parallel decomposition method in openfoam
 

Hi All,

In openfoam, the hierarchical method to split the computational domain gives the options to specify the order, e.g. xyz, does anybody know how this order affects the simulation results? Thanks.

Hi Hz283,

It could influence the simulation time, but that's basically it. It certainly does not affect the simulation results. At least it should not, else there is something wrong with the code.

Cheers,

L

Hi Lieven,

Thank you very much. Could you please say more about how it can affect the simulation time?

Thanks.

Sorry, not an expert in that field so I can't give you an exact answer to that.

Cheers,

L

Hi,

as far as I know, a general answer cannot be given. This substantially depends on your computational grid. Try to spread the work evenly on all processors/ cores. At the same time try to minimize the the interfaces of the mesh parts to reduce the communication between the nodes.

cutter

Thank you very much for your suggestions. About the method hierarchical, I found that we can change the order of xyz to yzx or zyx and so on. I was wondering in which case I need to do this. Is this helpful to improve the computational efficiency?

Maybe the best way for me is to directly test the case with different partition method. But my case is a little large. So can I try get some suggestions from you before using this method?

Thank you in advance!
h

Dear hz283
1) In my experience, one of the parameters that can affect your parallel simulation is the delta parameter which is equal to 0.001 by default. But if you have a mesh with faces of highly skewed cells you should increase this value to e.g. 0.01. you can find your cell skewness by running the following command in Terminal:
I remember that I had a simulation which worked just fine in a single processor but after decomposePar on several processors it would diverge (the courant number became very large). after increasing this delta parameter, it worked fine.
see the following post for more info:
http://www.cfd-online.com/Forums/ope...tml#post447958

2) Also there is another thing that you should notice. use the complex methods for decomposePar only if you have a complex mesh. but if you have a simple mesh, use the simpler methods. I have a experience in this field that by using complex methods (such as scotch) for my complex mesh (film cooling of turbine blades), my run time reduced to 1/3.
but by using scotch method for a simple mesh (flow around a cube) neither my run time nor the results did not change significantly in comparison with the simple method.
Summary: use complex methods for decomposePar only for complex meshes.
Also see the following post:
http://www.cfd-online.com/Forums/ope...-ptscotch.html

3) And finally about your 1st question:
I have not worked with hierarchical method and I don't know how to choose the order of xyz to yzx or zyx. but it definitely depends on your geometry.
Please share your experiences with hierarchical method in here.

Thank you so much for your so detailed reply. Besides, I found that the metis and scotch methods are intensively discussed in this forum. Most people think scotch is good. But I use OF211 and found that there is not such method. What kind of version are you using?

Thanks.

Are you sure?
https://github.com/OpenFOAM/OpenFOAM...llel/decompose

Ah, Thanks!!

I only saw the option in the file system/decompose, in which only three options. Could you please share me one of this file in your case? Thank you a million!

Hi cfdonline2mohsen,

About the metis coefficients, if all the cores are totally the same, the coefficients for all the cores are only needed to be set to 1? Any comments about this point? Thank you very much!

I don't recommend the metis method because if you review the cfd-online posts, most of them stated that metis has some restrictions about licensing problems.
It was just a recommendation. Search more about this matter.
I've used the scotch method with the same coefficients that exist in OpenFOAM tutorials.

Hello cfdonline2mohsen,

I have read the comments, but I am still facing an issue for my complex mesh (by using scotch), when I am running the decomposePar (after running the blockMesh and checking if everything is fine). I have to admit that I changed the size cells in blockMesh, but still the same error. The same errors occur with other methods, for example, hierarchical. I am facing the following error:

--> FOAM FATAL IO ERROR:
size 65662 is not equal to the given value of 250000

file: /.../MyCase_!/0/Co from line 18 to line 65708.

From function Foam::Field<Type>::Field(const Foam::word&, const Foam::dictionary&, Foam::label) [with Type = double; Foam::label = int]
in file /home/ubuntu/OpenFOAM/OpenFOAM-8/src/OpenFOAM/lnInclude/Field.C at line 213.

FOAM exiting


Here's my decomposeParDict:

numberOfSubdomains 16;

method scotch;

Any solution to this or opinions?

Your Co field is likely left over from a previous simulation and after you generate a new mesh with blockMesh there is no reason to believe that this field is still valid (ie, correct size, number and size of boundaries). The error message is correct.

Licensing for metis has evolved of the years. It is no longer an issue. ParMetis still has some restrictions.
I did some tests a while back (2018 perhaps) to compare the min/max/avg number of neighbours between domains since this is a reasonably good metric for the decomposition quality and gives an idea of how well balanced the decomposition is. Metis did surprising well and was consistent. Scotch was quite similar, but you can hit some oddities very occasionally where the decomposition is just a bit 'weird' - probably related to the initial seeding. Kahip was also very similar but without the scotch oddness.
To quickly test things, use 'decomposePar -dry-run -cellDist'. This will perform the decomposition internally (does not create processor directories) obtain some statistics and then write out the distribution as a serial field, which you can visualize in paraview. If you want a bit more insight, compile the application/test/decomposePar. This creates a Test-decomposePar that let's you specify method and number of domains as command line options and also provides some better statistics. Use this to conviently (and quickly) test different approaches.