07 February 2020
- Last edited 07 February 2020
On this computer, the oldest version I have is ANSYS 19.2 so you will have to redo this on 17.0 because you can't open my file on an older version. Is there any chance for you to upgrade to the latest version? There are many improvements in meshing and solving.
The first step is to get a great mesh.
1. Use Symmetry, it will take less time to solve.
2. Use Shared Topology and delete Contact. Note: this makes the meshing a bit more challenging. Actually, do this after all the slicing in step 4.
3. Reduce the tube size slightly to get rid of tangent conditions with walls to eliminate poor element shapes.
4. Slice the thin wall from the base to help meshing. Create a Tool and use Boolean Operations to make many parts to help meshing. I have exported these solids as a STEP file (attached below) that you should be able to import into DesignModeler.
Center Layer Mesh. Note two elements through the membrane thickness.
5. Under Analysis Settings, turn Auto Time Stepping On. Set the Initial, Minimum and Maximum Substeps to 100. turn Large Deflection On.
6. Create and assign the PDMS material to the bodies.
7. Repair the Fixed support and the Pressure loads to include the new faces. Repair the Named Selection. I reduced the pressure to 7 MPa.
8. Add Frictional Contact between the small membrane face and the top layer small face that it will close against. Set the Pinball radius so that the blue sphere reaches across the gap. Insert a Contact Tool under the Connections folder and Evaluate Initial Contact Status to confirm that the status is Near Open.
Change the units to mm, now you are ready to Solve! I will describe the results in the next post.