters Force:

N

Pressure:

MPa

Density:

Tonne / mm3

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 1

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Step 1: Start Femap and Set Preferences Start Femap.  From either a desktop icon, or from the Windows Start menu, select the icon for Femap v11. Close the Data Table and the Program File panes.  From the Panes toolbar, click the Data Table and Program File icons as shown below.

By clicking these icons, you have executed the Tools, Data Table and Tools, Programming, Program File commands.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 2

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Close and open toolbars.  Select the command, Tools, Toolbars, Customize. You can also right-click in an area near one of the docked toolbars and select Customize from the context-sensitive menu.  In the Customize dialog box, select the Toolbars tab.  Scroll to the bottom of the Toolbars: list and uncheck the boxes for both the SAToolkit and TMG Panel toolbars. This action will close these toolbars.

 Scroll up in the list and check the box for the View Orient toolbar to open it. Drag the toolbar to a preferred position.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 3

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Set your Femap preferences for the correct Geometry Scale Factor. The Geometry Scale Factor is number of length units per meter used by Parasolid.  Select the command, File, Preferences.  In the Preferences dialog box, select the Geometry/Model tab.  Under the Geometry Preferences option group, set the Geometry Scale Factor to Millimeters.

 Click OK to apply the changes and close the dialog box.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 4

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Step 2: Import the solid geometry of the lower control arm. Import a Parasolid geometry file of the Lower Control Arm.  Click the Import Geometry icon on the Main toolbar. By clicking this icon, you have executed the File, Import,

Geometry command.

 In the Geometry File to Import dialog box, navigate to the class Geometry folder and select the Parasolid file (.x_t file extension) ex1-LowerControlArm.x_t.

 Click Open to import the Parasolid file.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 5

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Solid Model Read Options dialog box, click OK to read in the lower control arm. The value for the Geometry Scale Factor should be the same as the Geometry Scale Factor you set for Femap’s preference (1000).

 Click OK to import the geometry.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 6

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Your Femap model should appear similar to the following (you will have a dark gradient background).

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 7

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Save the model.  Click the Save Model icon on the Model toolbar to execute the File, Save command.

 In the File, Save As dialog box, navigate up one folder to select the Exercises folder.  Enter Ex1-LowerControlArm as the name of the Femap model file. The .modfem extension for Femap models will be automatically appended to the name.



Click Save to complete saving the Femap model file.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 8

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Step 3: Create and assign the material and property to the part. Create an aluminum material.  In the Model Info pane, expand the Model tree by clicking the + icon to the left of Model in the tree.  Right-click Materials and select New from the contextsensitive menu. This is the same action as selecting the command, Model, Material.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 9

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Define Material – ISOTROPIC dialog box, enter the values for the Title, Young’s Modulus, Poisson’s Ratio,

Tension (Limit Stress) and Mass Density as shown in the table below.

Dialog Box Field

Title Young’s Modulus, E Poisson’s Ratio, nu (Limit Stress) Tension Mass Density

CT2060

Value Aluminum 68950 0.33 225 2.71e-9

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 10

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 Click OK in the Define Material dialog box to complete creating the material.  Since the Femap preference to Autorepeat Create

Commands option is enabled, you will continue to create materials until the command is cancelled. Click Cancel or press the Esc key to exit the material creation command. Note: If you create a material with E and/or G and Nu equal to zero, you will get a fatal error when running an analysis with NX Nastran and most other solvers. Review the material attributes in the Entity Editor pane.  Expand the Materials tree in the Model Info pane.  Select the Aluminum material. Note how the material appears in the Entity Editor pane.  Double-click the title bar of the Entity Editor pane to undock it.  Resize the window so that you can view all the attributes of the material.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 11

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 Select one of the attributes such as E, G, or Nu. Note how a description of the attribute and its value is displayed on the bottom Entity Editor pane.

 Dock the Entity Editor by double-clicking its title bar.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 12

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Create the solid property for the lower control arm.  In the Model Info pane, right-click the Properties object and select New from the context-sensitive menu.

 In the Define Property – PLATE Element Type dialog box, click the Elem/Property Type… button.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 13

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Element / Property Type dialog box, select Solid.

 Click OK to apply the selection and to update the Define

Property dialog box

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 14

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 In the Define Property dialog box, enter Lower Control Arm as the Title.  Set the Material to 1..Aluminum.

 Click OK to create the property.  Click Cancel or press the Esc key to end the property creation command.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 15

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Enable and set options for highlighting of selected entities.  In the Model Info pane, select the Show When Selected icon menu.

 By default, highlighting is turned off in new models. Select either Highlight or Transparent Highlight from the Show

When Selected pulldown menu.  Reselect the Show When Selected menu and select Show Labels to turn off display of labels when selected entities are highlighted.  Optionally, you can select Highlight Color… to change the highlight color to one you prefer. CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 16

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Note - To toggle highlighting on and off, you simply click the

Show When Selected icon. If highlighting is enabled, the Show When Selected icon shown as a filled box as displayed below.

