[potentialToto]

Hello everyone, I'm new here and have little experience with OpenFOAM so please bear with me.

I am working on a custom solver, which is conceptually very similar to potentialFoam. I have to apply some constraints to the solver, which I'm trying to do through the fvConstraints dictionary specifications.

The custom solver compiles correctly, however upon execution an error will be raised when calling "createFvConstraints.H", which looks like:

Creating fvConstraints from "system/fvConstraints"

Selecting finite volume constraint type limitVelocity
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigSegv::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::fvConstraint::New(Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ??:?
#4  Foam::fvConstraints::fvConstraints(Foam::fvMesh const&) at ??:?
#5  ? in "/home/admin/OpenFOAM/admin-10/platforms/linux64GccDPInt32Opt/bin/fcrFoam"
#6  ? in "/home/admin/OpenFOAM/admin-10/platforms/linux64GccDPInt32Opt/bin/fcrFoam"
#7  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? in "/home/admin/OpenFOAM/admin-10/platforms/linux64GccDPInt32Opt/bin/fcrFoam"
Segmentation fault (core dumped)

I'm using OpenFOAM 10.

Here is a more detailed example of what I've tried:
Let's say I make a custom solver using potentialFoam as prototype: "myPotentialFoam". I will only modify it to include the fvConstraints specifications. So what I do is:

In myPotentialFoam.C, include fvConstraints.H at the beginning:

#include "fvCFD.H"
#include "nonOrthogonalSolutionControl.H"
#include "fvConstraints.H"

In createFields.H, include createFvConstraints.H at the end:

#include "createMRF.H"
#include "createFvConstraints.H"

This compiles correctly using wclean and wmake. Then I copy the case from the tutorials/basic/potentialFoam/cylinder, and I add a system/fvConstraints dictionary file:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  10
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvConstraints;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

limitU
{
    type limitVelocity;
    active yes;

    selectionMode all;
    max 75.0;
}


// ************************************************************************* //

Inside it is defined a simple limitVelocity constraint. I know that I did not call fvConstraints.constrain() at any point in myPotentialfoam.C, so this wouldn't do anything anyway. But, the error occurs before the solver loop even starts. Also, I've tried using fixedValueConstraint instead of limitVelocity, but the problem is the same. When I execute:

./Allclean
blockMesh
myPotentialFoam

I get the said error. What am I doing wrong? I'm adding the minimal working example as attachment.

Any tip would be appreciated, thank you in advance for your help!

[potentialToto]

In the end, I figured it out by myself.

For anyone interested, the solution was to add an entry in Make/options so that the fvConstraints library is linked.

Effectively, modifying Make/options from:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools

to:

EXE_INC = \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmeshTools \
    -lfvModels \
    -lfvConstraints

solves the issue.