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.
In the New Session window, select HyperMesh from the list of tools.
For Profile, select OptiStruct.
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
On the menu bar, select File > Open > HyperMesh Model.
Navigate to and select the coffee_lid.hm file saved in your
working directory.
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 model has two component
collectors with no materials. A material collector needs to be created and assigned
to the component collectors.
In the Model Browser, right-click and select Create > Material from the context menu.
A default material displays in the Entity Editor.
For Name, enter plastic.
Set Card Image to MAT1.
Enter the material values next to the corresponding fields.
For E (Young's Modulus), enter 1137.
For NU, (Poisson's Ratio), enter 0.26.
For A (coefficient of linear thermal expansion), enter
8.1e-005.
For RHO (Mass Density), leave it undefined since only a static
analysis is performed.
A new material, plastic, has been created. The
material uses OptiStruct's linear isotropic material
model, MAT1.
Click Close.
Edit the PSHELL Property
In the Model Browser, Properties folder, double-click
PSHELL.
The PSHELL property entry is displayed in the Entity Editor.
Verify that the thickness value, T, is set to 2.5.
For Material, click Unspecified > to open Advanced Selection.
Select plastic as the material.
Note: The Value field next to Material is set to <Unspecified>.
This indicates that no material properties are being referenced by this
property.
Repeat steps 1 through 4 to update the PSHELL1 property and assign the
plastic material.
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
In the Model Browser, right-click and select Create > Load Collector from the context menu.
A default load collector displays in the Entity Editor.
For Name, enter constraints.
Click Color and
select a color from the color palette.
Set Card Image to None and click
Close.
Create Constraints at the Corners of the Spout Cut-out
From the menu bar, open the
Analyze ribbon.
On the ribbon, click Constraints.
Set the entity selector to nodes, then select the two
nodes at the corners of the spout cut-out.
Figure 3. Selecting Nodes for Constraints at Corners of Spout Cut-Out
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.
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.
Click Close.
Create Constraints Opposite the Spout Cut-Out
From the menu bar, open the
Geometry ribbon.
Select Create points.
In the guide bar, select Create Free Nodes from the
drop-down menu.
Left-click the window to open the XYZ popup.
In the XYZ panel, define coordinates for the node.
In the x field, enter 0.0.
In the y field, enter -10.0.
In the z field, enter 0.0.
From the Analyze ribbon, select Constraints.
Using the entity selector, select the nodes indicated in Figure 4.
Figure 4. Creating Constraints Opposite the Spout Cut-Out to Model
Hinges
Constrain only dof1, dof2, and
dof3.
Click create.
Four constraints are created. Again, this is verified by the appearance
of constraint symbols in the modeling window.
Click close.
From the Geom ribbon, select create points.
Click delete.
The temporary node that was created at (0, -10, 0) is
removed.
Create Load Steps
In the Model Browser, right-click and select Create > Load Step from the context menu.
For Name, enter brew cycle.
Set Analysis type to Linear Static.
Define SPC.
For SPC, click Unspecified > to open Advanced Selection.
In the dialog, select constraints and
click OK.
In Subcase Options, select TEMP > Loadcolid.
For TEMP, click Unspecified > to open Advanced Selection.
In the dialog, select THERMAL_LOADING and click
OK.
Click Close.
An OptiStruct subcase is created which
references the constraints in the load collector constraints and the forces in
the load collector THERMAL_LOADING.
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 5. Creating the brew cycle Loadstep
Submit the Job
Run OptiStruct.
From the Analyze ribbon, click Run OptiStruct
Solver.
Figure 6. Select Run OptiStruct Solver
A browser window opens.
Select the directory where you want to write the OptiStruct model file.
For File name, enter lid_complete.
The .fem filename extension is the recommended extension
for Bulk Data Format input decks.
Click Save.
Click Export.
For export options, toggle all.
For run options, toggle analysis.
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:
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
When the message ANALYSIS COMPLETED is received in the Solver
View window, click Results.
HyperView is launched and the results are
loaded.
Click the Wireframe Elements icon on the
toolbar.
Figure 7. Wireframe Elements
Set the Animation Mode to Linear.
Figure 8.
On the Results ribbon, select the Deformation
icon.
Figure 9.
Set Result type to Displacement (v).
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.
Set the toggle under Undeformed Shape to
Wireframe.
Select Color as the Component.
Click Apply.
A deformed plot of the model should be visible, overlaid on the original undeformed
mesh.Figure 10. 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
On the Results toolbar, click to open the
Contour panel.
Define settings in the Contour panel.
Set Result type to Displacement (v).
Set Data type Mag.
Mag represents the magnitude of the displacements.
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?
Define settings in the Contour panel.
Set Result type to Element Stresses (2D &
3D).
Set Data type to vonMises.
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?
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.Figure 11. Hinge Opposite of the Spout Cut-Out