[adorean]

Hello,

I have compiled Foam-extend 4.0 and the corresponding FsiFoam package on Slackware 14.2.
Foam-extend runs fine.

When trying to run the included FsiFoam tutorials I get the error:
"flux requested but p not specified in the fluxRequired sub-dictionary of fvSchemes",

but that is not the case, the mentioned entry being in place.

What could be the real issue here?

Thank you!

Ervin

[Sapere Aude]

Hello Ervin,

i had the same problem.

If you check out the bugfix

https://sourceforge.net/p/foam-exten...502bb3bc0040e/

you can find that they disabled the reading of "fluxRequired" by commenting this part in src/finiteVolume/finiteVolume/fvSchemes/fvSchemes.C. I simply uncommented lines 382-392.

It works fine for me since i only use fsiFoam.

Do not forget wmake libso.

Best regards
Thomas

[skyoung]

Originally Posted by Sapere Aude

Hello Ervin,

i had the same problem.

If you check out the bugfix

https://sourceforge.net/p/foam-exten...502bb3bc0040e/

you can find that they disabled the reading of "fluxRequired" by commenting this part in src/finiteVolume/finiteVolume/fvSchemes/fvSchemes.C. I simply uncommented lines 382-392.

It works fine for me since i only use fsiFoam.

Do not forget wmake libso.

Best regards
Thomas

Dear Thomas,

what do you mean "do not forget to wmake libso"?

I executed "./Allclean and ./Allwmake" for the foam-extend-4.0 in the dictionary of $HOME/foam-extend-4.0, but it does not work. It still occurred the same error.

[utkunun]

Hi,

I am also having the "p not specified in the fluxRequired sub-dictionary of fvSchemes" error on foam-extend 4.0. This is a case which runs smoothly on foam-extend 3.2.

There should be a reason why the flux required option is disabled.

Thanks in advance,

Utku

[ma-tri-x]

Hi!

I experience the same error and the above bugfix by Hvorje doesn't work for me.

cd $WM_PROJECT_DIR/src/finiteVolume/finiteVolume/fvSchemes
# apply patch from above link to fvSchemes.C
# no commands for that
cd $WM_PROJECT_DIR/
wmake libso finiteVolume

didn't work. Also changing line 1046 in fvMatrix.C and recompiling whole src libs didn't work.

[ma-tri-x]

Hi Guys, I solved the issue here,

there is one line in at the very end in createFields.H, that's new in fext 4.0:

mesh.schemesDict().setFluxRequired(p.name());

so besides the above solutions, you have to integrate that line into your createFields.H and recompile your solver.

Regards,
Ma-tri-x

[Big_bird]

Originally Posted by ma-tri-x

Hi Guys, I solved the issue here,

there is one line in at the very end in createFields.H, that's new in fext 4.0:

mesh.schemesDict().setFluxRequired(p.name());

so besides the above solutions, you have to integrate that line into your createFields.H and recompile your solver.

Regards,
Ma-tri-x

Hi Matrix,
Can you please clearly explain where to integrate the line? because it is already there in the file "createFields.H".

Thanks & Regards
Big_bird

[ma-tri-x]

HI Big_bird,

I did 3 things in total:
- apply patch to fvSchemes.C (the above buxfix)
- in src/finiteVolume/fvMatrices/fvMatrix/fvMatrix.C comment the following lines:

    if (!psi_.mesh().schemesDict().fluxRequired(psi_.name()))
    {
        FatalErrorIn("fvMatrix<Type>::flux()")
            << "flux requested but " << psi_.name()
            << " not specified in the fluxRequired sub-dictionary"
               " of fvSchemes."
            << abort(FatalError);
    }

and do

cd $WM_PROJECT_DIR
cd src
wmake libso

- add the line
to your createFields.H
mesh.schemesDict().setFluxRequired(p.name());

[Big_bird]

Hi matrix,
Thanks for your reply. I just only did the 3rd point you mentioned i.e, adding the line

mesh.schemesDict().setFluxRequired(p.name());

to the createFields.H and it works fine.

[hlf4223355]

Hi big_bird
Can you please tell me which file did you revised?
i.e. where the createFields.H located? there are so many in the foam.

Cheers
Luofeng

[rr3245]

Originally Posted by Big_bird

Hi matrix,
Thanks for your reply. I just only did the 3rd point you mentioned i.e, adding the line to the createFields.H and it works fine.

I am also having trouble with this. Where is createFields.H found? I can't find any reference to it in the fsitoolkit source code. Regards, RH.

