|
[Sponsors] |
MRF case - simpleFoam quits after building mesh for time = 0 |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 25, 2019, 11:40 |
MRF case - simpleFoam quits after building mesh for time = 0
|
#1 |
New Member
Join Date: Mar 2017
Posts: 25
Rep Power: 9 |
Hi.
I tried to set up an MRF case to be solved with simpleFoam based on the mixerVessel2D tutorial. When i try to run simpleFoam the process quits after creating the mesh for time = 0 without an reasonable error. Can anyone give me a hint what i'm doing wrong? Here is the log.simpleFoam file: Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 6-47517f2ebb1b Exec : simpleFoam Date : Nov 25 2019 Time : 16:34:20 Host : "892836" PID : 254 I/O : uncollated Case : /mnt/c/Users/72/Documents/lnxWork/TSOLA nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: No convergence criteria found Reading field p Reading field U Reading/calculating face flux field phi AMI: Creating addressing and weights between 12536 source faces and 6271 target faces AMI: Patch source sum(weights) min/max/average = 0.0919981, 1.0503, 0.982951 AMI: Patch target sum(weights) min/max/average = 0, 1.00164, 0.983866 AMI: Creating addressing and weights between 7424 source faces and 3337 target faces AMI: Patch source sum(weights) min/max/average = 0.999738, 1.0005, 1.00006 AMI: Patch target sum(weights) min/max/average = 0.999067, 1.00017, 0.999992 Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kEpsilon bounding k, min: 0 max: 0.075 average: 0 bounding epsilon, min: 0 max: 2 average: 2 RAS { RASModel kEpsilon; turbulence on; printCoeffs on; Cmu 0.09; C1 1.44; C2 1.92; C3 0; sigmak 1; sigmaEps 1.3; } Creating MRF zone list from MRFProperties creating MRF zone: MRF1 No finite volume options present |
|
November 25, 2019, 12:10 |
|
#2 |
Senior Member
Kmeti Rao
Join Date: May 2019
Posts: 145
Rep Power: 8 |
With the information provided by you, it is very difficult to add any input without seeing the case setup.
|
|
November 25, 2019, 13:25 |
|
#3 | |
New Member
Join Date: Mar 2017
Posts: 25
Rep Power: 9 |
Quote:
Below additional information to my case-setup. Do you have any particular file in mind that might give the solution? What surprises me the most is that the termination is done without error message.
system/controlDict:
system/fvSchemes:
system/fvSolution:
constant/transportProperties:
constant/MRFProperties:
0/U:
0/p:
0/nut:
0/k:
0/epsilon:
|
||
November 26, 2019, 03:21 |
|
#4 | |
Senior Member
Kmeti Rao
Join Date: May 2019
Posts: 145
Rep Power: 8 |
Hi Bastian,
your setup looks ok, now I found out the problem, Quote:
But I am not sure why OpenFOAM is not throwing out any error. Go through the following threads, to know more about 0 weight error. One half propeller simulation with MRFSimpleFoam crashing and Periodic cyclic AMI + MRF crashing on pressure Best wishes, K. Rao |
||
November 28, 2019, 12:16 |
|
#5 |
New Member
Join Date: Mar 2017
Posts: 25
Rep Power: 9 |
Hi Krao,
Thank you for your answer. I did a complete rework of the case including a better mesh. Although the weighting has improved, the result remains the same as you can see in the log file. Any idea what to check next? Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 6-47517f2ebb1b Exec : simpleFoam Date : Nov 28 2019 Time : 17:12:12 Host : "892836" PID : 316 I/O : uncollated Case : /mnt/c/Users/72/Documents/lnxWork/TSOLA nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: No convergence criteria found Reading field p Reading field U Reading/calculating face flux field phi AMI: Creating addressing and weights between 9430 source faces and 4928 target faces AMI: Patch source sum(weights) min/max/average = 0.999215, 1.02469, 0.999989 AMI: Patch target sum(weights) min/max/average = 0.990802, 1.00066, 1.00006 Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kEpsilon bounding k, min: 0 max: 0.075 average: 0 bounding epsilon, min: 0 max: 2 average: 2 RAS { RASModel kEpsilon; turbulence on; printCoeffs on; Cmu 0.09; C1 1.44; C2 1.92; C3 0; sigmak 1; sigmaEps 1.3; } Creating MRF zone list from MRFProperties creating MRF zone: MRF1 No finite volume options present |
|
November 29, 2019, 02:41 |
|
#6 |
Senior Member
Kmeti Rao
Join Date: May 2019
Posts: 145
Rep Power: 8 |
Hi Bastian,
difficult to add anything, the setup looks decent. Leave log file, before stopping does the terminal shows anything or is it also blank? If I get time on weekend I can go through your setup. If you don't want to share geometry, you can remove the geometry and important info from mesh and you can send the case to me. I can see if I could do something. Or if you think it is not a big secret then you can post it here and anyone can help you. K. Rao |
|
January 28, 2020, 05:43 |
|
#7 |
New Member
Join Date: Mar 2017
Posts: 25
Rep Power: 9 |
Hello Krao, sorry I'm late back.
