
[Sponsors] 
January 28, 2011, 13:18 

#21 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Hi Bruno,
Thanks for all your help. I figured out that the problem is because of the way OpneMPI behaves: "Unless otherwise specified, Open MPI will greedily use all TCP networks that it can find and try to connect to all peers upon demand (i.e., Open MPI does not open sockets to all of its MPI peers during MPI_INIT  see this FAQ entry for more details). Hence, if you want MPI jobs to not use specific TCP networks  or not use any TCP networks at all  then you need to tell Open MPI." When using MPI_reduce, the OpenMPI was trying to establish TCP through a different interface. The problem is solved if the following command is used: mpirun mca btl_tcp_if_exclude lo,virbr0 hostfile machines np 2 /home/rphull/OpenFOAM/OpenFOAM1.6/bin/foamExec interFoam parallel The above command will restrict MPI to use certain networks (lo, vibro in this case). 

January 28, 2011, 15:23 

#22 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122 
Hi pkr,
Congratulations! It would have taken me a while longer suspect that this would be the case I still only had the notion that something was fishy about the network or how things were connecting to each other. And thank you for sharing the solution! I guess this is one of those details that either comes from experience or from a dedicated MPI course! Best regards, Bruno
__________________


February 4, 2011, 13:40 

#23 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Hi Bruno,
I am would like to use scotch partitioning instead of metis. Please suggest a way to enable scotch partitioning in OpenFoam1.6. Thanks. 

February 4, 2011, 18:42 

#24 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122 
Hi Pkr,
I just tested to confirm it... it's as simple as editing the file "system/decomposeParDict" and setting the method like this: Code:
method scotch; Bruno
__________________


February 23, 2011, 23:54 

#25 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Bruno,
I have couple on questions on decompositions. On running decomposePar utiluty, the mesh gets decomposed into processor* directories. Each processor directory contains points, cells and neighbors on which the process works upon. As with the OpenFoam solver, we are trying to solve the equation Ax=b.So i have folowing queries: 1. Where in the code the processor* directories get converted to matrice A, vector x and b? 2. Now each processor will compute matrixvector product Ax on the set of data it works upon. After each multiplication the processor exchanges boundary elements with the neighbors and somehow updates the matrixvector product to rectify its own result? How does this update works? 3. How does working on small matrices by each processor equivalent to work on the complete matrix? I mean none of the processor gets the complete Matrix vector product at any time. Let me know if you have same idea on the same. Thanks 

February 24, 2011, 18:59 

#26 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122 
Hi Pkr,
Sadly I don't know how OpenFOAM does the Ax=b in parallel. But if I needed to find out, I would start looking for which solvers/functions/methods call upon the methods made available in "libPstream.so"! The source code for Pstream is in the folder "$WM_PROJECT_DIR/src/Pstream/mpi". It has the methods used for communicating between processors. If you trace back who calls these methods, you should be able to figure out how OpenFOAM does the matrix operations! The other keywords to keep an eye out for are the classes/methods related to the preconditioners and respective matrix solvers that we usually define in fvSolution. Good luck! Bruno
__________________


February 24, 2011, 22:24 

#27 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Bruno, Thanks for your response. Another query:
If the mesh is already decomposed among 4 processors. After decomposition, Is there a way where one of the processor transfer some of it's cells/points/faces to another processor at runtime. I am looking for some kind of join and split operation. Thanks 

February 24, 2011, 22:52 

#28  
Senior Member
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 399
Rep Power: 20 
Quote:
1. The processor directories only contain subdomains of the mesh after partitioning. Parallelisation is actually done at the lduMatrix level. 2. If you really want to see the exchange process in action, take a look at the lduMatrix class: ($FOAM_SRC)/OpenFOAM/matrices/lduMatrix/lduMatrix/lduMatrixUpdateMatrixInterfaces.C There's are (init/update)MatrixInterfaces member functions that do what you're looking for. 3. You're right  each processor does only its bit of the matrix multiply. The rest is handled through information exchange across processor boundaries. Most Krylov solvers require some form of global dotproduct reduction, but besides that, this is essentially the meatandpotatoes of it. Hope this helps. 

