Dear all,
I am struggling t
Dear all,
I am struggling to run meshes imported from FLUENT including interfaces. AFAIK there are two options: 1. stitchMesh -> use 1.5-dev 2. ggi -> use 1.5-dev First option works on some vanilla cases but fails on my real life geometries with various errors and large memory consumption. Could not get it running on all types of my interfaces. So I tried ggi and I am struggling: Starting time loop [node013:00375] *** Process received signal *** [node013:00375] Signal: Floating point exception (8) [node013:00375] Signal code: (-6) [node013:00375] Failing at address: 0xb5a00000177 [node013:00375] [ 0] /lib64/libc.so.6 [0x2b57acb3ec10] [node013:00375] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b57acb3eb95] [node013:00375] [ 2] /lib64/libc.so.6 [0x2b57acb3ec10] [node013:00375] [ 3] /opt/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam6divid eERNS_5FieldIdEERKNS_5UListIdEES6_+0xa1) [0x2b57ac2f0c 71] This is a simpleFOAM job in parallel. I guess I have to make sure interface is on one CPU? May this be the problem? How can I ensure this? Are there furter options to handle FLUENT interfaces? Regards |
Things to add after some more
Things to add after some more tries:
- I also get a Floating point exception when running in seriell - I do not know what "bridgeOverlap" is good for but I see the same behaviour if I turn it on or not. Maybe some ggi-expert can provide me with some hints. Regards |
Ok, I oriented on the mixerGgi
Ok, I oriented on the mixerGgi-tutorial and gave the ggi initial values. This does not seem to be essential. If I skip that it is running in serial but it still fails in parallel. I guess this to be a decomposition problem? How can this be solved?
Regards |
> I guess I have to make sure
> I guess I have to make sure interface is on one CPU
Try: preservePatches( patch1 patch2 ..) preserveFaceZones( facezone1 faceZone2 ..) in decomposeParDict /Johan |
Thanks Johan,
I can not get
Thanks Johan,
I can not get it running. How does decomposePar exactly have to look like? Is there an example hanging around somewhere? I always get: ill defined primitiveEntry starting at keyword 'preservePatches(patch1' on line 19 and ending at line 62 Regards |
BastiL, I don't know if there
BastiL, I don't know if there are examples. There should be a ; at the end of the line aswell:
preservePatches(patch1 ..); Could you post your dictionary? |
Yes, I currently have:
/*--
Yes, I currently have:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.5 | | \ / A nd | Web: http://www.OpenFOAM.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object decomposeParDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // numberOfSubdomains 32; method hierarchical; //method metis; preservePatches( patch1 patch2 ); simpleCoeffs { n (6 1 1); delta 0.001; } hierarchicalCoeffs { n (32 1 1); delta 0.001; order xyz; } metisCoeffs { //processorWeights //( // 1 // 1 // 1 // 1 //); } manualCoeffs { dataFile ""; } distributed no; roots ( ); // ************************************************** *********************** // And I get: Create time Time = 0 Create mesh Calculating distribution of cells Selecting decompositionMethod hierarchical keyword hierarchicalCoeffs is undefined in dictionary "/path/to/case/system/decomposeParDict" file: /path/to/case/system/decomposeParDict from line 17 to line 27. From function dictionary::subDict(const word& keyword) const in file db/dictionary/dictionary.C at line 271. FOAM exiting Must it be placed somewhere else? |
Ok, miving it to the end (afte
Ok, miving it to the end (after roots ();) i get:
ill defined primitiveEntry starting at keyword 'preservePatches(patch1' on line 58 and ending at line 62 |
I did not have access to my Op
I did not have access to my OpenFOAM installation earlier today.
So it should be preservePatches (patch1 patch2); and not: preservePatches(patch1 patch2); Posted the decomposePar and output of a testcase below: Good luck! /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: dev | | \ / A nd | Web: http://www.OpenFOAM.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object decomposeParDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // numberOfSubdomains 32; method hierarchical; //method metis; preservePatches (fan inlet); preserveFaceZones (fanvol); simpleCoeffs { n (6 1 1); delta 0.001; } hierarchicalCoeffs { n (32 1 1); delta 0.001; order xyz; } metisCoeffs { //processorWeights //( // 1 // 1 // 1 // 1 //); } manualCoeffs { dataFile ""; } distributed no; roots ( ); // ************************************************** *********************** // ~ On my system this gives /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.5-extend | | \ / A nd | Web: http://www.OpenFOAM.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : decomposePar Date : Mar 10 2009 Time : 12:56:13 Host : linux3 PID : 9741 Case : Ggi nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Time = 0.00688181 Create mesh Calculating distribution of cells Keeping owner and neighbour of faces in patches 2 ( fan inlet ) on same processor Keeping owner and neighbour of faces in zones 1 ( fanvol ) on same processor Selected 1183862 faces whose owner and neighbour cell should be kept on the same processor Selecting decompositionMethod hierarchical Finished decomposition in 0.44 s Calculating original mesh data Distributing cells to processors Distributing faces to processors Calculating processor boundary addressing Distributing points to processors Constructing processor meshes Processor 0 Number of cells = 5654 Number of faces shared with processor 1 = 1229 Number of processor patches = 1 Number of processor faces = 1229 Number of boundary faces = 1743 Processor 1 Number of cells = 5654 Number of faces shared with processor 0 = 1229 Number of faces shared with processor 2 = 1689 Number of processor patches = 2 Number of processor faces = 2918 Number of boundary faces = 1050 ... |
Thanks looks good. Seems to wo
Thanks looks good. Seems to work now for my purposes. Only thing I am struggling with is a GGicheck-Function that makes my calculation crashing after iteration 1, Withaiut that it seems to run fine.
