Normal Modes Analysis of a Splash Shield - OS-1020

In this tutorial, an existing finite element model of an automotive splash shield will be used to demonstrate how to set up and perform a normal modes analysis. HyperMesh post-processing tools are used to determine mode shapes of the model.

The following exercises are included:

·   Retrieving the OptiStruct input file

·   Setting up the problem in HyperMesh

·   Submitting the job

·    Viewing the results

The following file is needed to perform this tutorial:

sshield.fem         Original ASCII OptiStruct input deck.

This file can be copied to your working directory from <install_directory>/tutorials/os.

Retrieving the OptiStruct Input File

To retrieve an existing FE (OptiStruct) model:

1. Launch HyperMesh.

2. Choose OptiStruct as the User Profile and click OK.

User Profiles… can also be accessed from the Preferences pull-down menu.

This loads the OptiStruct user profile. It includes the OptiStruct template, macro menu, and import reader. It simplifies the menu systems to give access to only the functionality of HyperMesh that is necessary for using OptiStruct.

3. From File pull-down menu select Import, and then Finite Element Model and click on OptiStruct… (as shown below).

The OptiStruct input translator allows model information stored in an OptiStruct input file (normally denoted with the .fem extension) to be retrieved.

An Open file… browser window pops up.

4. Select the sshield.fem file, located in the HyperWorks installation directory <install_directory>/tutorials/os/.

5. Click Open.

The sshield.fem OptiStruct input file is loaded into the current HyperMesh session.

Note the location of sshield.fem displays in the file: field.

6. Click Return.

Setting Up the Problem in HyperMesh

To review rigid elements:

Notice there are two rigid "spiders" in the model. They are placed at locations where the shield is bolted down. This is a simplified representation of the interaction between the bolts and the shield. It is assumed that the bolts are significantly more rigid in comparison to the shield.

The dependent nodes of the rigid elements have all six degrees of freedom constrained. Therefore, each "spider" connects nodes of the shell mesh together in such a way that they do not move with respect to one another.

The following steps show how to review the properties of the rigid elements.

1. From the 1D page, select the rigids.

2. Click review.

3. Select one of the rigid elements in the graphics region.

In the graphics window, HyperMesh displays the IDs of the rigid element and the two end nodes and indicates the independent node with an 'I' and the dependent node with a 'D'. HyperMesh also indicates the constrained degrees of freedom for the selected element, through the dof checkboxes in the rigids panel. All rigid elements in this model should have all dofs constrained.

4. Click return to go to the main menu.

To set up the material and geometric properties:

The imported model has three component collectors with no materials. A material collector needs to be created and assigned to the shell component collectors. The rigid elements do not need to be assigned a material. Shell thickness values also need to be corrected.

1. Select the Collectors toolbar button .

2. Select the create subpanel using the radio buttons on the left-hand side of the panel.

3. Click the collector type switch and select materials from the pop-up menu.

4. Click name = and enter steel.

5. Click card image = and select MAT1 from the pop-up menu.

6. Click create/edit.

The MAT1 card image pops up.

7. For E, enter the value 2.0E5.

8. For NU, enter the value 0.3.

9. For RHO, enter the value 7.85E-9.

If a quantity in brackets does not have a value below it, it is off. To change this, click the quantity in brackets and an entry field will appear below it. Click in the entry field, and a value can be entered.

10. Click return.

A new material, steel, has now been created. The material uses OptiStruct's linear isotropic material model, MAT1. This material has a Young's Modulus of 2E+05, a Poisson's Ratio of 0.3 and a material density of 7.85E-09. A material density is required for the normal modes solution sequence.

At any time, the card image for this collector can be modified using Card Editor.

11. Click return to exit the Collectors panel.

12. Select the Card Editor toolbar button .

13. Click the toggle under Card Editor to choose comps from the pop-up menu.

14. Click the yellow comps button and then check the box next to design.

15. Click select.

16. Make sure card image= is set to PSHELL.

17. Click edit.

The PSHELL card image for the design component collector pops up.

18. Replace 0.300 in the T field with 0.25.

19. Click return.

20. Click the reset button to refresh the selection.

21. Click the yellow comps button and select the box next to nondesign.

22. Make sure card image= is set to PSHELL.

23. Click edit.

The PSHELL card image for the nondesign component collector pops up.

24. Replace 0.300 in the T field with 0.25.

25. Click return to save the changes to the card image.

26. Click return to go to the main menu.

27. Select the Collectors toolbar button .

28. Select the update subpanel using the radio buttons on the left side of the panel.

29. Click the collector type switch and select comps from the pop-up menu.

30. Click the yellow comps button and then check the box next to design.

31. Click material= and select steel from the pop-up menu.

32. Click update and the material steel is assigned to the design component.

33. Follow this procedure (steps 28 to 32) to update the component nondesign with the new material steel.

Applying Loads and Boundary Conditions to the Model

The model is to be constrained using SPCs at the bolt locations, as shown in the following figure. The constraints will be organized into the load collector, 'constraints'.

Selecting nodes for constraining the bolt locations (zoomed in from a top view).

To perform a normal modes analysis, a real eigenvalue extraction (EIGRL) card needs to be referenced in the subcase. The real eigenvalue extraction card is defined in HyperMesh as a load collector with an EIGRL card image. This load collector should not contain any other loads.

To create load collectors:

1. Select the Collectors toolbar button .

2. Select the create subpanel using the radio buttons on the left-hand side of the panel.

3. Click the collector type switch and select load collectors from the pop-up menu.

4. Click name = and enter constraints.

5. Click color and select and color from the palette.

6. Click the switch beside card image= and select no card image from the pop-up menu.

7. Click create.

A new load collector, constraints, is created.

