|
[Sponsors] |
March 10, 2009, 04:08 |
Dear all,
I am struggling t
|
#1 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 10, 2009, 04:21 |
Things to add after some more
|
#2 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 10, 2009, 05:16 |
Ok, I oriented on the mixerGgi
|
#3 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 10, 2009, 05:46 |
> I guess I have to make sure
|
#4 |
Member
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 17 |
> I guess I have to make sure interface is on one CPU
Try: preservePatches( patch1 patch2 ..) preserveFaceZones( facezone1 faceZone2 ..) in decomposeParDict /Johan |
|
March 10, 2009, 05:58 |
Thanks Johan,
I can not get
|
#5 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 10, 2009, 06:17 |
BastiL, I don't know if there
|
#6 |
Member
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 17 |
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? |
|
March 10, 2009, 06:34 |
Yes, I currently have:
/*--
|
#7 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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? |
|
March 10, 2009, 06:40 |
Ok, miving it to the end (afte
|
#8 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 10, 2009, 08:08 |
I did not have access to my Op
|
#9 |
Member
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 17 |
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 ... |
|
March 10, 2009, 09:33 |
Thanks looks good. Seems to wo
|
#10 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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. |
|
March 11, 2009, 18:18 |
Ok I have run some tests, most
|
#11 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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?
|
|
March 12, 2009, 04:09 |
Ok on a non running case i get
|
#12 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 12, 2009, 05:07 |
Hello all,
Bastil, I am just
|
#13 |
New Member
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 17 |
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 __________ Fig 2.: 3 blocks with mesh looks like __________ 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) __________ Attach simple case with gambit mesh. May I ask you for helping me with set-up case. David |
|
March 12, 2009, 05:14 |
I hope in sucessful picture at
|
#14 |
New Member
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 17 |
I hope in sucessful picture attach.
Fig 1.: 3 blocks, split with ggi __________ Fig 2.: 3 blocks with mesh looks like __________ Fig 3.: complex geometry with quad and tri interface (source TGrid mesh) __________ Attach simple case with gambit mesh: |
|
March 12, 2009, 05:53 |
Hello again,
Mattijs wrote me
|
#15 |
New Member
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 17 |
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 _____ |
|
March 12, 2009, 07:24 |
All of these GGIs will work wi
|
#16 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
March 12, 2009, 07:56 |
Hello Hrvoje,
thanks for shar
|
#17 |
New Member
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 17 |
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 ______ |
|
March 12, 2009, 08:22 |
Hallo Hrv,
thanks for these
|
#18 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
March 12, 2009, 12:23 |
If you have uncovered faces, y
|
#19 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
March 12, 2009, 12:37 |
Thanks Hrv for this explanatio
|
#20 |
Senior Member
BastiL
Join Date: Mar 2009
Posts: 530
Rep Power: 20 |
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 |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Partioning of Mesh having nonconformal interfaces | Saji | FLUENT | 0 | July 15, 2006 05:58 |
Grid interfaces in Fluent | Omar Qazi | FLUENT | 1 | January 28, 2006 19:55 |
Fluent - discontinuous grid interfaces | Simon Archen | FLUENT | 2 | November 16, 2001 10:52 |
Sliding mesh interfaces | Karl Kevala | FLUENT | 1 | February 20, 2001 05:31 |
Periodic grid-interfaces in FLUENT 5 | tom | Main CFD Forum | 8 | May 13, 1999 21:27 |