Default settings for type of highlighting (Highlight,

Transparent Highlight, or Show Selected Only), Show Labels toggle, Show Normals toggle, and Highlight Color can be set by using the File, Preferences command and choosing the User Interface tab.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 17

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Apply the newly created property as the Mesh Attribute to the lower control arm. A Mesh Attribute is the Property that is used when meshing geometry.  Expand the Geometry tree in the Model Info pane by clicking the

icon.

 Click the Lower Control Arm solid. Note how the part is highlighted in the graphics window.  Right-click Lower Control Arm in the Model Info pane and select Attributes from the context-sensitive menu.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 18

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 In the Select Mesh Property dialog box, select 1..Lower Control Arm.

 Click OK to confirm your selection and to assign the property as a Mesh Attribute to the lower control arm. Note - To refresh the display remove highlighting, press the Ctrl+g shortcut key combination.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 19

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Step 4: Create constraints and loads for the lower control arm. Display the Constraint and Loads toolbars.  Right-click in an area next to one of the other toolbars and select Loads from the context-sensitive menu.

 Repeat the previous step to select Constraints from the context-sensitive menu.  Move the two toolbars to a position you prefer if needed.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 20

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Create the constraint on the end of the arm.  Rotate your view by clicking and holding the Left Mouse Button while dragging your cursor in the graphics window. Your view orientation should be similar to the view below so that you can clearly see the top of the boss on the right end of the arm and the holes on the left end of the arm.

 Click the Create Constraint on Surface icon on the

Constraints toolbar.

 Since there is no active Constraint Set, you are prompted to either create a constraint set or activate an existing set. In the New Constraint Set dialog box, enter Arm Hole Constraints as the Title. Click OK to create the constraint set. CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 21

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Entity Selection – Select SURFACE(s) to Select dialog box, select the two surfaces on the inside of the holes at the end of the arm as shown below. As you move the cursor, you will see different surfaces highlighted. The default method of selecting surfaces in Femap is to find the surface with the closest center of gravity to the cursor.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 22

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 Click the Preview icon

in the Entity Selection dialog

box to highlight the surfaces you selected.

 Click OK to confirm your selection.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 23

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

In the Create Constraints on Geometry dialog box, enter Fixed Mount as the Title.  Select Fixed as the constraint type. Click OK to create the constraint.

 Click Cancel or press the Esc key to exit the command.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 24

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Highlight the newly created constraint.  In the Model Info pane, expand the Constraints, Arm Hole Constraints constraint set and the Constraint Definitions object.  Select the Fixed Mount Holes constraint to highlight the geometry it is applied to.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 25

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Create the load on the boss at the end of the arm.  Since you do not have a Load Set, you will need to create one. In the Model Info pane, right-click the Loads object and select New from the context-sensitive menu.

 In the New Load Set dialog box, enter Arm Boss Load as the title. Click OK to create and activate the new load set.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 26

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 Expand the newly created Arm Boss Load load set. Rightclick Load Definitions and select On Surface from the menu. This is equivalent to selecting the command, Model, Load, -

> On Surface or by selecting the Create Load on Surface icon on the Loads toolbar.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 27

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 Select the surface on the bottom of the boss on the right side of the arm. Again, use the Preview button in the Entity

Selection dialog box to confirm your selection.

 Click OK to complete the selection of the surface(s) you are applying the force to.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 28

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 In the Create Loads on Surface dialog box, set the Title to Boss Normal Load, select Force as the Load Type and set the Direction to Normal to Surface.

Set the Load Magnitude to -500.  Click OK to apply the load to the control arm.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 29

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Turn off display of points, surfaces and nodes.  Activate and position the Entity Display toolbar by one of the methods used in the beginning of this exercise (right-click on a blank area adjacent to one of the other docked toolbars or by using the Tools -> Toolbars command).  In the Entity Display toolbar, click the View Points Toggle, View Surfaces Toggle, and the View Nodes Toggle.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 30

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Step 5: Mesh the lower control arm. Mesh the lower control arm.  Right-click the Lower Control Arm solid under the Geometry tree in the Model Info pane and select Tet Mesh from the menu.

 In the Automesh Solids dialog box, click the Update Mesh Sizing button.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 31

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Automatic Mesh Sizing dialog box, enter or set the following options:  Set the value for Element Size to 5.0.  Set the value for Max Angle Tolerance to 15.  Disable the option for Max Elem on Small Feature by clicking the check box for this option. This will automatically disable the option for Max Size of Small

Feature.  Disable the option for Suppress Short Edges.

 Leave all other options unchanged and click OK to apply the mesh sizing to the lower control arm.  Click OK in the Automesh Solids dialog box to mesh the lower control arm.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 32

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Your model should appear similar to the model below.

Turn off display of the Mesh Size indicators. After any operation that sets a mesh size (other than the default mesh size), Mesh Size indicators are displayed on the model as a view default.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 33

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 To toggle off the display of the mesh size indicators, select the View Style, Mesh Size icon on the View toolbar.

 Save your model.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 34

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Step 6: Analyze the Lower Control Arm Create an Analysis Set for a linear static analysis.  In the Model Info pane, right-click the Analyses object and select Manage from the menu.

