|
[Sponsors] |
October 27, 2009, 14:50 |
Snappy in parallel mode
|
#1 |
New Member
Join Date: Oct 2009
Posts: 3
Rep Power: 16 |
Hi everybody
i am new to OpenFOAM and snappyHexMesh. I need to create a mesh with a lot of cells (arround 8 Mio.) so I thought it would be usefull to use more than one cpu. I tried to generate the mesh with the help of several cpu in OpenFOAM 1.6.x. Everything went fine so far after: -blockMesh -decomposePar -mpirun -n 4 snappyHexMesh -parallel -reconstructParMesh (after I added master time 1 to the controlDict) If I open the mesh now in paraFoam I just can see the 'first mesh'. That means the surface is not smooth it's square cut (?). Does anybody know if the step with the 'master time' was right (after that it finished reconstructing the first time!)? Maybe there is another mistake I made. I really hope that someone can help me! Thanks a lot! Jakob |
|
October 27, 2009, 20:05 |
|
#2 |
New Member
Axel Mohr
Join Date: Mar 2009
Location: Kiel, Schleswig-Holstein, Germany
Posts: 24
Rep Power: 17 |
Hello Jakob,
I don't know what these 'master time' is you're about. Maybe there is another thing, I have to learn ;-) After a parallel run of snappyHexMesh in each processor folder are the the folders for the 'time steps' 1 + 2 + 3 (if add layers had been set in snappyHexMeshDict). For the smooth surface you need the second time step. Normaly reconstructPar - without any parameter - will reconstruct each time step in the processor folders. You should try reconstructPar -time 2 (or '-time 3' or '-latestTime') if you have problems, try this one: reconstructParMesh -mergeTol 1e-03 -latestTime Hope, that helps! Good night and greetings, Axel |
|
October 28, 2009, 05:03 |
|
#3 |
New Member
Join Date: Oct 2009
Posts: 3
Rep Power: 16 |
Hi Axel
thanks a lot it works!!! You really made my day! best greetings Jakob |
|
December 3, 2014, 06:24 |
|
#4 |
New Member
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 11 |
If i use reconstructPar without any parameters, it tells me that there is no times selected. If i run reconstructParMesh -mergeTol 1e-06 it tells me there is no mesh
Code:
Merge tolerance : 1e-06 Write tolerance : 1e-06 Doing geometric matching on correct procBoundaries only. This assumes a correct decomposition. Found 8 processor directories Reading database "snappyMultiRegionLayerMeshing_2/processor0" Reading database "snappyMultiRegionLayerMeshing_2/processor1" Reading database "snappyMultiRegionLayerMeshing_2/processor2" Reading database "snappyMultiRegionLayerMeshing_2/processor3" Reading database "snappyMultiRegionLayerMeshing_2/processor4" Reading database "snappyMultiRegionLayerMeshing_2/processor5" Reading database "snappyMultiRegionLayerMeshing_2/processor6" Reading database "snappyMultiRegionLayerMeshing_2/processor7" Time = 0 No mesh. End. Code:
├── processor7 │ ├── 0 │ │ ├── cellLevel │ │ └── pointLevel │ └── constant │ └── polyMesh │ ├── boundary │ ├── boundaryProcAddressing │ ├── cellLevel │ ├── cellProcAddressing │ ├── cellZones │ ├── faceProcAddressing │ ├── faces │ ├── faceZones │ ├── level0Edge │ ├── neighbour │ ├── owner │ ├── pointLevel │ ├── pointProcAddressing │ ├── points │ ├── pointZones │ ├── refinementHistory │ ├── sets │ │ └── wrongFaces │ └── surfaceIndex |
|
December 3, 2014, 11:48 |
|
#5 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 |
Code:
reconstructParMesh -mergeTol 1e-6 -constant Code:
mpirun -np x snappyHeMesh -parallel -overwrite
__________________
Keep foaming, Tobias Holzmann |
|
December 4, 2014, 02:57 |
|
#6 |
New Member
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 11 |
you solved my problem
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Unsteady Inlet Velocity UDF in Parallel Batch Mode | vtyler | Fluent UDF and Scheme Programming | 4 | April 1, 2020 06:44 |
UDF Fluent running in Parallel mode | Abhiroop | FLUENT | 2 | September 1, 2016 18:19 |
problem with compiling boundary condition udf in parallel mode | chem engineer | Fluent UDF and Scheme Programming | 11 | June 29, 2015 07:23 |
Does anyone have any experience with cfd-fastran (2008.2) on parallel mode? | CFD_1977 | Main CFD Forum | 0 | March 30, 2014 08:01 |
How to run icoFsiFoam in parallel mode? | AsDF | OpenFOAM Running, Solving & CFD | 2 | February 21, 2014 08:56 |