Getting frictional contact to solve is difficult if you don't know all the steps to follow, and adding in plasticity makes it very difficult to solve to the full load. You can show your appreciation by clicking "Like" on the posts that are helpful.
1) Make sure the geometry is in contact
I bet that the pin and hole are concentric, which means when you made the hole larger than the pin, they are no longer touching. I calculate a radial clearance of 0.0125 mm. You must translate the pin up by that distance to get it to touch the top of the hole. That way, the solver can start with the mesh in initial contact.
2) Add a Contact Tool to the Connections Folder
When you Generate Initial Contact Results from the Contact Tool, it will tell you if there is initial contact or not, and the size of the gap or penetration. A very small penetration is good, a very small gap is a problem. If you have a very small gap, use Adjust to Touch.
3) Use Adjust to Touch
Go to the details for the Frictional Contact where in Geometry Modification, Interface Treatment you will find Adjust to Touch. This will take your very small gap and close it.
4) Turn On Auto Time Stepping instead of Program Controlled
In Analysis Settings, Step Controls, change Auto Time Stepping from Program Controlled to On. Define By Substeps. Set Initial Substeps to 50, Minimum Substeps to 10 and Maximum Substeps to 500. You don't want the solver trying to apply the full load in a single step, since the displacement can be so large that the pin ends up meters past the hole. You need to tell it to take 50 substeps as an initial step size. The solver will automatically increase the step size as it converges on each substep. Also, if you want to plot a curve on the way to the full load, you want to specify a minimum step size, so you are guaranteed at least 10 points on your curve.
5) Turn on Large Deflection.
Under Analysis Settings. This is essential when using a plasticity model that will see large strains.
6) Displacements are easier to converge on than Forces
You want a Force-Displacement curve, so you can either apply force and calculate displacement, or you can apply a displacement and calculate reaction force. It is much easier for the solver to do the later.
Applied displacement is required when using plasticity if you want to simulate beyond the point where the force-displacement curve approaches a maximum.
You haven't used symmetry as I advised above and there is a potential problem in your model with forces applied at the two ends of a pin that extends so far from the plate. Is each end of the pin exactly the same distance from the face of the plate? If not, there will be a moment that tries to tilt the pin and you don't want that. Symmetry would fix that. However, I strongly recommend you delete the force BC on the ends of the pin and replace it with a displacement BC. You can specify a 1 or 2 mm Y displacement. You could either set X and Z to zero or leave them free. There is less chance of a convergence error if you set them to zero.
It probably won't matter in this model, but the best practice is to put the contact side of the contact pair on the softer material and the target side of the contact pair on the harder material. So in your case you should flip the contact pair. If the two materials are similar modulus, then the contact side goes on the geometry with a smaller radius and the target side goes on the larger radius (or flat) side of the contact pair.
The reason the ridiculously large elements worked was because they "cut the corner" on the radial clearance to give you an initially closed contact. Go back to smaller elements after you translate the pin to be in contact.