8. Click name = and enter frequencies.

9. Click the switch beside card image= and select card image from the pop-up menu.

10. Click card image = and select EIGRL from the pop-up menu.

11. Click color and select and color from the palette.

12. Click create/edit.

The EIGRL card image pops up.

13. For V2, enter the value 200.000.

14. For ND, enter the value 6.

If a quantity in brackets does not have a value below it, it is off. To change this, click on the quantity in brackets and an entry field will appear below it. Click on the entry field, and a value can be entered.

15. Click return to save changes to the card image.

A real Eigenvalue extraction card has been created. The first 6 roots between 0 and 200Hz are to be extracted.

16. Click return twice to return to the main menu.

To create constraints at the bolt locations:

1. Press G on the keyboard to enter the Global panel.

2. Confirm that the page toggle is set to pg1.

3. Click on loadcol=.

4. Select constraints from the list of load collectors.

5. Click return to exit the Global panel and return to the main menu.

6. From the Analysis page, select the constraints panel.

7. Select the create subpanel using the radio buttons on the left-hand side of the panel.

8. Click the entity selection switch and select nodes from the pop-up menu.

9. Select the two nodes, shown in the figure above, at the center of the rigid spiders, by clicking on them in the graphics window.

10. Constrain all dofs.

Dofs with a check will be constrained while dofs without a check will be free.

Dofs 1, 2, and 3 are x, y, and z translation degrees of freedom

Dofs 4, 5, and 6 are x, y, and z rotational degrees of freedom.

11. Click create.

Two constraints are created. Constraint symbols (triangles) appear in the graphics window at the selected nodes. The number 123456 is written beside the constraint symbol, indicating that all dofs are constrained.

12. Click return to go to the main menu.

To create an OptiStruct subcase (also referred to as a loadstep):

1. From the Analysis page, select the subcase panel.

2. Click the type: switch and choose normal modes from the pop-up menu.

3. Click name = and enter bolted.

4. Check the box preceding SPC.

An entry field appears to the right of SPC.

5. Click on the entry field and select constraints from the list of load collectors.

6. Check the box preceding METHOD.

An entry field appears to the right of METHOD.

7. Click on the entry field and select frequencies from the list of load collectors.

8. Click create.

An OptiStruct subcase has been created which references the constraints in the load collector constraints and the real eigenvalue extraction data in the load collector frequencies.

9. Click return to go to the main menu.

Submitting the Job

To launch OptiStruct:

1. From the Analysis page, select the OptiStruct panel.

2. Click save as… following the input file: field.

3. A Save file… browser window pops up.

4. Select the directory where you would like to write the OptiStruct model file and enter the name for the model, sshield_complete.fem, in the File name: field. .fem is the suggested extension for OptiStruct input decks.

5. Click Save.

Note that the name and location of the sshield_complete.fem file is now displayed in the input file: field.

6. Set the memory options: toggle to memory default.

7. Click the run options: switch and select analysis.

8. Set the export options: toggle to all.

9. Click OptiStruct.

This launches the OptiStruct job. If the job is successful, new results files can be seen in the directory where the OptiStruct model file was written. The sshield_complete.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

The default files written to your directory are:

Viewing the Results

Eigenvector results are output, by default, from OptiStruct for a normal modes analysis. This section describes how to view the results in HyperView.

To load the model and result files into the animation window:

In this section, you will load a HyperMesh .h3d file into the HyperView animation window.

1. Click the HyperView button in the OptiStruct panel.

HyperView is launched and the sshield_complete.h3d file is loaded.

2. Click Close to exit the Message Log menu that appears.

To view the deformed structure:

It is helpful to view the deformed shape of a model to determine if the boundary conditions have been defined correctly and also to check if the model is deforming as expected. In this section, use the Deformed panel to review the deformed shape for last Mode.

1. From the Graphics pull-down menu, choose Select Load Case to activate the Load Case and Simulation Selection dialog as shown below.

2. Select Mode 6-F=1.4942E+02 from the list and click OK.

3. Click on the switch next to the traffic light signal and choose Modal .

4. Select the Deformed toolbar button .

5. Leave Result type set to Animation(v).

6. Set Scale: to Model Units.

7. Set Type: to Uniform: and type in a scale factor of 25 for Value.

This means that the maximum displacement will be 25 modal units and all other displacements will be proportional.

Using a scale factor higher than 1.0 amplifies the deformations while a scale factor smaller than 1.0 would reduce them. In this case, we are accentuating displacements in all directions.

8. Set Show under Undeformed shape to Wireframe.

9. Click Apply.

A deformed plot of the model overlaid on the original undeformed mesh is displayed in the graphics window.

Does the deformed shape look correct for the boundary conditions you applied to the mesh?

10. To animate the mode shape, click the animation mode: modal .

11. To control the animation speed, use the Animation Controls accessed with the director’s chair toolbar button .

12. View the rest of your mode shapes using the same model units.

Does the shape of mode #5 match the shape shown in the second figure?

Mode shape of 5th root.

Analysis Review

Review the following points:

Representation of the boundary conditions at the bolt locations:

In this analysis, it was assumed that the bolts were significantly stiffer than the shield. If the bolts needed to be made of aluminum and the shield was still made of steel, would the model need to be modified, and the analysis run again?

It is necessary to push the natural frequencies of the splash shield above 50Hz. With the current model, there should be one mode that violates this constraint: Mode 1. Design specifications allow the inner disjointed circular rib to be modified such that no significant mass is added to the part. The available package space for this new rib is shown as the solid region in the figure below. The thickness of the solid region is equal to the depth of the original rib. Is there a better configuration for this rib within the above stated constraints that will push the first mode above 50Hz? See tutorial OS-2020 to redesign this part.

Green solid region represents the available package space for redesigning the inner disjointed circular rib.

Go To

OptiStruct Tutorials