 In the Analysis Set Manager dialog box, click the New button to create a new Analysis Set.  In the Analysis Set dialog box, enter the Title as Linear Statics. Click OK to create the analysis set.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 35

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 Returning to the Analysis Set Manager dialog box, expand the Master Requests and Conditions tree along with the Boundary Conditions and Output Displacements sub trees. Note how the Boundary Conditions are automatically set to the active constraint and load sets.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 36

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Run the analysis.  Click the Analyze button in the Analysis Set Manager dialog box. Once an NX Nastran analysis is started, Femap will automatically open the Analysis Monitor pane as shown below (in an undocked and resized mode). This window displays the NX Nastran .log file as it is being updated during the analysis. You have the option to change the display of the status from the default .log file to either the .f04 or the .f06 file. You can also change the Max Lines to display (the Femap default preference is 5000 lines), to turn off Update Monitor and to turn off the option to

Automatically Load Results.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 37

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Once an analysis has successfully completed, the Femap

Messages pane should display the following lines: Today’s Date NX NASTRAN Version Date PAGE

2

Reading... Creating Output Set 1... Beginning Cleanup of Output Set 1... Cleanup of Output Set 1 is Complete.  Close the Analysis Monitor pane.  Save your Femap model.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 38

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Step 7: Post Process (review) the Results of the Analysis. Select the Output Set, Deformation Vector, and Contour Vector for Postprocessing.  Right-click your mouse in the graphics window and select Post Data from the context-sensitive menu.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 39

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 In the Select Postprocessing Data dialog box, note that the following have been automatically set: The Output Set is set to 1..NX NASTRAN Case 1. The Output Vector for Deformation is set to 1..Total Translation. And the Output Vector for Contour is set to 60031..Solid Von Mises Stress.

 Click OK to apply your selections.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 40

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

If the PostProcessing Toolbox pane is not open, open it using by clicking the PostProcessing icon on the Panes toolbar.

Note: When an icon is shown as “filled” like the first four and the last icon on the toolbar as show above, this indicates that the option is enabled, or in this case, the pane associated with the icon is open. By default, when you first open the PostProcessing Toolbox pane, it will be docked and tabbed along with the Model Info and Meshing Toolbox panes as shown below.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 41

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 Click on the PostProcessing tab to bring the toolbox to the front.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 42

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Turn on display of the stress contours and the deformed shape using the PostProcessing Toolbox.  On the PostProcessing Toolbox’s toolbar, click the Deformed drop-down icon and select Deform.

Your model should appear as below.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 43

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Display the Von Mises Stress contours. 

On the PostProcessing Toolbox’s toolbar, click the Contour drop-down icon and select Contour.

Your model should be similar to the one below.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 44

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Change the deformed shape to display the actual deformation at ten (10) times the real deformation. Femap’s default view displays the maximum deformation scaled to ten percent (10%) of the view extents. In this step, you will change that to display the deformation as a scale factor of the actual deformation.  Expand the Deform tool.  Expand the Scale tool and select Actual Deformations from the Scale drop-down.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 45

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

 Double-click Scale Actual By and set the value to 100.0. Use either the Tab or Enter key to update the display of the deformed shape.

Toggle the display of constraints and loads  On the Entity Display toolbar, click the View Constraints Toggle and the View Loads Toggle icons.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 46

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

Turn off the display of results.  On the PostProcessing Toolbox’s toolbar, click the icon for Set to Undeformed, No Contour, No Freebody.

 Collapse the Deform tool and expand the Contour tool.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 47

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Review stress results inside the model using a moving cut plane.  On the Postprocessing Toolbar’s toolbar, click the Set the Contour Style pull-down and select Section Cut from the menu.

 In the PostProcessing Toolbox, click the Dynamic Control arrow button.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 48

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 Using the scroll bar in the Dynamic Section Cut Control dialog box, move the cutting plane to show different locations in the model.

You can also directly input the offset of the plane from its origin in the Value field and the incremental offset of the cutting plane in the Delta field in the Dynamic Section Cut

Control dialog box.

The Plane button in this dialog box allows you to modify the orientation and origin of the cutting plane.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 49

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 - Analyzing a Solid Part

Display locations in the model of a specific stress value using

Isosurfaces.  On the Postprocessing Toolbar’s toolbar, click the Set the Contour Style pull-down and select IsoSurface from the menu.

Your model will appear similar to below.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 50

© Siemens AG 2013 All rights reserved.

Siemens PLM Software

Exercise 1 – Analyzing a Solid Part

 Click the Dynamic Control arrow button under the Contour tool. You should only see one value of stress displayed throughout the model. The initial value will be the average of the minimum and maximum values of the contour vector.

Note that you can directly enter a Value and the Delta value.  Click OK to close the dialog box and return to the previous view display of the isosurfaces. Save your model and close Femap.  Save your model and Exit Femap.

CT2060

Femap 101 for Femap v11 – Student Workbook – Rev A 1 - 51

© Siemens AG 2013 All rights reserved.

Siemens PLM Software