OS-HM-T: 10010 Design Concept for a Structural Clip

Tutorial Level: Intermediate In this tutorial, a topology optimization on a model is performed to create a new topology for the structure, removing any unnecessary material. The resulting structure is lighter and satisfies all design constraints.

The topology optimization technique yields a new design and optimal material distribution. Topology optimization allows designers to start with a design that already has the advantage of optimal material distribution and is ready for fine tuning with shape or size optimization.

Before you begin, copy the file(s) used in this tutorial to your working directory.
The optimization problem for this tutorial is stated as:
Objective
Minimize volume fraction.
Constraints
Translation in the y-axis for node A < 0.07 mm.
Translation in the y-axis at node B > -0.07 mm.
Design Variables
The density of each element in the design space.
The following exercises are included:
  • Set up the model in HyperMesh.
  • Analyze the baseline model.
  • Set up the optimization.
  • Post-process size optimization results.

Launch HyperMesh

  1. Launch HyperMesh.
  2. In the New Session window, select HyperMesh from the list of tools.
  3. For Profile, select OptiStruct.
  4. Click Create Session.
    Figure 1. Create New Session


    This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

Open the Model File

  1. On the menu bar, select File > Open > HyperMesh Model.
  2. Navigate to and select the cclip.hm file saved in your working directory.
  3. Click Open.
    The cclip.hm database is loaded into the current HyperMesh session, replacing any existing data.
    Figure 2. Model Import Options


    Tip: Alternatively, you can drag and drop the file onto the viewport from the file browser window.

Set Up the Model

Create Materials and Properties for the Components

Properties and materials can be created from within the Component editor.

  1. In the Model Browser, double-click on Components.
    Tip: Alternatively, you can right-click on Components and click Open.
  2. Select the component comp_shell.
  3. In the Entity Editor, right click on Property and select Create.
    This creates and assigns the property to the selected Component.
  4. In the embedded Entity Editor, for Name, enter prop_shell.
  5. For Card Image, select PSHELL.
  6. Click the T (thickness) field and accept the default value of 1.0 by pressing Enter.
  7. Right-click on Material and select Create.
    This creates and assigns the material to the selected component/property.
  8. For Name, enter Steel.
  9. For Card Image, select MAT1.
  10. Click the E field and accept the default value of 2.1E5 by pressing Enter.
  11. Similarly, click the Nu field and accept the default value of 0.3.
  12. For RHO, enter 7.9E-9.
  13. Click Close.
  14. Close the Entity Editor.

Create Load Collectors

Next, create two load collectors (Constraints and Forces) and assign each a color.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter Forces.
  3. Click Color and select a color from the color palette.
  4. Click Close.
  5. Using the same method, create a second load collector named Constraints.
    The Constraints load collector is set as Current as it was created last. The SPCs created next are set into the Constraints load collector.

Create Constraints

For the three nodes that show constraints in Figure 3, you need to create the SPC constraints and assign them to the Constraints load collector.
Figure 3. Nodes Showing Constraints


  1. From the Analyze ribbon, click Constraints.
    Figure 4. Constraints Tool


  2. Orient the model to the TOP view.
  3. Select the upper left node and click .
  4. Deselect all DOF check boxes except for DOF3.
  5. For DOF3, accept the default value of 0.
    Figure 5. DOF3 Active on Upper Left Node


    Tip: To deselect a node, hold Shift and left-click on it, or left-click + drag a box around it.
  6. For Enties, click Nodes to select another node.
  7. Select the node at the halfway point on the left edge of the part and click .
    Figure 6. Left Middle Node Selection for DOFs 1, 2, 3


  8. Select the DOF1, DOF2, and DOF3 check boxes.
  9. Accept all default values of 0.
  10. Click Create.
  11. Repeat from step 6 to select the node at the left of the slot radius.
    Figure 7. Middle Node on Radius Selection for DOF 2


  12. Select the DOF2 check box and accept the default value of 0.
  13. Click Create.
  14. Click Close.
    Tip: To increase the size of the spc markers: click File > Preferences. Under HyperMesh, click Appearance. For Boundary conditions, increase the Size value.

