[cstebbings]

I am trying to simulate an air and steam mixture being blown into a room with CFX 14.5.7. The steam has water droplets in it. So it's a 2 phase and multi component problem. The room has 2 outlets. The mixture is coming in at 125 ft/s. The room is 50ft x 10 ft. The ultimate goal is to look at the relative humdity on some cabinet surfaces in the room. I have one domain. I have used the setup from tutorial 31 (steam jet) whereby you create 2 subdomains to capture the liquid to gas and gas to liquid. I tried a run where the mesh count was 12M and the run died on the 2nd iteration with no message. My time step was 1e-5. I have tried 1e-6 and e-7 timesteps and they die on the 1st iteration. I then made the mesh finer (24M) and I can get it to run with 1e-5 but then when I try to change it to 1e-4 it dies. Not sure why the mesh size was imapcting it so much. I did another case with a real coarse mesh (100K) and it ran with a timestep of 1e-5.

[ghorrocks]

It looks like your simulation is highly numerically unstable, so convergence is sensitive to some things it should not normally be sensitive to. I would recommend, in order of importance:

1) You check that the physics is correct. No point continuing if you are specifying something which missed an important piece of physics
2) Mesh quality - everything is easier with a better mesh. If you have a rectangular room you can hopefully make a mesh which is very high quality hexs.
3) Double precision
4) Small time steps
5) Use a better initial condition

[cstebbings]

Thanks. I appreciate the response.

[cstebbings]

Also as a follow up - do you have any recommendations about the size of the mesh elements? I tried a run with 12.9M elements with no success and then a run with 29M elements with partial success. It's not clear to me yet if I really need the smaller element size to capture all that I have here namely 2 phase, 2 component and buoynacy. Would you agree that there could be a threshold of element size whereby a smaller mesh would be needed to capture all this? What kind of size are we talking about?

[ghorrocks]

Finer meshes are less numerically stable than coarse ones. So I would expect you will get divergence problems as you refine the mesh. So I would do all the development on coarse meshes, and once that is working reliably you refine the mesh and do a mesh sensitivity study to determine the mesh you need.

There are some cases when a coarse mesh cannot resolve a fundamental flow feature so you either get divergence or a totally unrealistic result - you will have to use your judgement to determine whether this is the case. But this is rare, most of the time a coarse mesh will converge easily and have a result which is generally correct but the actual quantitative values could have significant error.

Final: please do not PM me to tell me you have a question on the forum. If it is on the CFX forum I will see it. Please leave PM for messages which are actually private.

[cstebbings]

In the end it ended up being a bad partition. I was trying to run on 8 cpus. I made a change and ran it on 5 cpus by which you get a different partition. it ran fine. this was the only change. So the previous partition must have been in a bad/sensitive location.