OS-HM-T: 1010 Linear Static Analysis with Thermal Loading of a Coffee Pot Lid

In this tutorial, an existing finite element model of a plastic coffee pot lid is used to demonstrate how to apply thermal loading and perform an OptiStruct linear static analysis.

Before you begin, copy the file(s) used in this tutorial to your working directory.

HyperView post-processing tools are used to determine deformation and stress characteristics of the lid.

The following exercises are included:
  • Retrieve the HyperMesh database file.
  • Set up the problem in HyperMesh.
  • Apply loads to the model.
  • Submit the job.
  • View the results in HyperView.

Launch HyperWorks

  1. Launch Altair HyperWorks.
  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 coffee_lid.hm file saved in your working directory.
  3. Click Open.
    The coffee_lid.hm database is loaded into the current HyperMesh session, replacing any existing data. The database only contains geometric data.
    Figure 2. Model Import Options

Set Up the Model

Create the Material

The imported model has two component collectors with no materials. A material collector needs to be created and assigned to the component collectors.

  1. In the Model Browser, right-click and select Create > Material.
    A default MAT1 material template displays in the Entity Editor.
  2. For Name, enter plastic.
  3. Enter the following material values in the dialog:
    1. [E] Young’s modulus = 1137
    2. [NU] Poisson’s ratio = 0.26
    3. [A] Coefficient of linear thermal expansion = 8.1e-05
    The material uses the OptiStruct linear isotropic material model, MAT1. If a material property does not display a value next to it, it is turned off. It is not necessary to define a density value since only a static analysis is performed. Density values may be required for other solution sequences.
    Figure 3. Material Property Values for plastic

Edit the Properties and Update the Component Collector

  1. In the Model Browser, expand the Property folder and click on PSHELL.
    The PSHELL property entry is displayed in the Entity Editor.
  2. Verify the thickness value, T, is set to 2.5.
  3. Notice the value field for Material is set to <Unspecified>.
    This indicates that no material properties are being referenced by this property.
  4. For Material, select Unspecified > Material.
    Figure 4. Select the Material plastic for the Property PSHELL

  5. In the Select Material dialog, select plastic and click OK.
    The material, plastic, is now assigned to the property PSHELL.
    Figure 5. PSHELL Property Entry Fields in Entity Editor

  6. Repeat steps 1 through 5 to assign the plastic property to PSHELL1.

Apply Loads to the Model

Constraints have already been applied to the model. In the following steps, thermal loading is applied.

Create a Load Collector

  1. In the Model Browser, right-click and select Create > Load Collector.
    A default load collector template displays in the Entity Editor.
  2. For Name, enter temp_initial.
  3. For Card Image, select TEMPD.
  4. For Default Temperature Value (T1), enter 70.
  5. Click Close.
    Figure 6. Create temp_initial Load Collector

  6. Similarly, create another load collector with the name thermal_loading.
  7. For Card Image, use TEMPD.
  8. For Default Temperature Value (T1), enter 70.
  9. Click Close.
    Figure 7. Create thermal_loading Load Collector

Create a Temperature Load

  1. From the Analyze ribbon, select Temperatures.
  2. For Entities, choose Nodes.
  3. From the Advanced Selection window, select both PSHELL and PSHELL1, then click OK.
  4. For Value, enter 200.
  5. Click Create and Close.
    Figure 8. Create Temperature Load

Create a Subcase

OptiStruct subcases are also referred to as load steps.

  1. In the Model Browser, right-click and select Create > Load Step.
    A default load step template displays in the Entity Editor.
  2. For Name, enter brew cycle.
  3. For Analysis type, select Linear Static.
  4. For SPC, select Unspecified > Loadcol.
    Figure 9. Select Constraints

  5. In the Select Loadcol dialog, select constraints and click OK.
  6. Select the TEMP check box.
  7. For TEMP, click Unspecified > Loadcol.
  8. In the Select Loadcol dialog, select temp_initial and click OK.
  9. Similarly, select the TEMP_LOAD and for TEMP_LOAD, select Unspecified > Loadcol.
  10. In the Select Loadcol dialog, select THERMAL_LOADING and click Close.
    Figure 10. Create brew cycle Load Step

Submit the Job

Run OptiStruct.

  1. From the Analyze ribbon, click Run OptiStruct Solver.
    Figure 11. Select Run OptiStruct Solver

    A browser window opens.
  2. Select the directory where you want to write the OptiStruct model file.
  3. For File name, enter lid_complete.
    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. For run options, toggle analysisoptimization.
  8. For memory options, toggle memory default.
  9. Click Run.
    If the job is successful, you should see new results files in the directory in which lid_complete.fem was run. The lid_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 default files written to your directory are:
    HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
    OptiStruct output file containing specific information on the file setup, the setup of your optimization problem, estimates for the amount of RAM and disk space required for the run, information for each of the optimization iterations, and compute time information. Review this file for warnings and errors.
    HyperView binary results file.
    HyperMesh binary results file.
    Summary, providing CPU information for each step during analysis process.

View Contour Plot of Stresses and Displacements

  1. Click Contour.
  2. For Results type, select Displacement (v).
  3. For Data type, select Mag.
    This represents the magnitude of the displacements.
  4. Click Apply.
    A contoured image of your model should be visible. The contours represent the displacement field resulting from the applied loads and boundary conditions.
    Figure 12. Contour Plot Showing Displacement

  5. For Results type, select Element Stresses (2D & 3D).
  6. For Data type, select von Mises.
  7. Click Apply.
    Each element in the model is assigned a legend color, indicating the von Mises stress value for that element, resulting from the applied loads and boundary conditions.
    Figure 13. Contour Plot Showing von Mises Element Stress