CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

codedFixedValue: accessing other patch causes crash in parallel

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree9Likes
  • 5 Post By RL-S
  • 4 Post By RL-S

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 27, 2017, 09:09
Default codedFixedValue: accessing other patch causes crash in parallel
  #1
New Member
 
Lennart Steffen
Join Date: Mar 2017
Location: Braunschweig, Germany
Posts: 17
Rep Power: 5
RL-S is on a distinguished road
Hey foamers,

first of all, because this is about a BC, it's technically about the "Solving" portion of OF, but codedFixedValue is still code, so should this thread be moved to the OF/Programming sub-forum?

Now, to the my problem:

I'm working with a solver under OF2.4.0, which only uses p, not p_rgh. I want to define a pressure gradient between my inlet (left side of the mesh) and my outlet (right side of the mesh). On the outlet, I'm using a zeroGradient BC, and on the inlet I'm using codedFixedValue, which does the following:
  1. Read pressure values of outlet patch
  2. Read two values from a dictionary called caseDict, which are a pressure gradient and a ramp time for a linear ramp
  3. Calculate pressure gradient for current time
  4. Write pressure values of outlet patch + current pressure gradient to inlet patch
This works fine when the solver runs in serial. But when run in parallel, it crashes at the first time step.
My strong feeling is that the codedFixedValue BC of the inlet can simply not access the outlet patch anymore, because the mesh got decomposed and the outlet patch is on another processor core and in another folder.


Does that sound correct? And if so, does anyone know how to solve it?


Here's my code btw:
Code:
type             codedFixedValue;
value            uniform  0;
redirectType     BcPressureLB;
code
#{
    // get patch ID on opposite side
    word oPatchName = "inandouthalf12";
    label oPatchID = this->patch().boundaryMesh().
                        findPatchID(oPatchName);
    // get pressure on other side
    const volScalarField& p = this->db().
                objectRegistry::lookupObject<volScalarField>("p");
    const scalarField& pFieldOpp = p.boundaryField()[oPatchID];

    // get pressure gradient from caseDict
    #include "readgradp.H"
            
    // write pressure from opposite side to this patch, add gradP
    scalarField& pField = *this;
    forAll(pField, faceI)
    {
        pField[faceI] = pFieldOpp[faceI] + gradP;
        Info << "p outlet: " << pFieldOpp[faceI] << 
                ", p inlet: " << pField[faceI] << endl;
    }
#};

codeInclude
#{
    #include "fvCFD.H"
#};

codeOptions
#{
    -I$(FOAM_CASE)/incl                 \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude
#};
    
codeLibs
#{
    -lmeshTools \
    -lfiniteVolume
#};
with readgradp.H being

Code:
// read the caseDict file 
const IOdictionary dict
(
 IOobject
 (
      "caseDict",
      ".",
      this->db(),
      IOobject::MUST_READ,
      IOobject::NO_WRITE,
  false
  )
);
scalar gradP = 0;
gradP = readScalar(dict.lookup("pressureGradient"));
if (gradP != 0)
{
    scalar rampTime = readScalar(dict.lookup("rampTimePG"));
    scalar curTime = this->db().time().value();
    if (rampTime != 0 && (curTime <= rampTime))
    {
        gradP = gradP * min(1, curTime / rampTime);
//        Info << "\nCurrent pressure gradient: " << gradP << "\n\n";
    }
}
Thanks in advance to anyone who has any ideas how to deal with this.
Lennart
RL-S is offline   Reply With Quote

Old   September 29, 2017, 07:17
Default
  #2
New Member
 
Lennart Steffen
Join Date: Mar 2017
Location: Braunschweig, Germany
Posts: 17
Rep Power: 5
RL-S is on a distinguished road
Ok, I have found a way, thanks to this post, which describes using Pstream and the reduce() function to make data available on all processors.

The relevant part of my code now looks like this:
Code:
// get patch ID on opposite side
label oPatchID = this->patch().boundaryMesh().
                    findPatchID(oPatchName);
// get pressure on other side
const volScalarField& p = this->db().
        objectRegistry::lookupObject<volScalarField>("p");

// patch field on opposite side for single processor
const scalarField& fieldOSP = p.boundaryField()[oPatchID];

// get patch field size from each processor
labelList fSizePerProc( Pstream::nProcs(), 0.0 );
label thisProcNo = Pstream::myProcNo();
fSizePerProc[thisProcNo] = fieldOSP.size();

// combine field sizes from all processors
reduce( fSizePerProc, sumOp<labelList>() );

// get field values from all processors
label totalFSize = sum( fSizePerProc );

// get field from each processor
scalarField fieldOAP( totalFSize, 0.0 );

// if patch is on current proc
if( fSizePerProc[thisProcNo] > 0 )
{
    // get field size on previous processors
    label prevFSize = 0;
    for (label i = 0; i < thisProcNo; ++i)
    {
        prevFSize += fSizePerProc[i];
    }
    // write field from patch on current proc
    for (label i = 0; i < fSizePerProc[thisProcNo]; ++i)
    {
        fieldOAP[i + prevFSize] = fieldOSP[i];
    }
}

// combine fields from all processors
reduce( fieldOAP, sumOp<scalarField>() );

// get pressure gradient from caseDict
#include "readgradp.H"

// write pressure from opposite side to this patch, add gradP
scalarField& pField = *this;
forAll(pField, faceI)
{
    pField[faceI] = fieldOAP[faceI] + gradP;
}
The workaround I used before this was simply keeping the relevant patches on the same processor, by manual decomposition using the setFields utility. I described that process here.
Given the additional overhead my code introduces, it might still be the case that the workaround provides better performance. I'll edit my experiences into this post later, if I don't forget it.
yushiw, tonnykz, MattS and 1 others like this.
RL-S is offline   Reply With Quote

Old   December 24, 2019, 21:20
Default this pointers!
  #3
New Member
 
Ehsan
Join Date: Oct 2019
Posts: 1
Rep Power: 0
Ehsanrah is on a distinguished road
Hi Lennart, can you explain to me which object does each"this" pointer point to? I want to use this method but I an a little confused!
Ehsanrah is offline   Reply With Quote

Reply

Tags
codedfixedvalue, openfoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[Other] dynamicTopoFVMesh and pointDisplacement RandomUser OpenFOAM Meshing & Mesh Conversion 6 April 26, 2018 07:30
Near wall treatment in k-omega SST Arnoldinho OpenFOAM Running, Solving & CFD 38 March 8, 2017 13:48
Compressor Simulation using rhoPimpleDyMFoam Jetfire OpenFOAM Running, Solving & CFD 107 December 9, 2014 13:38
[Commercial meshers] Fluent msh and cyclic boundary cfdengineering OpenFOAM Meshing & Mesh Conversion 48 January 25, 2013 03:28
[blockMesh] Cyclic BC's: Possible face ordering problem? (Channel flow) sega OpenFOAM Meshing & Mesh Conversion 3 September 28, 2010 12:46


All times are GMT -4. The time now is 17:10.