|
[Sponsors] |
FOAM FATAL IO ERROR: keyword pcorrFinal is undefined in dictionary |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 30, 2017, 22:57 |
FOAM FATAL IO ERROR: keyword pcorrFinal is undefined in dictionary
|
#1 |
New Member
Lieh
Join Date: Mar 2017
Posts: 26
Rep Power: 9 |
Hello everyone
I have simulated a T-juction for oil and water. Now I wanted to make use of dynamic mesh refinement. So having my current case I am modifying "dynamicMeshDict" as Code:
dynamicFvMesh dynamicRefineFvMesh; dynamicRefineFvMeshCoeffs { refineInterval 1; field alpha.water; lowerRefineLevel 0.001; upperRefineLevel 0.999; unrefineLevel 10; nBufferLayers 1; maxRefinement 2; maxCells 200000; correctFluxes (( phi none) (nHatf none) (rhoPhi none) (ghf none) (phirb none)(rho*nuEff none)); dumpLevel true; } Also in my "controlDict" I changed to "application interDyMFoam;" Now when running the case with "interDyMFoam" I get the error that FOAM FATAL IO ERROR: keyword pcorrFinal is undefined in dictionary "/home../run/Tjunction/system/fvSolution.solvers" But my fvsolution is as below: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "alpha.water.*" { nAlphaCorr 2; nAlphaSubCycles 1; cAlpha 1; MULESCorr yes; nLimiterIter 3; solver smoothSolver; smoother symGaussSeidel; tolerance 1e-8; relTol 0; } pcorr { solver PCG; preconditioner DIC; tolerance 1e-5; relTol 0; } p_rgh { solver PCG; preconditioner DIC; tolerance 1e-07; relTol 0.05; } p_rghFinal { $p_rgh; relTol 0; } U { solver smoothSolver; smoother symGaussSeidel; tolerance 1e-06; relTol 0; } } PIMPLE { momentumPredictor no; nOuterCorrectors 1; nCorrectors 3; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } relaxationFactors { equations { ".*" 1; } } // ************************************************************************* // Where I have made a mistake you think? |
|
March 30, 2017, 23:55 |
|
#2 |
New Member
Lieh
Join Date: Mar 2017
Posts: 26
Rep Power: 9 |
I solved the error by changing "pcorr" to the format "pcorr.*". But still don't know why this solved the issue. But now I am stuck in a error saying that
Solving for p_rgh, Initial residual = 1, Final residual = 0.0485562, No Iterations 185 #0 Foam::error:: printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64-linux-gnu/libc.so.6" #3 ? at tensorField.C:? #4 ? at ??:? #5 ? at ??:? #6 ? at ??:? #7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #8 ? at ??:? Floating point exception (core dumped) |
|
March 31, 2017, 04:59 |
|
#3 |
Senior Member
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 252
Rep Power: 21 |
But that is exactly the problem.
You need the keyword pcorrFinal for the same reason that you need p_rghFinal: in the last iteration the "Final" version of the dictionary is used to give you better control over your simulation. Your floating point exception (FPE) can have an infinite number of causes. Start by checking whether your physical set-up is correct: boundary conditions, reasonable initial condition, mesh quality, etc. Also check whether the FPE occurs when you do not use a dynamic mesh. |
|
March 31, 2017, 16:11 |
|
#4 |
New Member
Lieh
Join Date: Mar 2017
Posts: 26
Rep Power: 9 |
Thanks for your reply.
To clarify that, I did not touch anything from my static mesh case that runs properly except those I mentioned above, so initial, boundary conditions mesh and all set up should be fine. Even if the same dynamic mesh case that I have now, I switch back to static mesh it runs perfectly, or even if I run it with interFoam instead of interDyMFoam it runs without error again. Any guess that what is the issue? Thanks |
|
March 31, 2017, 16:36 |
|
#5 |
New Member
Lieh
Join Date: Mar 2017
Posts: 26
Rep Power: 9 |
I narrowed my investigation to the file "dynamicMeshDict".
there if I put the lower and upper intervals of Code:
lowerRefineLevel 0.001 upperRefineLevel 0.999; This is weird to me, why with for example 0.1 and 0.9 or 0.001 and 0.999 as above I get that error. And this is my whole file Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object dynamicMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dynamicFvMesh dynamicRefineFvMesh; dynamicRefineFvMeshCoeffs { // How often to refine refineInterval 1; // Field to be refinement on field alpha.water; // Refine field inbetween lower..upper lowerRefineLevel 0.001; upperRefineLevel 0.999; // If value < unrefineLevel unrefine unrefineLevel 10; // Have slower than 2:1 refinement nBufferLayers 1; // Refine cells only up to maxRefinement levels maxRefinement 2; // Stop refinement if maxCells reached maxCells 200000; // Flux field and corresponding velocity field. Fluxes on changed // faces get recalculated by interpolating the velocity. Use 'none' // on surfaceScalarFields that do not need to be reinterpolated. correctFluxes ( (phi none) (nHatf none) (rhoPhi none) (alphaPhi none) (ghf none) ); // Write the refinement level as a volScalarField dumpLevel true; } Code:
Starting time loop Courant Number mean: 0.00889225 max: 0.0998565 Interface Courant Number mean: 0 max: 0 deltaT = 5.48246e-06 Time = 5.48246e-06 PIMPLE: iteration 1 Selected 202 cells for refinement out of 50750. Refined from 50750 to 52164 cells. Selected 0 split points out of a possible 202. Execution time for mesh.update() = 0.25 s DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 9.05312e-06, No Iterations 466 time step continuity errors : sum local = 1.35364e-10, global = 2.31923e-13, cumulative = 3.11643e-11 smoothSolver: Solving for alpha.water, Initial residual = 1.50215e-05, Final residual = 6.51628e-09, No Iterations 1 Phase-1 volume fraction = 0.909086 Min(alpha.water) = 0 Max(alpha.water) = 1 MULES: Correcting alpha.water MULES: Correcting alpha.water Phase-1 volume fraction = 0.909086 Min(alpha.water) = 0 Max(alpha.water) = 1.00001 DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.049169, No Iterations 383 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64-linux-gnu/libc.so.6" #3 ? at tensorField.C:? #4 ? at ??:? #5 ? at ??:? #6 ? at ??:? #7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #8 ? at ??:? Floating point exception (core dumped) |
|
April 1, 2017, 11:04 |
|
#6 |
Senior Member
Kevin van As
Join Date: Sep 2014
Location: TU Delft, The Netherlands
Posts: 252
Rep Power: 21 |
If you set those two to the same value, then it does not refine. After all, it refines between X and X, but there exist no numbers between X and X.
