
[Sponsors] 
How to compute the integral in the parallel case 

LinkBack  Thread Tools  Search this Thread  Display Modes 
December 18, 2020, 14:25 
How to compute the integral in the parallel case

#1 
New Member
Saddam Hijazi
Join Date: May 2016
Posts: 12
Rep Power: 7 
Hi everybody, I have a question regarding the computation of integrals using fvc::domainIntegrate.
How can I compute the value of integrals over the different domains defined by the parallel decomposition ? For example, I run a case in parallel using 6 processors and I want to compute the following quantity, where Ufield is volVectorField for velocity. double A =fvc::domainIntegrate(Ufield & fvc::div(linearInterpolate(Ufield) & Ufield.mesh().Sf(), Ufield)).value(); when I then print the value of A using the following command std::cout << "A is " << A << " from " << "processor" + name(Pstream::myProcNo()) << endl; I get always  0.156 from processor 0  printed six times. This means that the integral is computed only over the first decomposed part of the domain. Ideally, I should be able to sum the values of A given by the computation of the integral across the six subdomains but I am not able to figure out how to do this. Could you help me in solving this issue ? Thank you very much, Saddam 

December 18, 2020, 15:22 

#2  
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,294
Rep Power: 31 
Quote:
Use Pout to see information on a perprocess basis. Eg, Code:
Pout<< "Hello from " << Pstream::myProcNo() << nl; Code:
scalar value = ...; reduce(value, sumOp<scalar>()); As a gentle hint, if you are working with OpenFOAM you will generally not use std:: cout for IO, but use OpenFOAMspecific ones. For stdout, it is "Info" which is more or less cout on the master process and /dev/null on all of the others. As soon as you start trying to print out a List or Field of values, you will notice that there are no operators for std ostream, but there are for the OpenFOAM Ostream. Also do not use "double" and "int", in OpenFOAM they are called "scalar" and "label". It may not seem important at the moment, but if you want code that will also compile with single or mixedprecision and/or 64bit labelling (for large meshes) it is better to use these OpenFOAM typedefs. 

December 18, 2020, 17:37 

#3  
New Member
Saddam Hijazi
Join Date: May 2016
Posts: 12
Rep Power: 7 
Quote:
Thank you very much Mark for your answer and helpful advice. I would like to write the line of codes that I modified according to what you have recommended: scalar value = fvc::domainIntegrate(L_U_SUPmodes[i] & fvc::div( linearInterpolate(L_U_SUPmodes[j]) & L_U_SUPmodes[j].mesh().Sf(), L_U_SUPmodes[k])).value(); reduce(value, sumOp<scalar>()); the last two lines are inside three nested loops which loop over i, j and k, and L_U_SUPmodes is a list of velocity vector fields. I printed the value of the scalar "value" by doing this: Pout<< "value from " << Pstream::myProcNo() << " is " << value << nl; I found it strange that the six values printed (I used six processors for the parallel run) are all the same and equal to 0.157144 so basically the reduce command just gives that value multiplied by the number of processors. It is worth mention that the correct value of the integral when the code is run in serial is totally different. Could you help me in identifying the source of this discrepancy. Thank you very much for your help, Saddam 

December 19, 2020, 10:35 

#4  
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,294
Rep Power: 31 
Quote:
After the global reduction, the value MUST be the same on all processors, anything else would be a bug. 

December 19, 2020, 11:20 

#5  
New Member
Saddam Hijazi
Join Date: May 2016
Posts: 12
Rep Power: 7 
Quote:
Ok I think I misunderstood the purpose of the reduce method. I thought that the integration will be carried out by each processor separately, which would have required a summation step of the values of the integrals. This is not the case according to what I understand from you. However, I still don't understand why the value of the integral computed in serial (which is the right one) differs from the one computed in parallel. Thank you very much for your help. 

December 19, 2020, 12:10 

#6 
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,294
Rep Power: 31 
I think that at this stage you need to write out what exactly you are doing. That is to say, if you are doing the reduce inside or outside of the loop etc. This might reveal some mismatch of concepts, and explain why you have a different value from the serial case. You say that the value is different than the serial case, but are not specific. Are they different by 12 %, different by 10 times, different by a factor equal to the number of processors? This all makes it incredibly difficult to provide anything remotely helpful.


December 19, 2020, 12:33 

#7  
New Member
Saddam Hijazi
Join Date: May 2016
Posts: 12
Rep Power: 7 
Quote:
I am sorry for not being clear. I will write the full method which basically computes a third order tensor (with the usage of c++ the library eigen) by looping over a list of volVectorFields (velocity fields) which is defined and read in the main of my application. Eigen::Tensor<double, 3> convectiveTensorParallel(label NUmodes, label NPmodes, label NSUPmodes) { label Csize = NUmodes + NSUPmodes + liftfield.size(); Eigen::Tensor<double, 3> C_tensor; C_tensor.resize(Csize, Csize, Csize); for (label i = 0; i < Csize; i++) { for (label j = 0; j < Csize; j++) { for (label k = 0; k < Csize; k++) { scalar value = fvc::domainIntegrate(L_U_SUPmodes[i] & fvc::div( linearInterpolate(L_U_SUPmodes[j]) & L_U_SUPmodes[j].mesh().Sf(), L_U_SUPmodes[k])).value(); reduce(value, sumOp<scalar>()); C_tensor(i,j,k) = value; } } } //if (Pstream:arRun()) //{ // reduce(C_tensor, sumOp<Eigen::Tensor<double, 3>>()); //} return C_tensor; } The important part is the one inside the nested loop, where I compute the value of the integral. The value of the integral for the first loop is 3.548312443e05 if computed in serial. In parallel I get the value 0.157144 for the integral and after the reduce command it becomes 0.9428640461 (I use six processors, this latter value is six times the earlier one) Note that Csize is equal also to the size of the list L_U_SUPmodes. Thank you very much. 

December 20, 2020, 17:06 

#8 
Member
Rodrigo
Join Date: Mar 2010
Posts: 94
Rep Power: 13 
What about splitting your code into simpler blocks that shall make your life easier when having to debug them? For instance, following lines should just work in a less cryptic manner:
Code:
// ... (after whatever update done for Ufield) //NOTE: useful when planning to interpolate it later... Ufield.correctBoundaryConditions(); //NOTE: nested just to ensure we don't mess up with your other variable names { const surfaceVectorField Ufield_f = linearInterpolate(Ufield); const surfaceScalarField phifield = Ufield_f & Ufield.mesh().Sf(); const volScalarField UdivU ( Ufield & fvc::div(phifield,"div(phifield)") ); //NOTE: "fvc::domainIntegrate()" is already parallel aware const dimensionedScalar A = fvc::domainIntegrate(UdivU); Info<<"your integrated value = "<<A.value()<< endl; } 

Tags 
integral computing, parallel code, parallel computation, parallel decomposition 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Sampling for graphs in parallel for AMI case  CL  OpenFOAM Bugs  5  January 15, 2018 11:55 
implementation of mapFields into parallel transient case  simpomann  OpenFOAM PreProcessing  4  August 2, 2016 04:41 
Superlinear speedup in OpenFOAM 13  msrinath80  OpenFOAM Running, Solving & CFD  18  March 3, 2015 05:36 
[OpenFOAM] parallel case with paraview  Ingenieur  ParaView  2  August 16, 2013 08:24 
Run in parallel a 2mesh case  cosimobianchini  OpenFOAM Running, Solving & CFD  2  January 11, 2007 06:33 