    To see the DOF labels, activate Labels for Boundary Conditions and Show load handle for Loads.

    Figure 8. Boundary Conditions Applied to C-clip


Create Forces

In this step, load the structure with two opposing forces of 100.0 N at the opposite tips of the opening of the c-clip.

  1. In the Model Browser, double-click on Load Collectors.
    Tip: Alternatively, you can right-click on Load Collectors and click Open.
  2. Right-click Forces and select Make Current.
  3. On the Analyze ribbon, Loads tool group, select Forces.
    Figure 9. Forces Tool


  4. Orient the model to the TOP view.
  5. Select the node at the right end, top edge of the slot (location A in Figure 10).
  6. Click .
  7. For Magnitude, enter 100.0.
  8. For Direction, enter X = 0, Y = 1, and Z = 0.
  9. Click Create.
    An arrow pointing upward appears at the selected node.
  10. Click Nodes to select another node.
  11. Select the node on the right end, bottom edge of the slot (location B in Figure 10).
  12. Click .
  13. For Magnitude, enter -100.0.
  14. For Direction, verify the values are X = 0, Y = 1, and Z = 0.
  15. Click Create.
    An arrow pointing downward appears at the selected node.
  16. Click Close.
    Tip: To increase the size of the load arrows: click File > Preferences. Under HyperMesh, click Appearance. For Loads, increase the Uniform value.
    Figure 10. Opposing Forces Created at Opening of C-clip


Create Load Cases

The last step in establishing boundary conditions is the creation of a load step.

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter opposing forces.
  3. For Analysis type, select Linear Static.
  4. For SPC, click Unspecified and select the search tool.
  5. Select Constraints from the list.
  6. Similarly, for LOAD, select Forces.
    Figure 11. Load Step Defined


  7. Click Close.

Analyze the Baseline Model

Run the Analysis

A linear static analysis of this C-clip is performed prior to the definition of the optimization process. An analysis identifies the responses of the structure before optimization to ensure that constraints defined for the optimization are reasonable.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    Figure 12. Select Run OptiStruct Solver


  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter cclip.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. For export options, toggle all.
  6. Click Export.
    The Compute Console opens with cclip.fem as the Input File.
    Figure 13. Altair Compute Console


  7. Click Run.
    Upon successful completion of the analysis, the message ANALYSIS COMPLETED appears in the Message log window.

View Displacement Contour

  1. From the Compute Console, click Results to launch the cclip.mvwresults file in HyperView.
    Figure 14. Launch Results


  2. From the Results ribbon, click Contour.
    Figure 15.


  3. For Results type, select Displacement.
  4. For the menu below Displacement, select Y.
  5. Click Apply.
    Figure 16. Contour of Y Displacements


  6. Verify the values are equivalent to Figure 16.
  7. From the menu bar, select File > Exit to close HyperView.
  8. In the Save Session? dialog, click No.
  9. In the Compute Console Solver View window, click Close.
  10. In the Compute Console, click Close.

Set Up the Optimization

The finite element model, consisting of shell elements, element properties, material properties, and loads and boundary conditions has been defined. Now a topology optimization is performed with the goal of minimizing the amount of material used. Typically, removing the material in an existing volume with the same loads and boundary conditions makes the model less stiff and more prone to deformation. Therefore, you need to track the displacements (which represent the stiffness of the structure) and constrain the optimization process such that the least material necessary is used and overall stiffness is also achieved.

The forces in the structure are applied on the outer nodes of the opening of the clip, making those two nodes critical locations in the mesh where the maximum displacement is likely to occur. In this tutorial, a displacement constraint is applied on the nodes so that they do not displace more than 0.07 in the y-axis.

