What to do about this warning?
 

During my simulation, after every iteration, I get this warning:

The number of cells changes each time. It goes up and down. One iteration it was as high as 1,500 cells. There was a jump up in the energy and z-momentum residuals that iteration. What exactly does this warning mean and do I need to worry about it or take action to fix the problem? I can't find info about it in the starccm+ manual or online.

FYI, I'm using a segregated flow and segregated energy solution.

Typically this means you have some bad cells in your mesh. Create a cell set to visualize these:

Go to Representations->Volume Mesh->Right click on Cell Sets->New->Threshold->Set it to Temperature -> hit Query.

you are wanting to find if they are min temps or max temps. Depending on that, create a min or max threshold and type a number below the value. You can then highlight this cell set in a scene to visualize

I took your advice. It is a max temp problem. I have temperatures up to 1500 K. I set a threshold of 700 K. The problem cells are all in a part of the geometry where two surfaces get very close together and contact each other, causing a region that probably has very low flow. Here's a 3D representation of the problem region with the max temp cells shown in pink:

http://i898.photobucket.com/albums/a...1/max_temp.png

Here's the same shot from above the region with the mesh shown. Note that the solid curved surface running across the top of the picture is the heated surface. The other curved surface going across the bottom that meets up with the top surface is not heated.

http://i898.photobucket.com/albums/a..._temp_grid.png

Here's the same picture of the mesh with the max temp cells highlighted in pink:

http://i898.photobucket.com/albums/a...emp_w_grid.png

Can you advise me what to do about this problem? If the solution is to make a new mesh, what should the mesh look like in those tight regions? What kind of settings do I need to use for the prism mesher or trim mesher to acheive a good mesh in those regions?

Well, to get the prism layer to work better in there I would try:

1) try setting your near wall boundary layer a bit smaller (i.e. add more layers, or change stretching raito). The more layers it has, the easier it is for it to chop off. I.e. if you had a prism layer with 2 equally spaced, you have to chop off 50% at a time. If you had same thickness but with 10 layers, you can remove in 10% increments.

then
All under Continuum->Mesh->Models->Prism Layer Mesher
2) Set minimum thickness percentage to a really low value. 1% may be a good starting place, but you can go to .1 I believe.
3) Set layer reduction percentage to high value. 95% is agood starting place, but you can go up to 99%

So, you're saying that I want to get the prism layers thinner so that I can get them further into that crevice? My original thinking was that I should try and just get one big cell to take care of that whole crevice region because I didn't think it was that important what was going on in that one spot. Plus, I was worried about computational resources, which are already stretched thin. The case that I just showed you took 9 hours to run 130 iterations using 30 cores. Cases I ran using coarser meshes took 4000 iterations to converge. Granted, I initialized this refined mesh case to the solution of the coarse mesh case to try and speed up the solution, but the residuals, velocities, and temperatures are pretty much all over the place at 130 iterations so I'm assuming this is still going to take a lot more iterations, if it does converge at all.

Well, I have had issues with poor solutions in geometry similar to this that were fixed by getting my prism into the crevice.

If you are wanting to avoid global prism changes, maybe try separating out the feature curve defining that gap and setting a smaller mesh size on it? This would create a finer mesh only in that region.

If you are trying to avoid increasing the mesh size at all, you might try modifying the gemoetry slightly to get rid of that gap. I.e. fill it across with a flat face. If there is little flow in the region, it shouldnt affect the solution too much.

I'm thinking about this problem a little more. You said the problem is either min or max temps, but I didn't get any warnings about the temperature being limited by the min or max limits like I did in previous runs. And, even though the max temp in my mesh was 1500 K, the max limit set under 'physics' is 5000 K. So it seems to me like the 'temperature correction' which is being limited is something different. I checked the coarse mesh case that I told you about and that only gave me seldom errors about the temperature correction being limited and only in one cell; however, that coarse mesh had the same problems with high fluid temperatures in those tight crevices as I saw in the refined mesh. And that still converged. Are these high temperatures in those spots a problem?

Either way, I think I'll give it a try to get the prism layer into the crevice to see if I still get the warnings or not. Thanks for your suggestions.

Cells having a sharp edge like yours are usually bad. It's better to cut the cells so the triangular cross sectional shape becomes a trapezoid.

Unfortunately, I don't think I'll have the time to re-mesh and run again because if I'm going to get results from this case, I need to get them very soon, so I'll just see where this case goes. I will keep your tips in mind though for when I generate new meshes and keep an eye on the angles of those prism layers and cells in those tight crevices. To update, I have now run for about 320 iterations and the residuals are looking good. The velocities and temperatures seem to be settling down to more consistent values with respect to the iteration count. Also, I'm getting much less of these 'temperature correction limited' warnings. I'm getting warnings for about 50 cells every iteration as compared to 300-400 cells at the beginning of the simulation.