# OS-T: 3100 Combined Topology and Topography Optimization of a Slider Suspension

In this tutorial you will perform a combined topology and topography optimization on a slider suspension using OptiStruct.

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

The objective of this tutorial is to increase the stiffness of the slider suspension and make it lighter at the same time. This requires the use of both topology and topography optimization.

The finite element model of the slider suspension contains force and boundary conditions. The structure is made of quad elements and has both linear statics and normal modes subcases (loadsteps). Steps are described to define topology and topography design space, responses, constraints, and objective function. The optimized structure will be stiffer for both linear statics and normal modes subcases and will have beads and less material.
Perform combined topology and topography optimization on a disk drive slider suspension to maximize the stiffness and weighted mode. The lower bound constraint on the seventh mode is 12 cycles/ms.
Objective Function
Minimize the combined weighted compliance and the weighted modes.
Constraints
7th Mode > 12 cycles/ms.
Design Variables
Element densities and nodes topography.

## 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.

## Import the Model

1. Click File > Import > Solver Deck.
2. For the File type, select OptiStruct.
3. Select the Files icon .
A Select OptiStruct file browser opens.
4. Select the combined.fem file you saved to your working directory.
5. Click Open.
6. Click Import, then click Close to close the Import tab.

## Set Up the Optimization

### Create Topology Design Variables

1. From the Analysis page, click optimization.
2. Click topology.
3. Select the create subpanel.
4. In the desvar= field, enter pin.
5. Set type: to PSHELL.
6. Using the props selector, select 1pin.
7. Verify that the base thickness is 0.0.

A value of 0.0 implies that the thickness at a specific element can go to zero, and therefore becomes a void.

8. Click create.
9. Repeat the above steps to create a design variable labeled bend, and assign it the 3bend property.
10. Click return.

### Define Topography Design Variables

For a topography optimization, a design space and a bead definition need to be defined.

1. From the Analysis page, click the optimization panel.
2. Click the topography panel.
3. Create a topography design space definition.
1. Select the create subpanel.
2. In the desvar= field, enter tpg.
3. Using the props selector, select 1pin and 3bend.
4. Click create.
A topography design space definition, tpg, has been created. All elements organized into the 1pin and 3bend component collector(s) are now included in the design space.
4. Create a bead definition for the design space tpg.
1. Select the bead params subpanel.
2. Verify the desvar = field is set to tpg, which is the name of the newly created design space.
3. In the minimum width= field, enter 0.4.
This parameter controls the width of the beads in the model. The recommended value is between 1.5 and 2.5 times the average element width.
4. In the draw angle= field, enter 60.0 (this is the default).
This parameter controls the angle of the sides of the beads. The recommended value is between 60 and 75 degrees.
5. In the draw height=, enter 0.15.
This parameter sets the maximum height of the beads to be drawn.
6. Select buffer zone.
This parameter establishes a buffer zone between elements in the design domain and elements outside the design domain.
7. Toggle draw direction to normal to elements.
This parameter defines the direction in which the shape variables are created.
This tells OptiStruct to leave nodes at which loads or constraints are applied out of the design space.
9. Click update.

A bead definition has been created for the design space tpg. Based on this information, OptiStruct will automatically generate bead variable definitions throughout the design variable domain.

Use 1-plane symmetric beads, as it is the simplest and can be symmetric at the same time.
1. Select the pattern grouping subpanel.
2. Click desvar = and select tpg.
3. Set the pattern type to 1-pln sym.
4. Click anchor node, and enter 41 in the id= field.
5. Click first node, and enter 53 in the id= field.
6. Click update.
6. Update the bounds of the design variable.
1. Select the bounds subpanel.
2. Verify the desvar = field is set to tpg, which is the name of the design space.
3. In the Upper Bound= field, enter 1.0.
Upper bound on variables controlling grid movement (Real > LB, default = 1.0). This sets the upper bound on grid movement equal to UB*HGT.
4. In the Lower Bound= field, enter 0.0.
5. Click update.
The upper bound sets the upper bound on grid movement equal to UB*HGT and the lower bound sets the lower bound on grid movement equal to LB*HGT.

### Create Optimization Responses

Since this problem is a combined linear static and normal mode analysis, you are trying to minimize compliance and increase frequency for the two load cases, while constraining the seventh frequency. Therefore, two responses are defined: freq and comb.

