CFD Online Discussion Forums - problems with DSMC in parallel

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - problems with DSMC in parallel (https://www.cfd-online.com/Forums/openfoam-solving/114382-problems-dsmc-parallel.html)

problems with DSMC in parallel

hi all
I have a case and decide solve with dsmc when I run my case in the parallel or one core of my cpu I face this error:

Quote:

mpirun noticed that process rank 2 with PID 2071 on node hadi.msi exited on signal 9 (Killed).

one thing that I forgot say:
I run this case in a 32 bit linux without any error but when I run in a 64 bit linux I face this error

Hi Hadi,

You haven't provided enough information in order to help you. What were the messages that showed up before that?

Best regards,
Bruno

this error in the log.dsmcFoam file:

Quote:

and this in the log.dsmcInitialise file:

Quote:

and this is in the log.reconstructPar file:

Quote:

Hi Hadi,

Once it crashes on dsmcInitialise, everything else will not work.
I've made quick tests on the tutorials and for this application, it should output something like this:

Code:

Create time



Create mesh for time = 0



Initialising dsmc for Time = 0





Constructing constant properties for

    N2

    O2



Initialising particles



Total number of molecules added: 20984





ClockTime = 0 s



End



Finalising parallel run

Which means that your application crashed before being able to add all of the molecules.

A few possibilities come to mind:

Check if the folder "processor0/0/lagrangian/dsmc" exists and if it has got anything inside it. If it does not, try running the following command:

Code:

mkdir -p processor0/0/lagrangian/dsmc
On which machine was the mesh generated? And where was the case decomposed?
I ask this because if you did this in the 32bit machine, and then copied the case to the 64bit machine, then:
1. You might have incompatible access permissions to the files on the 64bit machine. For example, if the case was executed with "root" permissions on 32bit, but then with normal user permissions on 64bit. The test on #1 should indicate this. You can further confirm this by running the following command inside your case folder:
  
  Code:
  
  ls -l processor0
2. Or you might need to do the steps of mesh generation and decomposition once again on the 64bit machine.

Best regards,
Bruno

thanks Wyldckat
I check it and put the result here

hi
I have a case that a flow pass over a cube that creat its mesh with gambit and convert to OpenFoam but the all of molcule of gas not add in the dsmcInitialise
I try some thing but not answer
I appreciate for any help

Hi Hadi,

I re-read the whole thread and this looks like to be the same problem. And unfortunately, it's not enough information yet to figure out what might be wrong.

Therefore, here are a few questions:

How exactly did you build/install OpenFOAM on your current machine?
Did you do any modifications to OpenFOAM's source code?
What were the exact steps you've taken to convert the mesh and then running the case?
And were these steps all performed on the same machine with the same OpenFOAM version?
What does checkMesh tell you about your converted mesh? More specifically:

Code:

checkMesh -allGeometry -allTopology
Can you reproduce this error with one of OpenFOAM's own tutorial cases?

Best regards,
Bruno

Quote:

Originally Posted by wyldckat (Post 439571)

How exactly did you build/install OpenFOAM on your current machine?
Did you do any modifications to OpenFOAM's source code?
What were the exact steps you've taken to convert the mesh and then running the case?
And were these steps all performed on the same machine with the same OpenFOAM version?
What does checkMesh tell you about your converted mesh? More specifically:

Code:

checkMesh -allGeometry -allTopology
Can you reproduce this error with one of OpenFOAM's own tutorial cases?

Best regards,
Bruno

thanks Wyldycat for your reply
1-copy-paste this orders in the OpenFOAMwiki an install OpenFOAM2.1.1 for fedora 17
2-No
3-I create my mesh with gambit in the windoes that my case a cube that defined as wall and then put it on a big cube for domain and left face of cube is defined as inlet and right face outlet and the other faces of big cube are outlet2(outlet from besides) then in the my fedora with this order fluent3DMeshtoFoam convert my mesh and befor these I copy supersonic folder and then change name of folder to my case then delete the BlockMes and Boundery in the PolyMesh then copy my .msh file and then copy to my folder and then convert then with the bounderyfile that's creat after the convert of mesh to Edit the 0 folder then select my case and Edit propertis in the costant folder and system folder then delete script that excute the BlockMesh in the Allrun file and save it then I creat my dsmcSigma TcR Max then in the terminal run this order ./Allrun
4-I performed all these steps in my netbook because I have windoes and linux together,first I decide run this case in the my netbook and solve errors of my case when I solve errors of my case after it run in a supercomputer and in the both of them I use OpenFOAM2.1.1
5-when I checkmesh at the end of that say Mesh OK.

