OS-T: 1010 Thermal Stress Analysis of a Coffee Pot Lid

In this tutorial, an existing finite element model of a plastic coffee pot lid demonstrates how to apply constraints and perform an OptiStruct finite element analysis. HyperView post-processing tools are used to determine deformation and stress characteristics of the lid.

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

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Open the Model

  1. Click File > Open > Model.
  2. Select the coffee_lid.hm file you saved to your working directory.
  3. Click Open.
    The coffee_lid.hm database is loaded into the current HyperMesh session, replacing any existing data.

Set Up the Model

Create the Material

The 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 from the context menu.
    A default material displays in the Entity Editor.
  2. For Name, enter plastic.
  3. Set Card Image to MAT1.
  4. Enter the material values next to the corresponding fields.
    1. For E (Young's Modulus), enter 1137.
    2. For NU, (Poisson's Ratio), enter 0.26.
    3. For A (coefficient of linear thermal expansion), enter 8.1e-005.
    4. For RHO (Mass Density), leave it undefined since only a static analysis is performed.


    Figure 1. Material Property Values for plastic
A new material, plastic, has been created. The material uses OptiStruct's linear isotropic material model, MAT1.

Edit the PSHELL Property

  1. In the Model Browser, Properties folder, click PSHELL.
    The PSHELL property entry is displayed in the Entity Editor.
  2. Verify that the thickness value, T, is set to 2.5.
  3. For Material, click Unspecified > Material.
    Note: The Value field next to Material is set to <Unspecified>. This indicates that no material properties are being referenced by this property.

    OS_1010_02
    Figure 2. Selecting the Material plastic for the Property PSHELL
  4. In the Select Material dialog, select plastic and click OK.
    The material plastic is now assigned to the property PSHELL.

    OS_1010_03
    Figure 3. The PSHELL Property Entry Fields in the Entity Editor
  5. Assign the material plastic to the property PSHELL1.
The property collectors and component collectors, PSHELL and PSHELL1, now reference the material plastic. The component collectors that reference the corresponding properties are automatically updated with the specified material. If you access the Entity Editor and edit either of these property or component collectors, notice that the Material fields are now all set to plastic.

Apply Loads and Boundary Conditions

Thermal loading has already been applied to the model. In the following steps, constraints will be applied to the model.

Create Load Collectors

  1. In the Model Browser, right-click and select Create > Load Collector from the context menu.
    A default load collector displays in the Entity Editor.
  2. For Name, enter constraints.
  3. Click Color and select a color from the color palette.
  4. Set Card Image to None.
    A new load collector, constraints is created.


    Figure 4. Creating the constraints Load Collector

Create Constraints at the Corners of the Spout Cut-out

  1. From the menu bar, click BCs > Create > Constraints to open the Constraints panel.
  2. Set the entity selector to nodes, then select the two nodes at the corners of the spout cut-out.

    os1010_pic1
    Figure 5. Selecting Nodes for Constraints at Corners of Spout Cut-Out
  3. Constrain only DOF3.
    • 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.
  4. Click create.
    Two constraints are created. Constraint symbols (triangles) appear in the graphics area at the selected nodes. The number 3 is written beside the constraint symbol, indicating the DOF constrained.
  5. In the size field, enter 1.0.
    The size of the constraint symbols in the modeling window change.
  6. Click return to go back to the main menu.

Create Constraints Opposite the Spout Cut-Out

  1. From the menu bar, click Geometry > Create > Nodes > XYZ to open the Nodes: XYZ panel.
  2. In the XYZ panel, define coordinates for the node.
    1. In the x field, enter 0.0.
    2. In the y field, enter -10.0.
    3. In the z field, enter 0.0.
  3. Click create.
    A node is created with the coordinates (0, -10, 0). This indicates the centerline of the coffee lid.
  4. Click return to go back to the main menu.
  5. From the menu bar, click BCs > Create > Constraints to open the Constraints panel.
  6. Using the entity selector, select the nodes indicated in Figure 6.

    os1010_pic2
    Figure 6. Creating Constraints Opposite the Spout Cut-Out to Model Hinges
  7. Constrain only dof1, dof2, and dof3.
  8. Click create.
    Four constraints are created. Again, this is verified by the appearance of constraint symbols in the modeling window.
  9. Click return to go back to the main menu.
  10. From the Geom page, select the temp nodes panel.
  11. Click clear all.
    The temporary node that was created at (0, -10, 0) is removed.
  12. Click return.

