CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions > OpenFOAM CC Toolkits for Fluid-Structure Interaction

[FSI] FsiFoam 4.0 - can not run tutorials

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

Like Tree11Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 31, 2017, 04:19
Default FsiFoam 4.0 - can not run tutorials
  #1
Member
 
Ervin Adorean
Join Date: Mar 2009
Posts: 72
Rep Power: 12
adorean is on a distinguished road
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
Attached Files
File Type: txt fsiFoam_log.txt (3.8 KB, 68 views)
adorean is offline   Reply With Quote

Old   April 19, 2017, 17:13
Default
  #2
New Member
 
Thomas
Join Date: Apr 2017
Posts: 1
Rep Power: 0
Sapere Aude is on a distinguished road
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
rezaeimahdi and fuxpaul like this.
Sapere Aude is offline   Reply With Quote

Old   July 4, 2017, 06:08
Default
  #3
New Member
 
WA
Join Date: Jun 2017
Posts: 5
Rep Power: 4
skyoung is on a distinguished road
Quote:
Originally Posted by Sapere Aude View Post
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.
pjagdale1 likes this.
skyoung is offline   Reply With Quote

Old   August 10, 2017, 05:44
Default
  #4
New Member
 
Join Date: Mar 2014
Posts: 17
Rep Power: 7
utkunun is on a distinguished road
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
utkunun is offline   Reply With Quote

Old   August 16, 2017, 06:45
Default Problem, too
  #5
Member
 
Join Date: Sep 2013
Posts: 42
Rep Power: 8
ma-tri-x is on a distinguished road
Hi!

I experience the same error and the above bugfix by Hvorje doesn't work for me.
Quote:
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 is offline   Reply With Quote

Old   August 16, 2017, 11:11
Default Found the error
  #6
Member
 
Join Date: Sep 2013
Posts: 42
Rep Power: 8
ma-tri-x is on a distinguished road
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:
Code:
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
ma-tri-x is offline   Reply With Quote

Old   August 18, 2017, 12:36
Default
  #7
New Member
 
Join Date: Aug 2017
Location: Germany
Posts: 3
Rep Power: 4
Big_bird is on a distinguished road
Quote:
Originally Posted by ma-tri-x View Post
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:
Code:
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
Big_bird is offline   Reply With Quote

Old   August 21, 2017, 06:31
Default where to integrate
  #8
Member
 
Join Date: Sep 2013
Posts: 42
Rep Power: 8
ma-tri-x is on a distinguished road
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:

Code:
    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
Code:
cd $WM_PROJECT_DIR
cd src
wmake libso
- add the line
to your createFields.H
mesh.schemesDict().setFluxRequired(p.name());
ma-tri-x is offline   Reply With Quote

Old   August 21, 2017, 16:04
Default
  #9
New Member
 
Join Date: Aug 2017
Location: Germany
Posts: 3
Rep Power: 4
Big_bird is on a distinguished road
Hi matrix,
Thanks for your reply. I just only did the 3rd point you mentioned i.e, adding the line
Quote:
mesh.schemesDict().setFluxRequired(p.name());
to the createFields.H and it works fine.
Big_bird is offline   Reply With Quote

Old   September 24, 2017, 17:08
Default
  #10
New Member
 
Luofeng
Join Date: May 2016
Posts: 5
Rep Power: 5
hlf4223355 is on a distinguished road
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
hlf4223355 is offline   Reply With Quote

Old   September 28, 2017, 06:05
Default
  #11
New Member
 
anonymous
Join Date: Nov 2016
Posts: 29
Rep Power: 5
rr3245 is on a distinguished road
Quote:
Originally Posted by Big_bird View Post
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.
rr3245 is offline   Reply With Quote

Old   October 4, 2017, 13:28
Default
  #12
Member
 
Join Date: Sep 2013
Posts: 42
Rep Power: 8
ma-tri-x is on a distinguished road
$WM_PROJECT_DIR/applications/solvers/some_sub_dir/the_solver_you_are_using/createFields.H
ma-tri-x is offline   Reply With Quote

Old   October 5, 2017, 05:21
Default
  #13
New Member
 
anonymous
Join Date: Nov 2016
Posts: 29
Rep Power: 5
rr3245 is on a distinguished road
Quote:
Originally Posted by ma-tri-x View Post
$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:
Code:
    
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.

