CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[snappyHexMesh] Snappy in parallel mode

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree9Likes
  • 1 Post By alexm
  • 8 Post By Tobi

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 27, 2009, 14:50
Default Snappy in parallel mode
  #1
New Member
 
Join Date: Oct 2009
Posts: 3
Rep Power: 16
jajoju is on a distinguished road
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
jajoju is offline   Reply With Quote

Old   October 27, 2009, 20:05
Default
  #2
New Member
 
Axel Mohr
Join Date: Mar 2009
Location: Kiel, Schleswig-Holstein, Germany
Posts: 24
Rep Power: 17
alexm is on a distinguished road
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
namsivag likes this.
alexm is offline   Reply With Quote

Old   October 28, 2009, 05:03
Default
  #3
New Member
 
Join Date: Oct 2009
Posts: 3
Rep Power: 16
jajoju is on a distinguished road
Hi Axel

thanks a lot it works!!! You really made my day!

best greetings Jakob
jajoju is offline   Reply With Quote

Old   December 3, 2014, 06:24
Default
  #4
New Member
 
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 11
estang is on a distinguished road
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.
This is the tree of one processor after snappyHexMesh has run
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
whats wrong?
estang is offline   Reply With Quote

Old   December 3, 2014, 11:48
Default
  #5
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Code:
reconstructParMesh -mergeTol 1e-6 -constant
Why you have to use it because you are using
Code:
mpirun -np x snappyHeMesh -parallel -overwrite
Therefor -overwrite tells sHM to overwrite the mesh in constant/polyMesh and therefor you will not get a time folder. Hence this happens reconstructParMesh is not able to reconstruct a mesh because it is searching in a time folder which you do not have. To avoid this error you have to tell the application that you want to reconstruct the mesh in constant folder.
namsivag, Yage, maminow and 5 others like this.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   December 4, 2014, 02:57
Thumbs up
  #6
New Member
 
Eugen
Join Date: Sep 2014
Posts: 18
Rep Power: 11
estang is on a distinguished road
you solved my problem
estang is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 03:43.