How come that my steady-state simulation converges and gives good results but the same mesh does not seem to be sufficient when I turn it into a steady-state FSI Two-Way simulation? The fluid part of the solver does not even reach the 10th accumulated time step altough I use same physical timestep as before.

Hi,

Are you sure the motion is correctly modelled? If the motion is rapid then the mesh motion will cause convergence difficulties.

Glenn Horrocks

Hi,

I have run simple but similar problems. I deal with Mach Numbers at about 7 and it all worked fine when the mesh of fluid and solid domain was coarse and simple.

Now I have made it quite complex and maybe solid and fluid domain mesh are slightly overlapping. Can this be a problem?

I also have problems with negative volumes now although the mesh of the fluid domain had no problems when I just did a CFD run.

Hi,

Well that will be your problem. If your mesh is getting negative volume elements then even before then the element quality will be terrible and high mach number flows and poor mesh quality will often lead to convergence problems. You will need to be a bit smarter about your mesh motion. Have a look at the mesh motion weighting functions.

Also have a look at V12 beta as that has lots of remeshing stuff so (I believe, I have not done it) you can monitor mesh quality and trigger a remesh when the quality exceeds a certain value. This type of approach may be useful for you.

Glenn Horrocks

Yes. The negative volume appears at elements with very poor quality. I have just checked. When I did a run without FSI with the same mesh it worked. Anyhow: Are there any certain restrictions concerning the mesh of the fluid and solid domain?

Like the nodes have to match between solid and fluid? Or is that independant? Any other things to keep in mind?

By the way: How can I open a mesh file in ANSYS Workbench (Simulation) I created with ANSYS ICEM?

Hi Abduri, try reducing Model Exponent for the mesh stiffness model. You can choose either "increase near small volumes" or "increase near boundary" , it doesn't affect much. Try 1 ro the model Exponent. If you look in the CFX manual, you will see the equation showing that if the gradient of the mesh stiffness will be higher when you use high value of model exponent(1 to 10). Imagine you have two adjacent elements, high gradient of mesh stiffness makes one element very stiff compare to the other. This might cause folded mesh in your domain. I normally use 1 but I think in some cases other values may allow larger deformation.

Pat

Thank you!! It helped a lot!

Cheers