Quote:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / 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 : checkMesh -allGeometry -allTopology
Date : Jul 23 2013
Time : 12:30:56
Host : "hadiAz"
PID : 2481
Case : /home/hadiaz/OpenFOAM/OpenFOAM-2.1.1/tutorials/discreteMethods/dsmcFoam/cube
nProcs : 1
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 polyMesh for time = 0

Time = 0

Mesh stats
points: 209952
faces: 607800
internal faces: 586200
cells: 199000
boundary patches: 4
point zones: 0
face zones: 1
cell zones: 1

Overall number of cells of each type:
hexahedra: 199000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Topological cell zip-up check OK.
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology Bounding box
Outlet2 16000 16200 ok (non-closed singly connected) (-10 -10 -10) (22 10 10)
Outlet 2500 2601 ok (non-closed singly connected) (22 -10 -10) (22 10 10)
Inlet 2500 2601 ok (non-closed singly connected) (-10 -10 -10) (-10 10 10)
wall 600 602 ok (closed singly connected) (-2 -2 -2) (2 2 2)

Checking geometry...
Overall domain bounding box (-10 -10 -10) (22 10 10)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (1.688142938e-17 -1.044207159e-16 -3.088289655e-16) OK.
Max cell openness = 2.602085214e-16 OK.
Max aspect ratio = 1.00000016 OK.
Minumum face area = 0.159999996. Maximum face area = 0.160000004. Face area magnitudes OK.
Min volume = 0.0639999984. Max volume = 0.0640000016. Total volume = 12736. Cell volumes OK.
Mesh non-orthogonality Max: 9.155702348e-06 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 1.491672516e-07 OK.
Coupled point location match (average 0) OK.
Face tets OK.
Min/max edge length = 0.39999999 0.40000001 OK.
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All face flatness OK.
Cell determinant (wellposedness) : minimum: 1 average: 7.573025126
Cell determinant check OK.
Concave cell check OK.

Mesh OK.

End

6-when I run the sample of dsmc in the OpenFOAM without any error is run
I have a question:
1-the unit of gambit is mm and the dimensions of my case is mm,after convert my mesh is necessary change of unit(i.e. convert to meter)?
when I run creat processor 0-3 and in the bounderys condition(i.e. U , T and other )write nonuniform in the inlet and outlet

no body here can help me

Hi Hadi,

Sorry, I've been very busy for the past few weeks and didn't manage to have time to even login on the forum.

OK, I've read the detailed post and the first thing that comes to mind is indeed the problems with the units of the mesh.
You wrote that the mesh made with Gambit is in millimetre, which possibly means that you still need to convert the units. So, if we look at the output from checkMesh, this is shown:

Code:

Overall domain bounding box (-10 -10 -10) (22 10 10)

Are these values in metre or millimetre?

The second thing that comes to mind to ask is: what's the exact command you used to convert the mesh from Gambit format to OpenFOAM format?

Best regards,
Bruno

hi Mr santos
thanks and I hope you always healthy

somebody say gambit is non-dimensional and when you decide process with fluent(i.e you can select in or mm or m in the Fluent) or OpenFoam you must identify the unit of case

1-this values in millimetre
2-I write this:

Quote:

fluent3DMeshtoFoam cube.msh

Hi Hadi,

OK, then use the following command:

Code:

fluent3DMeshToFoam -scale 0.001 cube.msh

Then try running up to and including dsmcInitialise in parallel, to first confirm if it worked well or not, before launching the solver itself.

Keep in mind that almost all OpenFOAM applications have the option "-help":

Code:

fluent3DMeshToFoam -help

Best regards,
Bruno

thanks so much

It's work with any error
problem was in the scale
I wish you all the best.

:eek: I'm very glad it's finally working! All the best to you too!