February 24, 2011, 23:15 

#29 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Thanks for your response Sandeep.
It seems that each process solves it's own part of Ax=b. Whre A, x and b are formulated by a subdomains of mesh in Processor* directories. Can you explain further what do you mean by parallelization at lduMatrix level? Talking about exchange of messages across the interface, I don't understand why is the following operation performed: void processorFvPatchField<scalar>::updateInterfaceMatr ix(...) const { scalarField pnf ( procPatch_.compressedReceive<scalar>(commsType, this>size())() ); const unallocLabelList& faceCells = patch().faceCells(); forAll(faceCells, facei) { result[faceCells[facei]] = coeffs[facei]*pnf[facei]; } } What's the need of subtracting coeff[]*pnf[] from matrixvector product result[]. How does it fix the result after being partitioned? Again, How does splitting of a big mesh into smaller meshes where each smaller mesh is solved for Ax=b gives the global solution for the complete large mesh. Thanks. 

February 25, 2011, 05:19 

#30  
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122 
Hi pkr,
Quote:
Best regards, Bruno
__________________


February 25, 2011, 07:58 

#31  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 914
Rep Power: 24 
Quote:
This is my guess, lets say you spit the main matrix into two parts A = A_local + A_parallel. Now A_Parallel has the matrix coefficients for neighbours on other processors. To solve Ax = b, you would have to write it like this: A_local x = b  A_parallel . x_old This why that vector is subtracting the product of coeff with boundary values. This is just a guess though.  Another guess is that Matrix is stored as Ap phi_p = Sum( Al phi_l ) + b In this case for vector matrix product you would have to subtract rather than add. 

February 27, 2011, 18:39 
Some basic doubts

#32 
Member
Join Date: Nov 2010
Posts: 33
Rep Power: 11 
Dear Bruno,
I have some basic doubts in the working of interFoam/dambreak case: 1. What difference does it make case if the following changes are made in controlDict: Start time: 0 end time : 1 Changed to start time: 0 end time: 0.25 I understand that it reduces the simulation time, but what happens to the quality/correctness of the results? 2.What equation is interFoam/dambreak actually solving? From the code in pEqn.H: Code:
{ volScalarField rUA = 1.0/UEqn.A(); surfaceScalarField rUAf = fvc::interpolate(rUA); U = rUA*UEqn.H(); surfaceScalarField phiU ( "phiU", (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rUA, rho, U, phi) ); adjustPhi(phiU, U, p); phi = phiU + ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1)*mesh.magSf() + fvc::interpolate(rho)*(g & mesh.Sf()) )*rUAf; for(int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rUAf, p) == fvc::div(phi) ); pEqn.setReference(pRefCell, pRefValue); if (corr == nCorr1 && nonOrth == nNonOrthCorr) { pEqn.solve(mesh.solver(p.name() + "Final")); } else { pEqn.solve(mesh.solver(p.name())); } if (nonOrth == nNonOrthCorr) { phi = pEqn.flux(); } } U += rUA*fvc::reconstruct((phi  phiU)/rUAf); U.correctBoundaryConditions(); } 3. How does solving of some equation narrows down to PCG solver which solves the equation of the form Ax=b? Looking forward to hear from you. Thanks. 

February 27, 2011, 19:04 

#33  
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122 
Hi Pkr,
My experience in CFD is really limited, so I ask of arjun and deepsterblue or any other experienced OpenFOAM user to fill in the gaps of what I can't answer Quote:
This is different from, for example, icoFoam and simpleFoam, which are stationary solvers (again, not sure of the terminology); in these the time steps are related to the number of iterations made, with no temporal relevance. In interFoam, what affects the quality are other parameters, such as: maxCo, maxAlphaCo, maxDeltaT, "writeControl adjustableRunTime", deltaT. For more information about these, and the physics/equations behind this, read the OpenFOAM's User Guide in the section about the damBreak tutorial: http://www.openfoam.com/docs/user/damBreak.php or more specifically Time step control. As for the other questions, I don't know enough. Again I suggest you read section in the user guide for the damBreak; also check the fvSchemes file for the list of equations possibly used and the methods used to solve them. Also, check the rest of the code that interFoam uses, because it might still be using pieces of code from other header files that you didn't look into Best regards, Bruno
__________________


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
bc's of a komegaSST case  Zymon  OpenFOAM  11  July 25, 2010 10:36 
Paraview decomposed case without reconstructing?  HelloWorld  OpenFOAM  3  May 8, 2010 10:47 
Interfoam Droplet under shear test case  adona058  OpenFOAM Running, Solving & CFD  3  May 3, 2010 19:46 
ScaleUp Study in Parallel Processing with OpenFoam  sahm  OpenFOAM  10  April 26, 2010 18:37 
Turbulent Flat Plate Validation Case  Jonas Larsson  Main CFD Forum  0  April 2, 2004 11:25 