peteroznewman
Subscriber

Use smaller elements around the two circled areas of the rubber part.

Mesh the rubber part with Linear elements, not Quadratic.

Add a small radius to the edge of the steel part and have frictional contact between the radius and the rubber face in the area circled in red.
Is the flat steel ring bonded to the rubber or is there frictional contact?

Use a Hyperelastic material model such as Neo Hookean, rather than a Linear Elastic material model.

While the above may solve the highly distorted element issue, other problems may arise such as convergence failure in a Static Structural model. This is because after the seal reaches the tip of the steel protrusion, it will have a lot of strain energy and will want to snap past the tip. That is a dynamic event which can’t easily be captured in a Static Structural model. There is no static equilibrium just a tiny bit past the tip of the protrusion. This could be overcome by solving in Transient Structural. There are some tricks that can be played in a Static Structrual model to temporarily switch to an explicit dynamics solver to get past the dynamic event.

The other issue is that you are enforcing axisymmetric response, but if you modeled this in 3D, you might find the rubber cylinder buckles into a non-round shape.

If you want to share your model, use File Archive and put the .wbpz file on a File Sharing site such as Google Drive or OneDrive and paste the link to the file in your reply and say what version of Ansys you are using. Members like me will be able to look at your model, but ANSYS Staff are not permitted to download files, so you can only get their help if you post details in your reply of the error messages.