|
[Sponsors] |
May 5, 2013, 23:27 |
decomposePar pointfield
|
#1 |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Dear All foamers:
I have met a problem when I use decomposePar to decompose the field which has a dynamic boundary. The boundary motion is described with a pointfield. The problem appears when the decompose plane crosses the dynamic boundary. Otherwise, it seems Ok. In additiion, I have found that the problem has been encountered by other users, but it seems that there are nobody to solve it. My error information as follows: [6] --> FOAM FATAL IO ERROR: [6] size 6977 is not equal to the given value of 933 [2] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor2/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [2] [2] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [2] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [2] FOAM parallel run exiting [2] [6] [6] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor6/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [6] [6] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [6] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [6] FOAM parallel run exiting [6] [0] [0] --> FOAM FATAL IO ERROR: [0] size 6977 is not equal to the given value of 944 [0] [0] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor0/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [0] [0] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [0] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [0] FOAM parallel run exiting [0] [4] [4] --> FOAM FATAL IO ERROR: [4] size 6977 is not equal to the given value of 866 [4] [4] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor4/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [4] [4] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [4] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [4] FOAM parallel run exiting [4] [7] [7] [3] [3] [3] --> FOAM FATAL IO ERROR: [3] size 6977 is not equal to the given value of 876 [3] [3] [7] --> FOAM FATAL IO ERROR: [7] size 6977 is not equal to the given value of 1025 [7] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor3/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [3] [3] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [3] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236[7] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor7/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [7] [7] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [7] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C. [3] FOAM parallel run exiting [3] at line 236. [7] FOAM parallel run exiting [7] [1] [1] [1] --> FOAM FATAL IO ERROR: [1] size 6977 is not equal to the given value of 840 [1] [1] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor1/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [1] [1] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [1] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [1] FOAM parallel run exiting [1] [5] [5] [5] --> FOAM FATAL IO ERROR: [5] size 6977 is not equal to the given value of 808 [5] [5] file: /gpfs/home/xgcui/OpenFOAM/xgcui-2.0.0/run/test1/flow3d-movingmesh-f-3/processor5/0/pointMotionU::boundaryField::WALL1 from line 26 to line 7013. [5] [5] From function Field<Type>::Field(const word& keyword, const dictionary&, const label) [5] in file /usr/local/OpenFOAM/OpenFOAM-2.0.0/src/OpenFOAM/lnInclude/Field.C at line 236. [5] FOAM parallel run exiting Does anybody have any ideas on it? Would you please give me some hints on it? Best wishes! Last edited by flying; May 5, 2013 at 23:28. Reason: add content |
|
May 6, 2013, 14:32 |
|
#2 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 |
Hi,
as you wrote in the PM you have an error while decomposing. Like I interprete the error you have the files in 0 always initialised with a other mesh. Maybe thats the reason! |
|
May 6, 2013, 22:16 |
|
#3 |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Hey Tobi:
Many thanks for your reply. In this case, how may I solve the problem? Please give me some hints on it. |
|
May 7, 2013, 12:25 |
|
#4 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 |
1. use decomposePar -force
2. check in your folder 0 the files pointMotionU if there are any lists in it. If yes you have to create that folder new. I am not familiar with moving meshes |
|
May 7, 2013, 21:14 |
|
#5 |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Dear Tobi:
Thanks so much for your reply. It stil doesn't work. However, I found that the problem comes from the number of p0 is not equal to the mesh point number. If I change the data in the pointMotionU and make the value uniform and delete the number of value. It will work. |
|
May 7, 2013, 21:36 |
|
#6 | |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Hey Bruno and all fomers:
I upload a simple case, it is orginally downloaded from the link as follows: http://www.tfd.chalmers.se/~hani/kur...atchDeform.tgz It is orginally solved with icoFoam, but I have changed it to the pimpleDyMFoam. The lib file is for the moving boundary. As my case is very large and it is changed based this case, then I uploaded this case. My problem is the same as it. It will be great for any further suggestions. Quote:
|
||
May 19, 2013, 07:02 |
|
#7 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Xinguang Cui,
I've finally taken a look into this and I cannot find any problems. I've tested on OpenFOAM 2.2.x, 2.0.x and 2.0.1 and I had no problems in performing the following steps: Code:
