OS-T: 5100 Stress Response based on Neuber Correction Method

The tutorial demonstrates Neuber shape optimization to reduce the stress concentration at the fillet regions by changing its shape.

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

neuber_shape_optimization.hm

The following exercises for shape optimization based on the Neuber correction method are:

Set up the objective, constraints and design variables in HyperMesh
Submit the job in OptiStruct
View results in HyperView

Figure 1 illustrates the structural model used for this tutorial. This tutorial has a half symmetric valve, which is modeled using first order tetra elements and has a force applied at a specific location. A shape ID is created using HyperMorph and the Shape design variables is created. A static stress response is created with Neuber correction and a mass response defined by an equation to minimize the change in the mass. A design constraint is defined for static-stress response.

The optimization problem for this tutorial is stated as:

Objective: Minimize the change in mass.
Constraints: Minimize the static stress to a value less than 330 MPa using Neuber correction method
Design Variables: Shape design variables.

Launch HyperMesh and Set the OptiStruct User Profile

Launch HyperMesh.
The User Profile dialog opens.
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

Click File > Open > Model.
Select the neuber_shape_optimization.hm file you saved to your working directory.
Click Open.
The neuber_shape_optimization.hm database is loaded into the current HyperMesh session, replacing any existing data. The database contains meshed data, material data and shape ID created.

Set Up the Model

Create Property

Here you will assign the property, as the Valve is a solid part.

In the Model Browser, right-click and select Create > Property.
For Name, enter PSOLID.
For Card Image, select PSOLID.
For Material, select Aluminum.
From the Model Browser, Component folder, right-click on Valve and assign the property PSOLID.

Create FORCE Load Collector

First you will isolate the component and then apply the force.

In the Model Browser, right-click the component axis and select isolate only.
In the Model Browser, right-click Create > Load Collector.
For Name, enter Force.
From the menu bar, click BCs > Create > Forces.
Toggle to nodes and select the middle node of AXIS element (RBE2 element).
Assign the values, as shown in the image.

Figure 2. Apply Force
Click Create.

Create SPC Load Collector

In the Model Browser, right-click Create > Load Collector.
For Name, enter SPC.
From the menu bar, click BCs > Create > Constraints.
For the first drop-down, toggle to nodes and for the second drop-down menu, select faces.
Select only dof2, deselect all other dof's and click Create.
Select the side face of the Valve and select only dof1, dof2 and dof3.
Click Create.
Similarly, select the other side faces of the Valve and select only dof1 and dof2.

Figure 3. Apply Constraints

Create Load Steps

In the Model Browser, right-click and select Create > Load Step.
A default load collector displays in the Entity Editor.
For Name, enter Static.
For Type, select linear static from the drop-down menu.
For SPC, select SPC.
For load definition, select force.

Create Design Equations

From the Analysis page, click optimziation > dequations panel.
In the dequation = field, enter Delta.
In the edit equation field, enter delta(x)=x-9.892e-02.

Figure 4. Design Equation
Click Create.

Note: Delta(x) is changed in mass; where, x represents the actual mass with respect to change in shape and mass of the valve is 9.892e-02 kg.
Select Tools > mass Calc > comps, select valve and click calculate.

Figure 5. Mass of the Valve

Create Shape Optimization Design Variables

From the Analysis page, click optimization > shape panel.
Toggle desvar subpanel.
For desvar =, enter Variable as the name of the design variable.
For shape =, enter Fillet_shape.
For lower bound, enter 0 and for upper bound, enter 1.
Click create and return.

Figure 6. Create Design Variables

Note: Potential variation in the shape of the Valve is increased in the fillet radius.

Create Optimization Responses

Create Mass Response Type

From the Analysis page, click optimization > responses panel.
For response =, enter Mass.
In the drop-down, select response type as mass and click return.

Figure 7. Mass Response

Create Static Stress Response Type

From the Analysis page, click optimization > responses panel.
For response, enter Neuber.
From the drop-down, select response type as static stress.
Click elems > by collector > Valve.
Select neuber correction, as shown in the image.

Figure 8. Static Stress Response
Click create.

Create Function Response Type

In the Model Browser, select Optimization View.
Right-click and select Window > Create > Responses.
For Name, enter Delta_Response.
For Function, select Response type.
For Function ID, select Delta, which is Dequation created in previous step.
Expand Response List and select Optiresponse as the Mass.

Figure 9. Function Response Type

Note: To create change in mass response, Function response is used here.

Create Design Constraints

Click the dconstraints panel.
In the constraint= field, enter Constraints.
Click response type and select neuber, which is a static stress response type.
Select loadstep 1 - Static.
Select upper bound and enter a value of 330.

Define the Objective Function

Click the objective panel.
Verify that min is selected.
Click response type and select Delta_Response.
Click Create.

Define the SHAPE Card

Only displacement and stress results are available in the .h3d file by default. In order to look at displacement/stress results on top of a shape change that was applied to the model in HyperView, a SHAPE card needs to be defined.

From the Analysis page, click the control cards panel.
In the Card Image dialog, click SHAPE.
Set FORMAT to H3D.
Set TYPE to ALL.
Set OPTION to ALL.
Click return twice to go back to the main menu.

Run the Optimization

From the Analysis page, click OptiStruct.
Click save as.
In the Save As dialog, specify location to write the OptiStruct model file and enter neuber_based_opimization for filename.
For OptiStruct input decks, .fem is the recommended extension.
Click Save.
The input file field displays the filename and location specified in the Save As dialog.
Set the export options toggle to all.
Set the run options toggle to optimization.
Set the memory options toggle to memory default.
Click OptiStruct to run the optimization.
Click Close.

View the Results

The following steps demonstrate how to review the contour plot with the optimized shape in HyperView.

It is helpful to view the deformed shape, stresses in the model using Neuber correction method .

From the OptiStruct panel, click HyperView.
HyperView is launched and the results are loaded. A message window appears to inform of the successful model and result files loading into HyperView.
Go to the Results tab.
In the Results tab, select Iteration 23, the last iteration.

Figure 10. Iterations Selection
On the Results toolbar, click to open the Contour panel.
Set Result type to Shape change (v) and click Apply to contour the elements.

Figure 11. Shape Change Results
Set Result type to Neuber stress.
Click Apply.

Figure 12. Element Stress Results
Open a new HyperView window and select File > Open > Session.
Select <filename>_hist.mwv to view the change in mass and the optimized mass after changing the shape.

Figure 13. Session Plot Results
View the plot results for objective function and total mass.

Figure 14. Objective Function and Total Mass Plot