Hello Mirvari,
In Workbench, delete the Topology Optimization system. Open the Geometry using SpaceClaim. On the Prepare tab, click the Midsuface button and click the two faces on this thin part. A surface will replace your solid model in Mechanical.
In Mechanical, delete the Fixed Support and delete the Force on the lower edge. Reattach the Force on the upper edge.
Insert a Remote Displacement on the lower edge. In the Details window, check the Behavior is Deformable and set all six rows to be 0.0 instead of Free.
Drag the Remote Displacment and drop it on the Solution branch to insert a Force Reaction output. This will show you that the reaction force is equal and opposite to the applied force. Right click on the Solution branch to Insert a Stress Tool for Max Equiv Stress to get the Safety Factor plot. Click the box next to Minimum on the Safety Factor to turn that into an output parameter.
One input parameter that is easy to adjust the mass is the thickness of the part. Click on the Midsurface under the Geometry in the Outline. Click on the box next to the word Thickness in the Detail window and a blue P will appear. Also click the box next to the Mass.
In Workbench, there will be a Parameter Set. Now you can type in a set of thickness values on several rows of the Table of Design Points and click the Update All Design Points to have Ansys automatically calculate the Safety Factor for each thickness and report the Mass.
Since you have only one input parameter, your response surface is a response curve, but you can plot the curve and find the value of the thickness when the curve crosses a value of 1.5 on the Safety Factor axis.
Once you have mastered this, you can add shape parameters to the geometry and have multiple input parameters. Then you can introduce the Response Surface tool under the Design Exploration category of Workbench and minimize the mass by varying many input parameters including thickness.
Regards,
Peter
You are navigating away from the AIS Discovery experience