Create Load Steps

  1. In the Model Browser, right-click and select Create > Load Step from the context menu.
  2. For Name, enter brew cycle.
  3. Set Analysis type to Linear Static.
  4. Define SPC.
    1. For SPC, click Unspecified > Loadcol.
    2. In the Select Loadcol dialog, select constraints and click OK.
  5. Define TEMP.
    1. For TEMP, click Unspecified > Loadcol.
    2. In the Select Loadcol dialog, select THERMAL_LOADING and click OK.

An OptiStruct subcase has been created which references the constraints in the load collector constraints and the forces in the load collector THERMAL_LOADING.



Figure 7. Creating the brew cycle Loadstep

Submit the Job

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

    OS_1000_13_17
    Figure 8. Accessing the OptiStruct Panel
  2. Click save as.
  3. In the Save As dialog, specify location to write the OptiStruct model file and enter lid_complete for filename.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The input file field displays the filename and location specified in the Save As dialog.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the lid_complete.fem was written. 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 the directory are:
lid_complete.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
lid_complete.out
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.
lid_complete.h3d
HyperView binary results file.
lid_complete.res
HyperMesh binary results file.
lid_complete.stat
Summary, providing CPU information for each step during analysis process.

View the Results

Displacement and Stress results are output from OptiStruct for Linear Static Analyses by default. The following steps describe how to view those results in HyperView.

View the Deformed Shape

  1. When the message ANALYSIS COMPLETED is received in the Solver View window, click Results.
    HyperView is launched and the results are loaded.
  2. Click the Wireframe Elements icon visualizationElementsWireframe-24 on the toolbar.
  3. Set the Animation Mode to Linear animationLinear-24.
  4. Select the Deformed panel toolbar icon resultsDeformed-24.
  5. Define settings in the Deformed panel.
    1. Set Result type to Displacement (v).
    2. Set Scale to Model units and enter a value of 2.
      This means that the maximum displacement will be two model units and all other displacements will be proportional.
    3. Set the toggle under Undeformed Shape to Wireframe.
    4. Select Color as the Component.
  6. Click Apply.
A deformed plot of the model should be visible, overlaid on the original undeformed mesh.

os1010_pic3
Figure 9. Isometric View of Deformed Plot Overlaid on Original Undeformed Mesh with Model Units Set to 2.
Try to answer the following questions to test your understanding of the current problem.
  • Does the deformed shape look correct for the boundary conditions applied to the mesh?

View a Contour Plot of Stresses and Displacements

  1. On the Results toolbar, click resultsContour-16 to open the Contour panel.
  2. Define settings in the Contour panel.
    1. Set Result type to Displacement (v).
    2. Set Data type Mag.
      Mag represents the magnitude of the displacements.
  3. 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.
    • What is the maximum displacement value?
    • At what location does the model have its maximum displacement?
    • Does this make sense based on the boundary conditions applied to the model?
  4. Define settings in the Contour panel.
    1. Set Result type to Element Stresses (2D & 3D).
    2. Set Data type to vonMises.
  5. 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.
    • What is the maximum von Mises stress value?
    • At what location does the model have its maximum stress?
    • Does this make sense based on the boundary conditions applied to the model?
  6. Click File > Exit to leave HyperView.
In this analysis, the region around the hinges may be a concern. There are relatively high stress values that must be resolved. For instance, if testing shows that the coffee pot lid wears out around the hinge area over time, these thermal stresses could possibly cause that fatigue.

rd1010_spout_cutout
Figure 10. Hinge Opposite of the Spout Cut-Out