So, it does not matter if you use time or substeps. Also, steps are to break the load conveniently for loading purposes, and substeps is used to break that step into smaller substeps. You do not need 20 steps. You just need 1 if you wish all loads to ramp up over that first step. Do make sure your pressure is ramping from zero at time zero to max at time = 1.0 (end of load step 1)
I would start with 200 substeps, min 10, max 2000.
In meshing, I would set the physics preference to nonlinear mechanical. One of the biggest issues is the elements are poorly shaped to begin with, so a little bit of deformation and they become ill-shaped and the solver can not solve with them.
You may wish to try a more uniform mesh, but turning off adaptive sizing.
Have you tried just testing the stability of the material? You can take a cube of the material and deform it in various modes of deformation to see that it is behaving numerically stable. This is helpful to debug material model issues.
I have seen users put values from papers into Ansys in wrong units, so please double-check this.
Also before you run, you go to Analysis Settings> Identify Element Violations and set to 1. After you run the model and it does not solve, under solution information, it will have some objects that indicate which elements are becoming highly distorted. You can share images of the elements and where they are located. By improving the mesh, you can sometimes go further.
If the deformations expected are very large, then the model may need to use nonlinear adaptive remeshing (NLAD).
Please try these recommendations first. Thank you!