1. From the Analysis page, click optimization.
2. Click Responses.
3. Create the frequency response.
1. In the responses= field, enter freq.
2. Below response type, select frequency.
3. For Mode Number, enter 7.0.
4. Click create.
A response, freq, is defined for the frequency of the seventh mode extracted.
4. Create the compliance index response.
1. In the response= field, enter comb.
2. Set the response type to compliance index.
3. Using the loadsteps selector, select force.
4. Toggle the option to define the normalizing factor to autonorm.
5. In the Mode and Weight fields, enter the mode numbers and their corresponding weights.
Mode
Weight
1
1.0
2
2.0
3
1.0
4
1.0
5
1.0
6
1.0
6. Click create.

### Create Design Constraints

1. Click the dconstraints panel.
2. In the constraint= field, enter frequency.
3. Click response = and select freq.
4. Check the box next to lower bound, then enter 12.
5. Using the loadsteps selector, select frequency.
6. Click create.

### Define the Objective Function

1. Click the objective panel.
2. Verify that min is selected.
3. Click response= and select comb.
4. Click create.
5. Click return twice to exit the Optimization panel.

### Define Optimization Control Cards

1. From the Analysis page, click the Optimization panel.
2. Click the opti control panel.
3. Select MINDIM, and enter 0.25.
Minimum member size is generally recommended to avoid checkerboarding. It also ensures that the structure has the minimum dimension specified in this card.
4. Select MATINIT, and enter 1.0.
MATINIT declares the initial material fraction in a topology optimization. MATINIT has several defaults based upon the following conditions: If mass is the objective function, the MATINIT default is 0.9. With constrained mass, the default is reset to the constraint value. If mass is not the objective function and is not constrained, the default is 0.6.
5. Click return twice to exit the panel.

### Set Mode Tracking

During the optimization, the frequencies and their mode shape may change order due to the change in element densities and other design changes. To overcome this, define a parameter to track the frequencies so that only the intended frequencies are tracked during optimization runs.
1. From the Analysis page, click the control cards panel.
2. In the Card Image dialog, click PARAM.
3. Select MODETRAK.
4. Set MODET_V1 to Yes.
5. Click return.
The PARAM button is now green, indicating that it is active.

## Run the Optimization

1. From the Analysis page, click OptiStruct.
2. Click save as.
3. In the Save As dialog, specify location to write the OptiStruct model file and enter comb_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 optimization.
7. Set the memory options toggle to memory default.
8. Click OptiStruct to run the optimization.
The following message appears in the window at the completion of the job:
OPTIMIZATION HAS CONVERGED.
FEASIBLE DESIGN (ALL CONSTRAINTS SATISFIED).
OptiStruct also reports error messages if any exist. The file comb_complete.out can be opened in a text editor to find details regarding any errors. This file is written to the same directory as the .fem file.
9. Click Close.

## View the Results

### Post-Process the Shape Results Change (Topography)

1. From the OptiStruct panel, click HyperView.
HyperView is launched.
2. On the Results toolbar, click to open the Deformed panel.
3. Under Deformed shape, define deformed shape settings.
1. Set the Result type to Shape Change(v).
2. Set Scale to Scale factor.
3. Set Type to Uniform.
4. In the Value field, enter 1.0.
4. Under Undeformed shape, set Show to None.
5. Click Apply.
The shape change due to the topography optimization displays.
6. In the Results Browser, set the Load Case and Simulation Selection to 25th iteration.

### Contour the Optimum Material Distribution (Topologic)

1. On the Results toolbar, click to open the Contour panel.
2. Set the Result Type to Element Densities (s) and Density.
3. Set the Averaging method to Simple.
4. Click Apply to display the density contour.

### Add Iso Surface of the Optimum Material Distribution (Topologic)

1. On the Results toolbar, click to open the Iso Value panel.
2. Set the Result Type to Element Densities (s) and Density.
3. Set Show values to Above.
4. Click Apply to display the density iso-surface plot.
5. In the Current value field, enter 0.3.
An iso-surface plot is displayed. Those parts of the model with a density greater than the value of 0.3 are shown in with density contour, the rest are removed from the display.