Code:
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 is offline   Reply With Quote

Old   October 19, 2017, 05:08
Default
  #14
New Member
 
anonymous
Join Date: Nov 2016
Posts: 29
Rep Power: 5
rr3245 is on a distinguished road
Quote:
Originally Posted by ma-tri-x View Post
$WM_PROJECT_DIR/applications/solvers/some_sub_dir/the_solver_you_are_using/createFields.H
Anyone able to help with the problem above? RH.
rr3245 is offline   Reply With Quote

Old   October 19, 2017, 14:43
Default
  #15
New Member
 
Hassan Adel
Join Date: Oct 2013
Location: Egypt
Posts: 18
Rep Power: 8
hassan1201 is on a distinguished road
Hallo

I face the same problem

Can anyone tell us what shall we do indetails?
__________________
H.Elsheshtawy
hassan1201 is offline   Reply With Quote

Old   October 19, 2017, 16:25
Thumbs up Solved
  #16
New Member
 
Join Date: Aug 2017
Location: Germany
Posts: 3
Rep Power: 4
Big_bird is on a distinguished road
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
Quote:
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
Big_bird is offline   Reply With Quote

Old   October 23, 2017, 07:43
Default
  #17
New Member
 
anonymous
Join Date: Nov 2016
Posts: 29
Rep Power: 5
rr3245 is on a distinguished road
Quote:
Originally Posted by Big_bird View Post
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):

HTML Code:
 https://www.cfd-online.com/Forums/openfoam-solving/185685-fsifoam-4-0-can-not-run-tutorials.html#post666611
rr3245 is offline   Reply With Quote

Old   November 22, 2017, 05:34
Default
  #18
New Member
 
anonymous
Join Date: Nov 2016
Posts: 29
Rep Power: 5
rr3245 is on a distinguished road
Quote:
Originally Posted by hassan1201 View Post
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

Code:
mesh.schemesDict().setFluxRequired(p().name());
after

Code:
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.
ilhado, Luttappy, sangeet and 3 others like this.
rr3245 is offline   Reply With Quote

Old   November 25, 2017, 18:05
Default
  #19
New Member
 
Sam
Join Date: Nov 2017
Posts: 24
Rep Power: 4
anufagbemi is on a distinguished road
@rr3245 thanks men, you're a lifesaver.
anufagbemi is offline   Reply With Quote

Old   June 2, 2018, 13:53
Default
  #20
New Member
 
Sangeet
Join Date: Jun 2017
Location: India
Posts: 26
Rep Power: 4
sangeet is on a distinguished road
Quote:
Originally Posted by rr3245 View Post
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

Code:
mesh.schemesDict().setFluxRequired(p().name());
after

Code:
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 .
sangeet is offline   Reply With Quote

Reply

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
[waves2Foam] Compiled with foam-extend-4.0, but I cannot run tutorials in parallel lxwd OpenFOAM Community Contributions 7 February 22, 2017 03:13
OpenFOAM can't be run in parallel in cluster sibo OpenFOAM Running, Solving & CFD 4 February 21, 2017 17:29
parallel run is slower than serial run (pimpleFoam) !!! mechy OpenFOAM 18 August 17, 2016 18:19
simpleFoam parallel AndrewMortimer OpenFOAM Running, Solving & CFD 12 August 7, 2015 19:45
[mesh manipulation] Cannot get refineMesh to run in parallel smschnob OpenFOAM Meshing & Mesh Conversion 2 June 3, 2014 12:20


All times are GMT -4. The time now is 20:44.