I really hope you achieve the effect through this idea.

Slice Master

Is it throwing any error? 

Negative cell volume detected in Fluent. You can open the Fluent results and check the exact location of failure. I guess it is in the lubricant thickness region between the ball and the race. Have a sufficient number of cells of good quality in that region. 

You can refer 'Mesh Folds within the First Coupling Steps' in the user guide: 42.6. FSI Setup Recommendations for Fluent-Mechanical Couplings (ansys.com)

How many cells do you have in that thin region and what are the dynamic mesh settings? Are you using remeshing?

1. After failure, check the location of the mesh fold in Fluent and improve the mesh at that location using local sizing. Also, check the suggestions from 'Mesh Folds within the First Coupling Steps' in the user guide: 42.6. FSI Setup Recommendations for Fluent-Mechanical Couplings (ansys.com).
2. Try applying the gradual load with ramping of data transfers to avoid the mesh failure at the start of the solution.
3. Set lubricant zone to 'Deforming' in Dynamic mesh zones settings. You can refer to tutorial Reed Valve FSI Co-Simulation with Partial Setup Export from Workbench (Fluent-Mechanical) to understand the Two-way coupling setup.

Hello,
Check your boundary conditions here to see if the forces/displacement applied to the correct boundary.

Check if the forces from fluent are transferred correctly. Have you tried running a Fluent alone case? Is it working well? 

Also, share the contact settings and BCs used in Mechanical participant.

By run fluent alone, I mean run Fluent alone with a representative load on the FSI boundary to see the mesh deformation and assess if it is solving correctly.

Have you removed this contact definition in the FSI case?

Try keeping the contact definition as is. It models a true gap as you are not providing any offset here. Using this setting will not close gaps.

Check 9.6.3.5. Geometric Modification for more info. 

Change it to frictionless contact type as they not touching each other.

Negative volume error, make sure the mesh mesh in fluent has an orthogonal mass of more than 0.2, and then try to lower the step size again

Okay. In that case, try using the gap model in Fluent with Flow modeling as discussed in this tutorial: Reed Valve FSI Co-Simulation with Partial Setup Export from Workbench (Fluent-Mechanical)

You can find info about gap model in user guide here: 6.8. Controlling Flow in Narrow Gaps for Valves and Pumps

Same problem? negative volume error or inner race not moving correctly?

As you have a very small gap between the race and the ball, it makes the setup difficult. Also, the mesh is moving in that zone, so it must be handled very carefully. 

This setting specifies the minimum distance to be maintained between the faces of the moving bodies equal to the current gap size. This will prevent the fluid mesh from collapsing by preventing the ball from interpenetrating the race (you can try specifying the offset = gap size).

Here Fluid flow(CFX) uses the CFX solver

         Fluid Flow(Fluent with Fluent Meshing) uses the Fluent solver and Fluent Meshing mesher is used to mesh the geometry

         Fluid Flow(Fluent) uses the Fluent solver and geometry is meshed with Ansys WB Mesher

         Fluid Flow(Polyflow) is not for case.

You can use Fluid Flow(Fluent with Fluent Meshing) or Fluid Flow(Fluent).

Again, I would recommend you check the BCs. 
There should be 3 surfaces (Coupling Interfaces) across which Fluent and Mechanical would exchange the data i.e. inner race, outer race, and ball surface.