wmake libso libMyPolynomVelocity cd movingCyl1 blockMesh decomposePar Best regards, Bruno
__________________
|
|
May 19, 2013, 09:51 |
|
#8 | |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
DEAR BRUNO:
Thanks for the information. Would you please put up the decomposePar file? I would like to see the way to decompose the mesh. bEST WISHES Quote:
|
||
May 19, 2013, 10:49 |
|
#9 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Xinguang Cui,
I didn't change anything on the "decomposeParDict". I used the one provided in your test case. All I did was clean up a bit the folder "0", by removing some strange files named ".goutputstream*" and one named "pointMotionU~". Best regards, Bruno
__________________
|
|
May 19, 2013, 11:02 |
|
#10 | |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Hey Bruno:
Thanks sor your reply. Have ever tried to run it? I also can decompose it, however it shows problem when it runs the case using pimpleDyMFoam. I also tried it in 2.2 0 and 2.1.1. Thanks and best wishes! Quote:
|
||
May 19, 2013, 12:44 |
|
#11 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Xinguang Cui,
The error was completely different from the one originally reported... and the case you prepared seems to be completely different from the initial report... and on top of that, the case was not fully prepared to run... Anyway, the attached case "movingCyl1_22x.tar.gz" runs fine on OpenFOAM 2.2.x. To run it: Code:
./Allrun Code:
./Allclean
Best regards, Bruno
__________________
|
|
May 21, 2013, 01:19 |
|
#12 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
Hi Bruno
It seems that the problem still exists. when I run the attached case in parallel I still see the reported problem in this page. I have same problem with my case, when I run it with pimpleDyMFoam in parallel. has anybody found a solution for this problem? Best Regards, Marhamat |
|
May 21, 2013, 10:18 |
|
#13 | |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Dear BRUNO:
Thanks so much for your reply, what your mention is right. I attached a different case, which is different with my orginal case because its size is small enough to attach. I will try the case you attached, and give you feedback ASAP. 3X Quote:
|
||
May 21, 2013, 17:44 |
|
#14 | ||
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
@Marhamat: Quote:
@Xinguang: Quote:
Best regards, Bruno
__________________
|
|||
May 21, 2013, 22:40 |
|
#15 |
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 17 |
Hey Bruno:
Many thanks for your reply and help. I have test in 2.2.0 and it works in this way. However, I found another bug in this case. When I reconstuctPar -lastestTime, and then I decomposePar it Code:
Decomposing mesh region0 Create mesh Calculating distribution of cells Selecting decompositionMethod simple Finished decomposition in 0.01 s Calculating original mesh data Distributing cells to processors Distributing faces to processors Distributing points to processors Constructing processor meshes Processor 0 Number of cells = 4000 Number of faces shared with processor 1 = 160 Number of faces shared with processor 2 = 250 Number of processor patches = 2 Number of processor faces = 410 Number of boundary faces = 1210 Processor 1 Number of cells = 4000 Number of faces shared with processor 0 = 160 Number of faces shared with processor 3 = 250 Number of processor patches = 2 Number of processor faces = 410 Number of boundary faces = 1210 Processor 2 Number of cells = 4000 Number of faces shared with processor 0 = 250 Number of faces shared with processor 3 = 80 Number of faces shared with processor 4 = 250 Number of processor patches = 3 Number of processor faces = 580 Number of boundary faces = 1180 Processor 3 Number of cells = 4000 Number of faces shared with processor 1 = 250 Number of faces shared with processor 2 = 80 Number of faces shared with processor 5 = 250 Number of processor patches = 3 Number of processor faces = 580 Number of boundary faces = 1180 Processor 4 Number of cells = 4000 Number of faces shared with processor 2 = 250 Number of faces shared with processor 5 = 160 Number of processor patches = 2 Number of processor faces = 410 Number of boundary faces = 1210 Processor 5 Number of cells = 4000 Number of faces shared with processor 3 = 250 Number of faces shared with processor 4 = 160 Number of processor patches = 2 Number of processor faces = 410 Number of boundary faces = 1210 Number of processor faces = 1400 Max number of cells = 4000 (0% above average 4000) Max number of processor patches = 3 (28.5714% above average 2.33333) Max number of faces between processors = 580 (24.2857% above average 466.667) Time = 0.08 --> FOAM FATAL IO ERROR: size 0 is not equal to the given value of 121 file: /home/cui/OpenFOAM/cui-2.2.0/run/test1/movingCyl1_22x/0.08/pointMotionU.boundaryField.cubeY from line 45 to line 51. From function Field<Type>::Field(const word& keyword, const dictionary&, const label) in file /opt/openfoam220/src/OpenFOAM/lnInclude/Field.C at line 236. FOAM exiting Last edited by wyldckat; May 22, 2013 at 18:49. Reason: Added the [CODE] delimiters |
|
May 22, 2013, 02:18 |
|
#16 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
Dear Bruno
Now when I run the attached case "movingCyl1_22x.tar.gz" on OpenFOAM 2.1.1. by using the Code: ./Allrun I get the below error: Code:
*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.1-221db2718bbb Exec : pimpleDyMFoam -parallel Date : May 22 2013 Time : 02:08:08 Host : "hydrocoeff-System-Product-Name" PID : 11868 Case : /home/hydrocoeff/Downloads/movingCyl1_22x nProcs : 4 Slaves : 3 ( "hydrocoeff-System-Product-Name.11869" "hydrocoeff-System-Product-Name.11870" "hydrocoeff-System-Product-Name.11871" ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh dynamicMotionSolverFvMesh // using new solver syntax: cellMotionU { solver PCG; preconditioner DIC; tolerance 1e-08; relTol 0; } // using new solver syntax: motionU { solver PCG; preconditioner DIC; tolerance 1e-06; relTol 0; } Selecting motion solver: velocityLaplacian [0] [0] [0] --> FOAM FATAL IO ERROR: [0] keyword diffusivity is undefined in dictionary "/home/hydrocoeff/Downloads/movingCyl1_22x/processor0/constant/dynamicMeshDict" [0] [0] file: /home/hydrocoeff/Downloads/movingCyl1_22x/processor0/constant/dynamicMeshDict from line 18 to line 31. [0] [0] From function dictionary::lookupEntry(const word&, bool, bool) const[3] [3] [3] --> FOAM FATAL IO ERROR: [3] keyword diffusivity is undefined in dictionary "/home/hydrocoeff/Downloads/movingCyl1_22x/processor3/constant/dynamicMeshDict" [3] [3] file: /home/hydrocoeff/Downloads/movingCyl1_22x/processor3/constant/dynamicMeshDict from line 0 to line 0. [3] [3] From function dictionary::lookupEntry(const word&, bool, bool) const [3] in file db/dictionary/dictionary.C at line 400. [3] FOAM parallel run exiting [3] [0] in file db/dictionary/dictionary.C at line 400. [0] FOAM parallel run exiting [0] -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them. -------------------------------------------------------------------------- [1] [1] [2] [2] [2] --> FOAM FATAL IO ERROR: [1] --> FOAM FATAL IO ERROR: . . . Marhamt Last edited by wyldckat; May 22, 2013 at 18:50. Reason: Added the [CODE] delimiters |
|
May 22, 2013, 05:40 |
|
#17 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
By updating my OF version to OF-2.2.0, now I can run the attached case in parallel. but in my own case I get the below error:
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh dynamicMotionSolverFvMesh Selecting motion solver: velocityLaplacian [0] [0] [0] --> FOAM FATAL IO ERROR: [2] [2] [0] keyword velocityLaplacianCoeffs is undefined in dictionary "/home/hydrocoeff/Desktop/MyDocuments/pimpleDymFoam/Elips1Par/processor0/constant/dynamicMeshDict" [0] [0] file: /home/hydrocoeff/Desktop/MyDocuments/pimpleDymFoam/Elips1Par/processor0/constant/dynamicMeshDict from line 18 to line 23. [0] [0] From function dictionary::subDict(const word& keyword) const [0] in file db/dictionary/dictionary.C at line 608. [0] FOAM parallel run exiting . . . so what is the reason of this error? Thanks alot, Marhamat. Last edited by marhamat; May 23, 2013 at 02:48. |
|
May 22, 2013, 08:54 |
|
#18 |
Senior Member
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 17 |
By changing the dynamicMeshDic the problem solved.
Thanks, Marhamat |
|
May 22, 2013, 19:29 |
|
#19 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Marhamat and Xinguang,
Marhamat sent me a private message with pretty much the same problem that Xinguang has got right now. The problem is not an easy one to solve and attached is only the first part of the solution, namely a case that should work... but doesn't work because of the broken "libMyPolynomVelocity" library. I'm not sure when I'll be able to look into this library code... I'll try to look at it tomorrow. In the meantime, please study attached case file. And please also study the post from the second link in my signature... namely this one: How to post code using [CODE] Best regards, Bruno
__________________
|
|
May 26, 2013, 08:43 |
|
#20 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Marhamat and Xinguang,
I've finally managed to look at this and make things work. A description of the necessary changes:
---- edit: I had a look at how it would be possible to avoid the need for "preservePatches". From what I can understand, the problem is that the "libMyPolynomVelocity" library does not implement all of the necessary methods and constructors. Compare with the class "sixDoFRigidBodyDisplacementPointPatchVectorFi eld" of the same kind of mesh manipulation: Code:
src/postProcessing/functionObjects/forces/pointPatchFields/derived/sixDoFRigidBodyDisplacement/sixDoFRigidBodyDisplacementPointPatchVectorField.H src/postProcessing/functionObjects/forces/pointPatchFields/derived/sixDoFRigidBodyDisplacement/sixDoFRigidBodyDisplacementPointPatchVectorField.C Best regards, Bruno
__________________
Last edited by wyldckat; May 26, 2013 at 09:00. Reason: I had forgotten that dynamic meshes are automatically reconstructed by decomposePar! - Also see "edit:" |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Other] mesh airfoil NACA0012 | anand_30 | OpenFOAM Meshing & Mesh Conversion | 13 | March 7, 2022 17:22 |
[blockMesh] non-orthogonal faces and incorrect orientation? | nennbs | OpenFOAM Meshing & Mesh Conversion | 7 | April 17, 2013 05:42 |
[blockMesh] error message with modeling a cube with a hold at the center | hsingtzu | OpenFOAM Meshing & Mesh Conversion | 2 | March 14, 2012 09:56 |
[blockMesh] BlockMesh FOAM warning | gaottino | OpenFOAM Meshing & Mesh Conversion | 7 | July 19, 2010 14:11 |
[blockMesh] Axisymmetrical mesh | Rasmus Gjesing (Gjesing) | OpenFOAM Meshing & Mesh Conversion | 10 | April 2, 2007 14:00 |