Create the Topology Design Variables

  1. In HyperMesh, open the Optimize ribbon.
  2. Click Topology.
    Figure 17. Topology Tool


  3. For Property Type, select PSHELL.
  4. For List of Properties, click 0 Properties > to open Advanced Selection.
    Figure 18. List of Properties


  5. Change the selection type to By List and select prop_shell.
    Figure 19. Select By List


  6. Click OK.
  7. Click Close.

Create a Volume Response

  1. On the Optimize ribbon, click Responses.
    Figure 20. Responses Tool


  2. For Name, enter volfrac.
  3. For Response Type, select volumefrac.
  4. Click Close.

Create a Displacement Response

To create a displacement as a response, supply a name for the response, set the response type to displacement, select the node for the response, and select the type of displacement (DOF).

  1. On the Optimize ribbon, click Responses.
  2. For Name, enter upper-disp.
  3. For Response Type, select static displacement.
  4. For List of Nodes, click 0 Nodes.
  5. Select the node at the upper opening of the c-clip (labeled A in Figure 21).
    Figure 21. Upper Opening of C-clip


  6. Click .
  7. From the drop-down menu, select dof2.
  8. Click Close.
  9. On the Optimize ribbon, click Responses.
  10. For Name, enter lower-disp.
  11. For Response Type, select static displacement.
  12. For List of Nodes, click 0 Nodes.
  13. Select the node at the lower opening of the c-clip (labeled B in Figure 22).
    Figure 22. Lower Opening of C-clip
  14. From the drop-down menu, select dof2.
    Figure 23. Optimization Response


  15. Click Close.

Create Constraints on Displacement Responses

In this step, the upper and lower bound constraint criteria for this analysis are set.

  1. On the Optimize ribbon, click Constraints.
    Figure 24. Constraints Tool


  2. For Name, enter c_upper.
  3. For Response, click Unspecified and select the search tool.
  4. Select upper-disp from the list.
  5. For List of Loadsteps, click 0 Loadsteps > to open Advanced Selection.
  6. Select opposing forces from the list.
  7. Click OK.
    Figure 25. Select opposing forces Loadstep


  8. For Upper Options, select Upper bound.
  9. For Upper Bound, enter 0.07.
    Figure 26. Optimization Constraint c_upper


  10. Click Close.
  11. On the Optimize ribbon, click Constraints.
  12. For name, enter c_lower.
  13. For Response, click Unspecified and select the search tool.
  14. Select lower-disp from the list.
  15. For List of Loadsteps, click 0 Loadsteps > to open Advanced Selection.
  16. Select opposing forces from the list.
  17. Click OK.
  18. For Lower Options, select Lower bound.
  19. For Lower Bound, enter -0.07.
    Figure 27. Optimization Constraint c-lower


  20. Click Close.

Define the Objective Function

  1. On the Optimize ribbon, select Objectives.
    Figure 28. Objectives Tool


  2. Verify that Objective Type is set to Minimize.
  3. For Response Id, click Unspecified and select the search tool.
  4. Select volfrac.
    Figure 29. Objective Definition


  5. Click Close.

Run the Optimization

  1. From the Optimize tool, click Run.
    Figure 30. Run Optimization


  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter cclip_complete.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. For Export, select All.
  6. Click Export.
  7. In the Altair Compute Console, click Run.
    If the job is successful, the following message appears in the window: 
    OPTIMIZATION HAS CONVERGED.
FEASIBLE DESIGN (ALL CONSTRAINTS SATISFIED).
    New results files are seen in the directory where the model file was written. The cclip_complete.out file is a good place to look for error messages that could help debug the input deck if any errors are present.
    The following default files are written to your run directory:
    cclip_complete_des.h3d
    HyperView binary results file containing the iso surface.
    cclip_complete_s1.h3d
    HyperView binary results file containing the displacement and stress results.
    cclip_complete.mvw
    Contains the design results and the displacement and stress results from the *_des.h3d and *_s1.h3d files.
    cclip_complete_hist.mvw
    Contains the iteration history of the objective, constraints, and the design variables. It can be used to plot curves in HyperGraph, HyperView, and MotionView.
    cclip_complete.out
    OptiStruct output file containing specific information on the file setup, the setup of the optimization problem, estimates for the amount of RAM and disk space required for the run, information for all optimization iterations, and compute time information. Review this file for warnings and errors that are flagged from processing the cclip_complete.fem file.
    cclip_complete.sh
    Shape file for the final iteration. It contains the material density, void size parameters, and void orientation angle for each element in the analysis. This file can be used to restart a run.
    cclip_complete.hgdata
    HyperGraph file containing data for the objective function, percent constraint violations, and constraint for each iteration.
    cclip_complete.oss
    OSSmooth file with a default density threshold of 0.3. You can edit the parameters in the file to obtain the desired results.
    cclip_complete.stat
    Contains information about the CPU time used for the complete run and also the break-up of the CPU time for reading the input deck, assembly, analysis, convergence, and so on.