Then, despite having a dynamic mesh, you do not actually have a dynamic mesh. Personally, I use 0.1 and 0.9 in interDyMFoam. Questions: 1) How come max Courant is not zero when you're only just starting? Since it starts at 0.1, and you then refine twice, max Courant very likely becomes 0.4. Whereas this should still be fine, it might get becomes too large when the new velocities are calculated. 2) What happens when you reduce the initial dt by, say, a factor 10? I also notice that you need a lot of iterations for pressure. 3) What happens when you add under-relaxation for PIMPLE? 4) Or what happens when you use PISO instead of PIMPLE (so nOuterCorrector=0)? |
|
April 3, 2017, 18:07 |
|
#7 |
New Member
Lieh
Join Date: Mar 2017
Posts: 26
Rep Power: 9 |
Kevin,
Thanks for your comment, FYI, everything was fine, the issue was that I was simulating a 2d case, I switched to 3d (added cells in the 3rd direction) now it is working fine. |
|
August 9, 2018, 07:29 |
|
#8 | |
New Member
Ainal Hoque Gazi
Join Date: May 2018
Location: India
Posts: 27
Rep Power: 8 |
Quote:
Hi.. For my understanding would you please tell me what change did you make with a example,that will be a great help for me. thanks and regards. Last edited by A H Gazi; August 10, 2018 at 08:57. |
||
August 10, 2018, 08:58 |
|
#9 |
New Member
Ainal Hoque Gazi
Join Date: May 2018
Location: India
Posts: 27
Rep Power: 8 |
||
September 26, 2018, 09:03 |
|
#10 |
Member
Kristjan
Join Date: Apr 2017
Location: Slovenia
Posts: 36
Rep Power: 9 |
I was surprised to see the keyword pcorrFinal not being required for interFoam v3.0.1, but required on v6. I ran my case with the fvSolution from the damBreak tutorial.
If anyone can effortlesly shed some light on the pcorr field I'd apreciate it. But it's not urgent. I just think it would be nice to have it explained online. I did a bit of research but it's starting to take to much time for me. "pcorr.*" didn't used to be required: https://github.com/OpenFOAM/OpenFOAM...199e76f37eb4a6 I was looking for clues in the interFoams pEqn.H: https://cpp.openfoam.org/dev/multiph...8H_source.html I did a Code:
grep -r 'pcorr' $FOAM_SRC https://cpp.openfoam.org/dev/CorrectPhi_8C_source.html I'm not sure if CorrectPhi.C is executed by interFoam. |
|
April 28, 2021, 07:14 |
|
#11 |
Member
Bushra Rasheed
Join Date: Dec 2020
Posts: 97
Rep Power: 5 |
||
November 19, 2021, 11:43 |
Could you add the pcorrFinal tolerance:
|
#12 |
New Member
Lima
Join Date: Oct 2020
Posts: 1
Rep Power: 0 |
In the fvSolution:
pcorr { solver PCG; preconditioner { preconditioner GAMG; tolerance 1e-5; relTol 0; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; nFinestSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e-5; relTol 0; maxIter 50; } Add the next code: the tolerance can be the same. pcorrFinal { $pcorr; tolerance 5e-9; relTol 0; } |
|
March 21, 2024, 07:23 |
|
#13 |
New Member
Join Date: Aug 2022
Posts: 19
Rep Power: 4 |
try changing the fvSolution from
Code:
pcorr { solver PCG; ...... .... } Code:
"pcorr.*" { solver PCG; ...... ...... } |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Second Derivative Zero - Boundary Condition | fu-ki-pa | OpenFOAM | 11 | March 27, 2021 05:28 |
LEMOS InflowGenerator | r_gordon | OpenFOAM Running, Solving & CFD | 103 | December 18, 2018 01:58 |
OpenFOAM 1.6-ext git installation on Ubuntu 11.10 x64 | Attesz | OpenFOAM Installation | 45 | January 13, 2012 13:38 |
Problem with rhoSimpleFoam | matteo_gautero | OpenFOAM Running, Solving & CFD | 0 | February 28, 2008 07:51 |
G95 + CGNS | Bruno | Main CFD Forum | 1 | January 30, 2007 01:34 |