[ma-tri-x]

$WM_PROJECT_DIR/applications/solvers/some_sub_dir/the_solver_you_are_using/createFields.H

[rr3245]

Originally Posted by ma-tri-x

$WM_PROJECT_DIR/applications/solvers/some_sub_dir/the_solver_you_are_using/createFields.H

Thanks for the reply, ma-tri-x. I have checked the createFields.H for every solver in incompressible and they all include that line. So these source files appear to have been updated? Although I don't have write control for them anyway. For example:

/incompressible/icoFoam/createFields.H:

    
label pRefCell = 0;
scalar pRefValue = 0.0;
setRefCell(p, piso.dict(), pRefCell, pRefValue);
mesh.schemesDict().setFluxRequired(p.name());

So my next question is- the fsiFoam solver appears to trip up when it's running consistentIcoFluid (see below). However, I can only find consistentIcoFluid files in the fsi package (FluidSolidInteraction/src/fluidSolidInteraction/fluidSolvers/consistentIcoFluid) that I downloaded, not in the foam-extend source files. This makes sense, I think consistentIcoFluid is an 'fsi-only' solver.

Evolving fluid solver: consistentIcoFluid
Courant Number mean: 2.74517e-18 max: 0.425797 velocity magnitude: 0.0464238
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 3.27614e-07, No Iterations 4
DILUPBiCG:  Solving for Uy, Initial residual = 0.988361, Final residual = 8.95334e-07, No Iterations 4
DILUPBiCG:  Solving for Uz, Initial residual = 0.985989, Final residual = 9.63029e-07, No Iterations 4
GAMG:  Solving for p, Initial residual = 1, Final residual = 7.79802e-07, No Iterations 19
GAMG:  Solving for p, Initial residual = 2.59508e-05, Final residual = 3.63815e-07, No Iterations 2


--> FOAM FATAL ERROR: 
flux requested but p not specified in the fluxRequired sub-dictionary of fvSchemes.

Therefore, do I need to amend consistentIcoFluid files instead? There are 4 files:
calcPhi.H consistentIcoFluid.C consistentIcoFluid.dep consistentIcoFluid.H

Many thanks, RH.

[rr3245]

Originally Posted by ma-tri-x

$WM_PROJECT_DIR/applications/solvers/some_sub_dir/the_solver_you_are_using/createFields.H

Anyone able to help with the problem above? RH.

[hassan1201]

Hallo

I face the same problem

Can anyone tell us what shall we do indetails?

[Big_bird]

Hi everyone,

Apologies for the late reply. The "createFields.H" will be located inside the folder of the solver which you are using.

just paste this line of code

mesh.schemesDict().setFluxRequired(p.name());

If at all you get same error, then try to re-compile "wmake" once again. Hopefully it should work.

Best Regards

Big_bird

[rr3245]

Originally Posted by Big_bird

Hi everyone,

Apologies for the late reply. The "createFields.H" will be located inside the folder of the solver which you are using.

just paste this line of code

If at all you get same error, then try to re-compile "wmake" once again. Hopefully it should work.

Best Regards

Big_bird

Hi Big_bird, I'm not sure about this fix. Please see my post above (#13):

 https://www.cfd-online.com/Forums/openfoam-solving/185685-fsifoam-4-0-can-not-run-tutorials.html#post666611

[rr3245]

Originally Posted by hassan1201

Hallo

I face the same problem

Can anyone tell us what shall we do indetails?

All/hassan1201, I had help from a member called alia in a separate thread.

I inserted one line of code into the evolve() function for each fluidSolver (i.e. consistentIcoFluid.C, icoFluid.C, pisoFluid.C)

Insert

mesh.schemesDict().setFluxRequired(p().name());

after

const fvMesh& mesh = fluidSolver::mesh();

...into:
src/fluidSolidInteraction/fluidSolvers/consistentIcoFluid/consistentIcoFluid.C
src/fluidSolidInteraction/fluidSolvers/icoFluid/icoFluid.C
src/fluidSolidInteraction/fluidSolvers/pisoFluid/pisoFluid.C

Then I ran ./Allwmake to update and the tutorial ran fine. RH.

[anufagbemi]

@rr3245 thanks men, you're a lifesaver.

[sangeet]

Originally Posted by rr3245

All/hassan1201, I had help from a member called alia in a separate thread.

I inserted one line of code into the evolve() function for each fluidSolver (i.e. consistentIcoFluid.C, icoFluid.C, pisoFluid.C)

Insert

mesh.schemesDict().setFluxRequired(p().name());

after

const fvMesh& mesh = fluidSolver::mesh();

...into:
src/fluidSolidInteraction/fluidSolvers/consistentIcoFluid/consistentIcoFluid.C
src/fluidSolidInteraction/fluidSolvers/icoFluid/icoFluid.C
src/fluidSolidInteraction/fluidSolvers/pisoFluid/pisoFluid.C

Then I ran ./Allwmake to update and the tutorial ran fine. RH.

Thank you GOD. fsiFoam tutorials finally running on foam-extend 4.0 .