Post-process the Results

OptiStruct provides element density information for all iterations, and also gives displacement and Von Mises stress results (linear static analysis) for the starting and last iterations. This section describes how to view those results in HyperView.

View an Iso Value Plot of Element Densities

  1. From the Compute Console Solver View, click Results.
    Figure 31. View Results


    The cclip_complete.mvw file launches in HyperView. This file contains two pages of results:
    • Page 1 - cclip_complete_des.h3d: Optimization history results (element density).
    • Page 2 - cclip_complete_s1.h3d: Subcase 1 results; initial and final (displacement stress).
  2. On the Results ribbon, click Iso.
    Figure 32. Iso Tool


  3. In the Results tab, select the last iteration from the drop-down menu.
    Figure 33. Select Last Iteration


  4. Click Apply.
  5. Orient the model to TOP view.
    Tip: If the color of the iso surface is difficult to see, go to the Results tab, expand Components, and click on the color indicator to select a different color from the pallet.
  6. For Current Value, enter 0.3.
    Figure 34. Iso Value Slider with Setting 0.3


    Figure 35. Results


  7. To change the density threshold, adjust the Current Value slider.
    The iso value updates interactively when you scroll to a new value. Use this tool to get a better look at the material layout and the load paths from OptiStruct.

Compare Static Contours

In this step, compare the static contour of the original design to the optimized material layout.

  1. Expand the page selection dialog.
    This is located at the top right of the window, near the search tool.
    Figure 36. Expand Page Selection


  2. Select Subcase 1 – opposing forces.
    Figure 37. Select Subcase 1


    Note: If the other pages are not available:
    • Click File > Import > Model.
    • Verify the file selected is cclip_complete_des.h3d.
    • Click Apply
    • Click Yes.
    Other options should now be available in the page selection dialog.
  3. Use the Page Layout icon to divide the page into two vertical windows.
    Figure 38. Page Layout


  4. Orient the model to TOP view.
  5. On the Results ribbon, click Contour.
    Figure 39. Contour Tool


  6. For Results type, select Displacement.
  7. For the menu below Displacement, select Y.
  8. Click Apply.
  9. On the Results ribbon, click Deformation.
    Figure 40. Deformation Tool
  10. Under Deformed shape, for Value, enter 100.
  11. Under Undeformed shape, for Show, select Edges.
    Figure 41. Results Display Settings


  12. Click Apply.
  13. On the Results ribbon, click Contour.
  14. Right-click in the modeling window with the model and select Active Model > Copy.
    Figure 42. Copy Active Model


  15. Right-click in the empty modeling window and select Active Model > Paste.
  16. In the second window, select Iteration 28.
    Figure 43. Compare Contour Plots
  17. In the Session Browser, right click on Subcase 1 - opposing forces 2 and select Copy.
    Tip: If you do not see the Session Browser, on the menu bar, click View and activate Session Browser.
  18. Right-click in the Session Browser and select Paste.
  19. Expand the page selection dialog and select the newly available third page.
    Figure 44. Page Selection


  20. On the new page, click in the left window.
  21. For Results type, select Element Stresses (2D & 3D) (t).
  22. For Averaging method, select Simple.
  23. Click Apply.
  24. Right-click on the left window and select Apply Style > Current Page > Contour.
    The right window now also displays a stress contour.
    Figure 45. Element Stress Results at Iteration 0 and Iteration 28


    These stress results can be used only as reference to help understand how far the design is from the limits.

    Topologic optimization shows a concept shape and the stress results should be validated during the next design phases.