It looks like you wanted to do a 2D analysis. You should do that.
First, set the Geometry properties to 2D instead of 3D
Then in DesignModeler, create surfaces from sketches instead of Extrude a solid.
Open Mechanical and set the geometry to Plane Strain.
What is in your 3D model is not Plane Strain because you only held one face of each body to have z=0. If you had picked the front and the back faces of each body to have z=0, then it would have been Plane Strain. What you have is more like Plane Stress, but two bodies that thin would buckle out of plane under these conditions.
So after not answering your questions, let me now answer them.
The first message is just a warning. Large deformation effects may have invalidated ... but in this case, they did not invalidate anything. Everything you wanted is still valid. You can ignore this warning.
The second message is seen when there may be rigid body motion, or a mechanism type of situation. There is no Static Equilibrium in those cases, so rather than throw an error and say no solution, ANSYS adds some weak spring to prevent a "divide by zero" error, and lets the solution continue. Usually contact is established and strong contact forces come into play. The contact forces are much larger than the weak springs, so the weak springs become negligible in the final solution, but they were needed to get the solution past the "divide by zero" problem at the beginning. You can check the reaction forces in the weak springs to verify that they are not significant. You can also make sure there is a tiny bit in penetration in the contact at the beginning, then weak springs will not be needed.
The ANSYS 19.0 2D Plane Strain model is attached.