parallel run for conjugateHeatFoam
 

Dear all,

I wish to run a parallel case with conjugateHeatFoam (OF-1.5-dev), but neither 'decomposePar' nor a manually decomposition works.

Does anyone have some experience or suggestions on it?

I would really appreciate some help....

Elisabet

Hi,

Please elaborate exactly what problems are you facing? Have you made the file decomposeparDict? What error message do you get on running decomposePar?

Ok, I've taken a very simple case of a square channel aligned with x axis and two solid walls (at y+ and y- locations). Fluid domain is defined at the main folder and corresponds to region0, while solid domain is linked and located at '0', 'constant' and 'system' folders under the name 'solid', as defined in the tutorial example.

The case runs perfectly without parallelisation.

In order to run the case in parallel, I first tried with the definition of the decomposeParDict at the main 'system' folder and run 'decomposePar', following the classical procedure in other solvers. However, an error was found. The output is rewritten here:

Hope it helps to understand the problem....

elisabet

Oh, by the way, I decompose the domain in 2 subdomains along x axis.

Hi

By reading this message

"request for polyMesh solid from objectRegistry conjugateHeat_parallel failed
available objects of type polyMesh are"

it seems to me that decomposePar is unable to split your solid region over two processors. As it can work only with mesh your solid region is coming in way.

I have never tried parallelisation of regions with solid boundary before and this is what I have understood based upon my understanding of decompoPar. Try searching this forum for ways to split meshes with solid regions or try splitting your mesh in such a way that solid region doesn't get split.

I've tried both things, without success.... that's why I decided to start a new threat.

When I split the domain avoiding to interact with the solid subdomain, 'decomposePar' provides the same error as before.

Any idea?

elisabet

it is possible but a lot of handish work
 

Hi,

According to this thread http://hi.baidu.com/awacsljt/blog/it...4e6113aaf.html it is possible. And I just tried it myself and it works.

Make also sure to use the harmonic scheme for the laplacian on the fluid side as mentioned in this thread: http://www.cfd-online.com/Forums/ope...penfoam-8.html

Otherwise there also exist explicit coupling through the boundary chtXXXXMultiRegionFoam.

Jens

Hi Jens,

First of all thank you for the hints.

I finally sorted out how to deal with parallel runs: it was so obvious.... but I didn't thought on it.... one just need to use the -region option with decomposePar !!!!

So, the required steps are (within the structure of the conjugateHeatFoam tutorial case):

1. First change the boundary file in order to avoid the 'regionCouple' type (just write 'patch' instead of 'regionCouple', for example). This step has to be done in the main 'polyMesh' folder and the solid one.
2. Modify the initial map accordingly for both main region (region0) and others (solid). For example, modifying 'regionCoupling' by 'fixedValue'.
3. Define 'decomposeParDict' for the main 'system' folder and the solid one.
4. Run 'decomposePar' and 'decomposePar -region solid'
5. Correct 'boundary' files and initial maps for all processors, including main domain and solid domain.
6. Run in parallel as usual: 'mpirun -np # conjugateHeatFoam -parallel > log &' (where # are the number of processors)
7. In order to reconstruct the meshes run 'reconstructPar' and 'reconstructPar -region solid'
8. In order to visualize: 'foamToVTK' and 'foamToVTK -region solid' and, execute 'paraview'. Load both cases and click on 'group Datasets' in 'filter' menu.

Hope it helps!!!!


By the way:
It is still not clear to me in which Laplacian should I use 'harmonic' scheme (among the ones for the fluid region). In the ones that include a couple patch or just the opposite ones?

Thanks!


Elisabet

Hi Elisabet,

i don't get you question, but maybe this makes it clear:

according to http://www.cfd-online.com/Forums/ope...penfoam-8.html
you need to set the laplacian scheme in fvSchemes for the energy equation. Otherwise the temperature gradient at the coupled boundary will be wrong.

laplacianSchemes
{
laplacian(DT,T) Gauss harmonic corrected;
}

Jens

Hi Jens,

Thanks for the answer. It's everything clear now.

Sorry if I was not very explicit in my question. I call uncoupled variables those that need to be solved in a single domain (velocity and pressure) and coupled ones those that have to be solved with coupled domains (temperature for conjugateHeatFoam).

Thank you very much!!

elisabet

Hi Elisabet,

Did you have luck with you parallel setup?

The reason I am asking:
-fluid (region0) decomposed and solid UNdecomposed runs fine with some speedup,
-fluid (region0) decomposed and solid decomposed gives me an error as soon as the energy equation (T+T) gets solved.

So I think it is because of the region coupling (e.g. attach detach)? But I don't know - maybe Hrv knows?

Jens

Hi Jens,

I definitely had luck with my parallel simulation. At least, until now....

From my experience, this first option is not right enough, at least for my case: I have a square fluid channel with the top and bottom walls. I don't really remember now which was the problem, but the obtained temperature field looked non-physical.


I'm sure Hrv can provide much more information than me, but try to attach/detach the solid domain in the same manner as the fluid domain (see attach/detachPatches.H in the source folder), as suggested in: http://www.cfd-online.com/Forums/openfoam-solving/57892-integrated-conjugate-heat-transfer-solver-openfoam-3.html#post179753

I guess this is the unique (relevant) code modification I've done.

Hope it helps!

elisabet

Since I use the OF-1.6.ext version the "bug" (which is http://www.cfd-online.com/Forums/ope...tml#post179753) was already gone. However I know where the code breaks right here:

in solveEnergy.H

So I guess I need to digg further, maybe Hrv can push me further?

Jens

Hi

I am trying to decompose the domain 2 rectangular domains, the first one is fluid an the second one is a rectangular solid domain immersed in the fluid, centered, this solid domain occupies 1/2 of the fluid domain in both directions, I decomposed the domain in the same number of processors, but unfortunately the boundaries do not match in the same the regionCoupling for solid and liquid do not match for some of the processors,

Should I decompose both domains in different numbers of processors, in such a way that boundaries match?

Any help is welcome,

Thank you

Alberto

decomposePar in parallel
 

Hi Alberto,

Since now, when I need to decompose a case with more than one domain, I must move to version 1.7.x to correctly decompose the case (with -region option, of course). Afterwards, I can return to my version (based on 1.6-ext) and run the case. I have experienced no problems with reconstruct tool.

The error obtained when I decomposed the main case with OF-1.6-ext was something about a missing region, as far as I remember.

I would appreciate to know other alternatives, if someone has experience on it!!!

regards,

elisabet

Hello Foamers

I am trying to use decomposePar for the geometry sketched below, fluid domain with a solid domain which length is a third of the liquid length, until now I can only run conjugateHeatFoam solver using 2 processor for the liquid and 2 for the solid (x-direction), is there a way to use at least 6 for the liquid and 2 for the solid, I have found the instruction



globalFaceZones ( nameofzone1 nameofzone2 );

but I do not know how it works or if it is useful for my problem,

Please let me know your opinion about this problem

Any help is welcome.

Thanks in advance.

Alberto

the step 7 is wrong!
 

when I run reconstructPar, there is a same error as decomposePar,like "Attempt to cast type wall to type lduInterface"