Regards. |
Ok I have run some tests, most
Ok I have run some tests, most run fine some are struggling. I guess this has to do with tolerances I get warnings (will post one later) How can tolerance be controlled? And I am still wondering about the bridgeOverlap parameter - what is it good for?
|
Ok on a non running case i get
Ok on a non running case i get something like this:
Evaluation of GGI weighting factors: --> FOAM Warning : From function Foam::SutherlandHodgman::lineSegmentIntersection() in file algorithms/polygon/clipping/SutherlandHodgman.C at line 109 ua does not match with ub: delta: 1.83103e-15 : epsilon: 1e-15 and: Evaluation of GGI weighting factors: From function void GGIInterpolation<masterpatch,>::rescaleWeightingFa ctors() const in file /opt/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/GGIInterpolationWeights.C at line 531 Uncovered faces found: on master:0 on slave: 165 Largest slave weighting factor correction : 0.998995 average: 0.0234367 Largest master weighting factor correction: 0.0314782 average: 0.00255351 I expect at least one of these to be the problem why this case is not running. How can I find out which of my ggis cause the problem? Secnd warning sounds like there is no suport for partial ggi so far? Thanks for clarification. Regards |
Hello all,
Bastil, I am just
Hello all,
Bastil, I am just preparing very simple testing case with ggi. This test may help me to understand how to set up case with interfaces / ggi. This testing case looks like cavity with upper mowing wall. The cavity domain is split into the 3 blocks (see Figure 1, 2). Fig 1.: 3 blocks, split with ggi http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ Fig 2.: 3 blocks with mesh looks like http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ After sucessfull runnig case, I would like use ggi with more complex geometry, where I have to use retriangulation interface which is neighbour to the side of the prismatic layer (see Figure 3) Fig 3.: complex geometry with quad and tri interface (source TGrid mesh) http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ Attach simple case with gambit mesh. May I ask you for helping me with set-up case. David |
I hope in sucessful picture at
I hope in sucessful picture attach.
Fig 1.: 3 blocks, split with ggi http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ Fig 2.: 3 blocks with mesh looks like http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ Fig 3.: complex geometry with quad and tri interface (source TGrid mesh) http://www.cfd-online.com/OpenFOAM_D...your_image.gif __________ Attach simple case with gambit mesh: |
Hello again,
Mattijs wrote me
Hello again,
Mattijs wrote me, that discusion board is some time full and the web browser does not responce to the attaching files. So I attach all picture and testing case here: http://drop.io/dsponiar I hope this would be functional - it is for me for the first time, what I attach file any at the "on-line space". Ragards, David _____ |
All of these GGIs will work wi
All of these GGIs will work without any trouble. For a really cool (and really new) one, have a look at: OpenFOAM: VOF + 6-DOF + GGI http://www.cfd-online.com/OpenFOAM_D...part/happy.gif
Hrv |
Hello Hrvoje,
thanks for shar
Hello Hrvoje,
thanks for sharing nice animation. I think for me, it is so far to simulate this complex phenomenom. Yesterday, I was building the newest OF release and testing GGI. When I start simulation with cavity (mesh prepare in Gambit) split into the 3 blocks, I found this log: Exec : simpleFoam -case 18-GGI_interface_OF-1.5-dev Date : Mar 12 2009 Time : 12:45:01 Host : sponiar PID : 29352 Case : ./18-GGI_interface_OF-1.5-dev nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading field p Reading field U Reading/calculating face flux field phi Evaluation of GGI weighting factors: Largest slave weighting factor correction : 1.19209e-07 average: 8.34465e-08 Largest master weighting factor correction: 1.19209e-07 average: 4.76837e-08 Evaluation of GGI weighting factors: Largest slave weighting factor correction : 1.19209e-07 average: 1.19209e-08 Largest master weighting factor correction: 1.19209e-07 average: 1.78814e-08 Evaluation of GGI weighting factors: Largest slave weighting factor correction : 1.19209e-07 average: 2.98023e-08 Largest master weighting factor correction: 1.78814e-07 average: 5.07743e-08 Selecting incompressible transport model Newtonian Selecting RAS turbulence model laminar Starting time loop Creating ggi check Time = 1 PBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.52828e-06, No Iterations 8 PBiCG: Solving for Uy, Initial residual = 1, Final residual = 7.84278e-06, No Iterations 7 Continuity error cannot be removed by adjusting the outflow. Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow. Specified mass inflow : 5.25403e-07 Specified mass outflow : 0 Difference : 5.25403e-07 Adjustable mass outflow : 5.25403e-07 From function adjustPhi ( surfaceScalarField& phi, const volVectorField& U, const volScalarField& p ) in file cfdTools/general/adjustPhi/adjustPhi.C at line 128. FOAM exiting I tried to set up ggi with some initialization value for velocity and pressure, but the same error occured. Any hint? Regards, David ______ |
Hallo Hrv,
thanks for these
Hallo Hrv,
thanks for these hints. What about my two warnings? I found out that removing the second warning " Uncovered faces found" makes my simulation to run. this seems to be caused by "partial" interfaces, right? Are there plans to implement partial interfaces? What about first warning? Thanks BastiL |
If you have uncovered faces, y
If you have uncovered faces, you need to use bridging, otherwise their values are undefined. Regarding the other warning, it is to do with the accuracy of your geometry - 1e-15 does not sound too bad. Martin and I will probably re-tune the tolerances once we get enough experience with the real cases.
Hrv |
Thanks Hrv for this explanatio
Thanks Hrv for this explanation,
so I only use brigding if I get this warning? Or always? I don't really understand what bridging is intended for? The GGIs with "uncovered faces" are definitely partial once. Will this work with bridging turned on? Thanks once more. Regards BastiL |
All times are GMT -4. The time now is 02:44. |