OS-HM-T: 16000 Phone Drop Test Analysis

Tutorial Level: Advanced This tutorial demonstrates a cellular phone drop test simulation using explicit analysis in OptiStruct.

Figure 1 illustrates the structural model used for this tutorial; the phone and its parts are considered in this model. The phone is dropped on the floor with a velocity of 5425 mm/s.
Figure 1. Model and Loading Description


Before you begin, copy the file(s) used in this tutorial to your working directory.
The following exercises are included:
  • Set up the explicit drop test model in HyperMesh.
  • Submit the OptiStruct job.
  • View the results in HyperGraph and HyperView.

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 2. 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 Drop_test_phone.hm file saved in your working directory.
  3. Click Open.
    The Drop_test_phone.hm database is loaded into the current HyperMesh session, replacing any existing data.
    Figure 3. Model Import Options


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

    The database contains meshed data, contact definitions, and control cards.

Set Up the Model

Create a Load Collector for TSTEPE

In this step, the time-step control parameters for explicit analysis is defined.

  1. In the Model Browser, right-click and select Create > Load Collector.
    If the Model Browser is not open by default, you can open it from the menu bar by clicking View > Model Browser.
  2. For Name, enter TSTEPE.
  3. Select a color from the color palette.
  4. For Card image, select TSTEPE from the drop-down menu.
  5. For Type, select ELEM.
  6. For DTFAC, enter 0.9.
    Figure 4. TSTEPE Definition


  7. Click Close.

Create a Load Collector for SPC

In this step, Single Point Constraints (SPCs) are used to fix the floor.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter SPC.
    The load collector SPC is automatically made current as it was the most recently created. If it is not, you can right click on SPC and select Make Current.
  3. Open the Analyze ribbon.
  4. Click Constraints.
    Figure 5. Constraints Tool


  5. For Entities, select Nodes.
  6. Rotate the model over to the underside of the floor and select the independent node (center node) of the RBE2 element (see Figure 6).
  7. Click .
  8. Select all DOF check boxes (1, 2, 3, 4, 5, 6) and enter a value of 0.
    This indicates all degrees of freedom are fixed.
    Figure 6. Definition of SPC on Selected Node


  9. Click Create.
  10. Click Close.

Create Load Step Inputs for NLOUT

  1. In the Model Browser, right-click and select Create > Load Step Inputs.
  2. For Name, enter NLOUT.
  3. For Config type, select Output Parameters from the drop-down menu.
    The default type is NLOUT.
  4. For Nonlinear Incremental output, select NINT from the drop-down menu.
  5. For VALUE, enter 30.
    Figure 7. NLOUT Definition


  6. Click Close.

Create a Load Collector for Initial Velocity

In this step, an initial velocity of 5425 mm/s is applied to the phone in the negative Z direction.

  1. In the Model Browser, right-click and select Create > Load Collector.
  2. For Name, enter INI_VEL.
  3. Click Close.
  4. On the Analyze ribbon, click Constraints.
    Figure 8. Constraints Tool


  5. For Load type, select TIC(V).
  6. For Entities, select Nodes > to open Advanced Selection.
    Figure 9. Open Advanced Selection


  7. For selection type, from the drop-down menu select By Set.
    Figure 10. Select Nodes by Set


  8. From the list of sets, select phone_nodes.
    Figure 11. Phone Nodes Set


  9. Click OK.
  10. Deselect all DOF check boxes except DOF3.
  11. For DOF3, enter a value -5425.
    Figure 12. Definition of Initial Velocity


  12. Click Create.
  13. Click Close.

Create an Explicit Load Step

In this step, an explicit load step is created referencing the previously defined load collectors.

  1. In the Model Browser, right-click and select Create > Load Step.
  2. For Name, enter phone_drop.
  3. For Subcase Definition, Analysis type, select Explicit.
  4. For SPC, click Unspecified > to open Advanced Selection.
  5. Select the SPC load collector and click OK.
  6. Similarly, for TSTEPE, select the TSTEPE load collector.
  7. For TTERM, enter 0.001.
  8. For NLOUT, click Unspecified > to open Advanced Selection.
  9. Select the NLOUT Load Step Input and click OK.
  10. For SUBCASE OPTIONS, select the IC check box.
  11. For IC, click Unspecified > to open Advanced Selection.
  12. Select the INI_VEL load collector and click OK.
  13. Close the Entity Editor.
    Figure 13. Explicit Load Step Definition


Create Control Cards

In this step, control cards for the simulation are defined.

  1. In the Model Browser, right-click and select Create > Cards > Output.
  2. Select the CONTF check box.
  3. For FORMAT, select H3D.
  4. For OPTION, select ALL.
    Figure 14. CONTF Settings


  5. Select the DISPLACEMENT check box.
  6. Set FORMAT = H3D and OPTION = ALL.
  7. Select the STRAIN check box.
  8. Set FORMAT = H3D and OPTION = ALL.
  9. Select the STRESS check box.
  10. Set FORMAT = H3D and OPTION = ALL.
  11. Click Close.

Submit the Job

Run OptiStruct.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    Figure 15. Select Run OptiStruct Solver


  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter Drop_test.
    The .fem filename extension is the recommended extension for Bulk Data Format input decks.
  4. Click Save.
  5. Click Export.
  6. For export options, toggle all.
  7. Click Export.
    The .fem file is exported. The Compute Console should open with the file loaded in Input file(s).
  8. In the Altair Compute Console, click Run.
    If the job is successful, an "OptiStruct Job Completed" message appears in the Compute Console Solver View Message Log. New results files are in the directory where the model file was written. The Drop_test.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

View the Work and Energy Curve Plots

In the Altair Compute Console, click Results.
Figure 16. Load Results


HyperGraph launches and loads the Drop_test _expl_energy.mvw file, plotting the curves.
Figure 17. Work and Energy Curve Plots


View a Contour Plot of Stresses and Displacement

  1. In HyperGraph, select Subcase 1 (phone drop) to expand the page creation dialog.
  2. Click to add a page.
    Figure 18. Create New Page


  3. On the menu bar, switch from HyperGraph to HyperView.
  4. Click File > Open > Model.
  5. For Load model and results, select the File icon.
    Figure 19. Open Results File in HyperView


  6. Navigate to and select the Drop_test_phone_expl.h3d file.
  7. Click Open, then Apply.
    The results file loads in HyperView.
  8. From the ribbon, click Contour.
  9. In the Results tab, select the last time increment at Time = 0.001.
  10. For Results type, select Displacement.
    Figure 20. Displacements


  11. Click Apply.
    The contour of the displacement plot is displayed at the final increment.
    Figure 21. Displacement Contour