Hello Henrique,

Thank you for the details! 

I have built O-ring seal models to determine if the O-ring will succeed in making a seal. The seal works if the contact pressure of the O-ring is greater than the fluid pressure. Otherwise, the fluid pressure would penetrate the seal. The contact pressure ends where the seal ends, and that appears to be where you ended the fluid pressure, so it looks like you have made a reasonable idealization.

The M30 threads have radial clearance and the contact face on the thread has a 30 degree angle relative to the X axis (which is vertical in these screen shots). A more accurate model would be to include the thread geometry.  A simplified boundary could be to use a Displacement of Y=0 and leave X=Free so that radial deformation can occur. Once the model converges, you can see if this makes a better boundary condition than a Fixed Support. 

It sometimes helps the solver converge if, under Analysis Settings, you turn on Auto Time Stepping and change the Maximum Substeps to a large number like 2000.  It will only use them if it needs to, but if you limit it to a small number, convergence may fail. In your case, it didn't need that, but it is a best practice to do this.

You created a good quality mesh. I opened your model on a computer with the Ansys Student license installed, so I can't solve your model with the mesh you created as it exceeds the student node count limit of 128,000 nodes.  I changed the Element Order from Program Controlled to Linear and the node count went down to 43,000 nodes.

To diagnose why convergence fails, click on the Solution Information folder and type a 3 for the Newton-Raphson Residuals and type a 3 for Identify Element Violations.  When convergence fails, first look at the Solution ouput and scroll to the bottom to find the first ERROR.  In this case it says a highly distorted element.

Click on the HDST_Elements plot to see where the highly distorted elements are located.

During the solution, the shape became worse.

The corrective action is to make a better quality element shape in the mesh before solving. I made much larger elements and made sure the inflation layer had layers that would cover the region of concern.

Now the model converges.

If you add the thread geometry back on the plug and include frictional contact with the female threads on the part with the hole in it, you will see the stress in the threads be distributed over several threads and the stress concentration from the Fixed Support will be reduced.