chtMultiRegionSimpleFoam
Dear All,
I am trying to run chtMultiRegionSimpleFoam. I have prepared a case with 1 fluid region and 6 solid regions. I have set my case and when I lauch it, I get this error: Code:
Adding to radiations I can not understand what it means. Could you help, please? Thanks a lot, Samuele |
Hi Samuele,
Can you attach the boundary conditions for the "pcm" region, as well as any regions that are in touch with it? Although, if I have to guess, I think that this sentence: Code:
Attempt to cast type zeroGradient to type compressible::turbulentTemperatureCoupledBaffleMixed Best regards, Bruno |
1 Attachment(s)
Dear Bruno,
thanks for answering, first. Also, about your suggestions, I completely agree. The point is that I chacked the boundary conditions twice and I can't find any error. I am attaching to this email all the changeLogDictionary I use. Could you kindly have a look and let me know what's wrong with it? Thanks a lot, Samuele |
Dear Samuele,
it seems that you put this B.C for a patch in a region (compressible::turbulentTemperatureCoupledBaffleMi xed). then you put zeroGradient to the same patch in the other region which is not applicable. the B.C must be the same for same patch in different regions. hope it helps. BR, |
I will check it again, then.
Thanks a lot, Samuele |
I have found a first error: I haven't set the right BC in the fluid region.
I ran my case and I get a different error: could you help in solving this, too? Thanks a lot, Samuele The error message is: Code:
/*---------------------------------------------------------------------------*\ |
Dear Samuele,
this error always appears when there is a problem with three factors: cell size, time step, velocity value. you must compromise the three factors to get smooth run. hint: adjust dimensions and cell size such that patches boundaries lays on cells boundaries not in middle of it. hope it helps, Best Regards, Ahmed |
Do you mean that it could be necessary to remesh my geometry?
|
no i don't mean so, i only drag your attention to revise it, but you can change your velocity value, or time step. you can go back to the user manual to know how to set time step.
|
I think that being a steady simulation, the time-step does not influence the solution: is this right?
|
Greetings to all!
@Samuele: Quote:
The unusual example might be LTSInterFoam: http://www.openfoam.org/version2.0.0/steady-vof.php Quote:
Code:
checkMesh -allGeometry -allTopology Bruno |
Dear Bruno,
thanks for answering and pardon for the late reply. This is the output of the command you suggested: Code:
zampini@pc-zampini:~/Documenti/personali/Epta/SCC/steady$ checkMesh -allGeometry -allTopology |
Hi Samuele,
Quote:
paraFoam provides you with the ability to also see the sets. Turn on that option and choose to see "underdeterminedCells" that should appear in the same list as the patches. Then try to see where exactly where the problem cells are and try to re-do your mesh. Another possibility is to follow the example shown here: http://openfoamwiki.net/index.php/SetSet#Usage_example - more specifically, to only remove the cells associated to "underdeterminedCells". But keep in mind that this kind of cell removal strategy has certain limitations, such as possibly and wrongly removing some important cells. Best regards, Bruno |
1 Attachment(s)
Dear Bruno,
I am attaching a picture of the whole volume where it is evident where the underdeterminedCells are. I can't understand what's wrong with them. Do you have any idea? First of all, I will try your suggestions. Thanks a lot, Samuele |
Dear Bruno, Dear All,
after having re-meshed my geometry, I get a very strange result. First of all, all the mesh checks are ok! Hance I thought that my simulation would have started immediately, but.. ..but I got this error: Code:
lab@lab-laptop:~/Documenti/Ethics/FRISBEE/CFD/SCC/steady$ chtMultiRegionSimpleFoam And this happens for each region. Do you have any idea? Could you help? |
Hi Samuele,
There seems to be a problem with a patch that is defined to be a symmetry plane: Quote:
Best regards, Bruno |
Here is the case: https://www.dropbox.com/sh/tgdwuqkfodgdffk/zFNdkvUgjH
Could you have a look? Thanks a lot, Samuele |
Code:
Solving for solid region packs_2 Code:
this error always appears when there is a problem with three factors: cell size, time step, velocity value. you must compromise the three factors to get smooth run. If I am right you have a Problem in the Boundary Conditions of T in packs_2 or in your fluid Region. Maybe your boundary file is wrong (patch type). Maybe you have no value set.? Your mesh seems okay. Regards Tobi |
Dear Tobi,
thanks for answering. Actually, I have solved this very problem (it was due to a bad definition of the boudary conditions) and the simulation's running. However, the temperature seems to be meaningless: I do have a max temperature of about 740000 K. Too much, I say. I am going to check this problem, too. Any idea to begin to investigate the issue? Thanks a lot, Samuele. |
Hi,
write out the first 10 or 20 integrations and have a look at your Domain. You will be able to see the regions where you get the high temperature values. It could be possible that this Problem occure due to a mesh Problem. otherwise you see if your BC are incorrect or your Settings are wrong. Good luck |
All times are GMT -4. The time now is 23:32. |