peteroznewman
Subscriber

1. Yes, make the flat plates in 3D but make them thicker, like a 6 mm cube, so the cylinder is in the center and the contact faces must be tangent to the cylinder.

Symmetry should be used to make this problem easier and faster to solve. The cylinder gets squeezed from both sides equally, therefore if you put a horizontal plane through the center of the cylinder the top half and the bottom half of the cylinder look like mirror images. Therefore, cut the model in half (keep the top) and use a Symmetry boundary condition. Similarly, if you put a vertical plane through the center of the cylinder, the left side looks like a mirror image of the right side. Therefore, cut the model in half again (keep the left) and use another Symmetry boundary condition.

2,3,4. Use a Static Structural analysis block, and import or draw your Geometry in SpaceClaim, then close that and open the Model. Click on the Static Structural branch. Since you are not interested in the deformation of the cube, you can make it rigid. Pick the body in the tree and where it says Flexible, pull down and select Rigid. While you are there, rename the three solids: Base, Coating and Plate.

RMB on the Connections folder and Insert Joint. There are a row of filters on the toolbar for Vertex, Edge, Face and Body. Pick the Face filter. Select the top face of the top quarter cube. Change Body-Body to Body-Ground. Change Fixed to Translation. You then have to reorient the Coordinate System under the joint so that the X axis of that Coordinate System points in the Global Y direction.

Drag and drop that Translation joint on the Static Structural branch to create a Joint Load. Change from displacement to Force and enter the force you want, but use a negative number to make it point down.

The default installation will automatically create all the contacts, but they are all bonded. Select all the contacts and RMB to Rename based on definition. That will make it use the names you gave the solids above. Select the two contacts with Plate in the name and change them from Bonded to Frictional. Enter a friction coefficient.

Go to Engineering Data and create the materials for Base and Coating. At a minimum you need a Isotropic Elasticity and in there you enter Young's Modulus and Poisson's Ratio.  Refresh the Project, then in Mechanical, assign those two materials to those two parts.

In Analysis Settings, you will want to turn on Auto Time Stepping and use 100 substeps.

In Meshing you will want to add mesh controls to get nice small elements at the contact point.

Then you can finally Solve.

Regards,
Peter