It seems that the problem was due to a too big imbalance between the number of source faces to target faces. After I adjusted the mesh again, it worked. Nevertheless, I have switched to foam-extend. The GGI interfaces have more options and look much more stable and evolved than AMI. |
|
February 6, 2020, 04:50 |
|
#8 |
Senior Member
Kmeti Rao
Join Date: May 2019
Posts: 145
Rep Power: 8 |
Hi Bastian,
After receiving your feedback about foam-extend, I have though to make a comparison of results obtained using openFoam and foam-extend. I tried MRFsimpleFoam with ggi instead of AMI. I am facing problems during parallel running. My case runs very well in serial, when I decompose and run the case in parallel, my simulation stop after reading 'Reading/calculating face flux field phi'. Did you face similar problem by any chance? Which type of decomposition method are you using? It would be nice to know. Thank you, K. Rao |
|
February 7, 2020, 17:42 |
|
#9 |
New Member
Join Date: Mar 2017
Posts: 25
Rep Power: 9 |
Hi Krao,
generally, in the decomposeParDict, you have to specify all interfaces (ggi/mixingPlane) as globalFaceZones. Additionally, at least for mixing planes, you have to do the partitioning patchConstrained. This means that the interfaces are assigned to a single processor instead of getting "cutted". Like i mentioned before, i'm not sure if its a only necessary in case of mixing planes or also affects ggi interfaces. Anyway it works for both. See below my decomposePar dict. Just adapt the names of the interfaces to your case. The numbers after the names in the patchConstrainedCoeffs sets the number of the processor to which they will be assigned to. Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | foam-extend: Open Source CFD | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: http://www.foam-extend.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object decomposeParDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // nCores 12; numberOfSubdomains $nCores; method patchConstrained; globalFaceZones ( rotorOutletZone rotorPeriodicPSZone rotorPeriodicSSZone statorInletZone ); patchConstrainedCoeffs { method metis; numberOfSubdomains $nCores; patchConstraints ( (rotorOutletMP 1) (statorInletMP 1) (rotorPeriodic_PS 2) (rotorPeriodic_SS 2) ); } metisCoeffs { processorWeights ( 1 1 1 1 1 1 1 1 1 1 1 1 ); } // ************************************************************************* // Last edited by .bastian; February 9, 2020 at 13:59. |
|
Tags |
mrf simplefoam, simplefoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM.org] Instructions to install OpenFOAM-2.4.x on CentOS-6.10 | redbullah | OpenFOAM Installation | 9 | September 7, 2019 18:18 |
[foam-extend.org] Error compiling OpenFOAM-1.6-ext | Canesin | OpenFOAM Installation | 137 | January 20, 2016 15:56 |
[snappyHexMesh] No layers in a small gap | bobburnquist | OpenFOAM Meshing & Mesh Conversion | 6 | August 26, 2015 10:38 |
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! | sc298 | OpenFOAM Meshing & Mesh Conversion | 2 | March 27, 2011 22:11 |
Free surface boudary conditions with SOLA-VOF | Fan | Main CFD Forum | 10 | September 9, 2006 13:24 |