I looked at a model jonnyflowers was working on and wrote some suggestions that may be helpful. The model has one body, a silicon chip, inside a large rubber block.
First Observation is to set Topology to Shared in SpaceClaim, and delete the Contact in Mechanical. That creates the bond between the silicon chip and the rubber by having them share nodes instead of adding contact elements. However, contact elements can be useful if you want to get the pressure at the interface. If you need the contact, then create a New Component and put the silicon chip in that new component, leaving the other component to hold all the sliced parts of the block.
Second observation is you can have a better mesh within the Student limit if you slice the block up around the silicon chip, so that hex meshing can be used instead of tet meshing. The section view below show the silicon chip in the center of the block.
Third observation, you can reduced the number of equations in the model if you slice off the end where you are applying the remote displacement on four side faces, and just apply the remote displacement on the cut end face.
Last observation is to change Automatic Time Stepping to On instead of Program Controlled, then set initial substeps of 40, and limit the maximum substeps to 20. That will allow the solver to have more successful converged substeps and spend less time bisecting to smaller substeps after taking too large of a substep.
I incorporated these suggestions in the attached ANSYS 18.2 archive. It will solve in 394 iterations, which took 10.8 minutes on 16 cores, but 40.6 minutes on 2 cores.