[ChrisPro]

Hey All!

I'm trying to do some parallel calculations.
I've access to several computers. Each of them has 6 processors.

For testing I'm running the motorBike tutorial.

So when I want to use 12 processors, how do I have to set "n" in hierarchicalCoeffs?

Originally: (3 2 1) <== with 6 processors

I read the user guide, but couldn't find the right solution, because e.g. (6 4 2) doesn't work.

greets
Christian

[megacrout]

Well, if you need 12 subdomains, (6 4 2) is obviously not going to work, as it leads to 6*4*2=48 subdomains. Use e.g. (3 4 1) instead.

I do not know what your conditions and geometry are, so make sure that your decomposition is meaningful. A (6 2 1) or even (12 1 1) decomposition might turn out to be more suited.

As for how to make your computer understand it has to use processors on several computers, I can unfortunately not help. It might work automatically as soon as the computers are connected to each other through the same server. Just give it a shot, I guess =D

Tibo

[romant]

Originally Posted by megacrout

As for how to make your computer understand it has to use processors on several computers, I can unfortunately not help. It might work automatically as soon as the computers are connected to each other through the same server. Just give it a shot, I guess =D

Tibo

You can also use the scotch method, which will decrease the number of processor patches to a minimum and also balances the number of cells to the processors. In this case you don't need to state in which direction you want to decompose.

optionally you can then state a processor weight, for example if you have different computers (different cpu's ...) then you can state that one processor has more weight than another.

in order to get this working on more than one computer, check out any mpi tutorial that explains on how to set up automatic ssh login by sharing keys and so on.

[Phicau]

Hi

I recommend you to use Scotch decomposition method if you are unsure about the suitability of Hierarchical.

If you encounter any problems with running in parallel you should check out mpi machinefile options.

Best

[ChrisPro]

thanks for your replies!!

it worked so far! except, when I use more then 6 processors (doesn't matter if all on the same machine or split to others) the computer crashes.


AND when i want to run potentialFoam in parallel it always prints the error:

Reading field p

[0] 
[0] 
[0] --> FOAM FATAL IO ERROR: 
[0] keyword motorBike_frt-fairing:001%1 is undefined in dictionary "/home/lav09/prosch/OpenFOAM/prosch-2.0.1/run/motorBike/processor0/0/p::boundaryField"
[0] 
[0] file: /home/lav09/prosch/OpenFOAM/prosch-2.0.1/run/motorBike/processor0/0/p::boundaryField from line [1] 
[1] 
[1] 26 to line 53.
[0] 
[0]     From function dictionary::subDict(const word& keyword) const
[0]     in file db/dictionary/dictionary.C at line 461.
[0] 
FOAM parallel run exiting

and for all other processorfolder too.

Do I have set some special options in decomposePar or snappyHexMesh?
I tried all I could see in the help files, but always get the same error.

greets

[wyldckat]

Greetings to all!

@ChrisPro: why do I have the feeling that you are trying to use the motorBike case from an older version of OpenFOAM on the newer 2.0.1!? That error message indicates that the mesh that has been created has patches that are not present in the "0/p" field! If you are not using the motorBike case from 2.0.1, you better compare your modified case with the one in 2.0.1!

If this is not the case, please gives us a (short) step-by-step list of what you are doing, so it'll be easier for us to test it ourselves or at least diagnose what might be missing

Best regards,
Bruno

[ChrisPro]

hey! sorry for the late answer.

I tried the same thing on several computers but always get the same error.
I made sure, using the newest version of openFoam AND the tutorials.


Here is what i do in the motorBike example:
making a file called machines where the computername and the number of processors is in.

running blockMesh

decomposePar <== works

mpirun --hostfile machines -np 4 snappyHexMesh -overwrite -parallel > log & (here on a machine with 4 processors) <== works

mpirun --hostfile machines -np 4 potentialFoam -noFunctionObjects -writep -parallel > log &
this displays the error:

[0] 
[0] --> FOAM FATAL IO ERROR: 
[0] keyword motorBike_frt-fairing:001%1 is undefined in dictionary "/home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor0/0/p::boundaryField"
[0] 
[0] file: /home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor0/0/p::boundaryField from line 26 to line 53.
[0] 
[0]     From function dictionary::subDict(const word& keyword) const
[0]     in file db/dictionary/dictionary.C at line 461.
[0] 
FOAM parallel run exiting
[0] 
[2] 
[2] 
[2] --> FOAM FATAL IO ERROR: 
[2] keyword motorBike_frt-fairing:001%1 is undefined in dictionary "/home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor2/0/p::boundaryField"
[2] 
[2] file: /home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor2/0/p::boundaryField from line 26 to line 53.
[2] 
[2]     From function dictionary::subDict(const word& keyword) const
[2]     in file db/dictionary/dictionary.C at line 461.
[2] 
FOAM parallel run exiting
[2] 
--------------------------------------------------------------------------
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.
--------------------------------------------------------------------------
[3] 
[3] 
[3] --> FOAM FATAL IO ERROR: 
[3] keyword motorBike_frt-fairing:001%1 is undefined in dictionary "/home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor3/0/p::boundaryField"
[3] 
[3] file: /home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor3/0/p::boundaryField from line 26 to line 53.
[3] 
[3]     From function dictionary::subDict(const word& keyword) const
[3]     in file db/dictionary/dictionary.C at line 461.
[3] 
FOAM parallel run exiting
[3] 
[1] 
[1] 
[1] --> FOAM FATAL IO ERROR: 
[1] keyword motorBike_frt-fairing:001%1 is undefined in dictionary "/home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor1/0/p::boundaryField"
[1] 
[1] file: /home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike/processor1/0/p::boundaryField from line 26 to line 53.
[1] 
[1]     From function dictionary::subDict(const word& keyword) const
[1]     in file db/dictionary/dictionary.C at line 461.
[1] 
FOAM parallel run exiting
[1] 
--------------------------------------------------------------------------
mpirun has exited due to process rank 0 with PID 4825 on
node ubuntu exiting without calling "finalize". This may
have caused other processes in the application to be
terminated by signals sent by mpirun (as reported here).
--------------------------------------------------------------------------
[ubuntu:04824] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
[ubuntu:04824] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

log file:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.0-0bc225064152
Exec   : potentialFoam -noFunctionObjects -writep -parallel
Date   : Dec 25 2011
Time   : 21:56:27
Host   : "ubuntu"
PID    : 4825
Case   : /home/christian/OpenFOAM/christian-2.1.0/run/Test/motorBike
nProcs : 4
Slaves : 
3
(
"ubuntu.4826"
"ubuntu.4827"
"ubuntu.4828"
)

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

Reading field p

do I have to change things in the processor folders?

greets
Christian

[wyldckat]

Hi Christian,

OK, I managed to reproduce the same error you got. But I don't have time right now to figure out how to fix this.
My suggestion is that you check the "turbineSiting" tutorial:

• 2.0.x: https://github.com/OpenFOAM/OpenFOAM.../turbineSiting
• 2.1.x: https://github.com/OpenFOAM/OpenFOAM.../turbineSiting

Good luck!
Bruno

[ChrisPro]

I tried the tutorial, but even when I do not change anything in the tutorial, snappyHexMesh reports an error, that the ptscotch library has to be installed.
but ptscotch isn't used when snappyHexMesh is executed!

Shell refinement iteration 4
----------------------------

Marked for refinement due to refinement shells    : 3818 cells.
Determined cells to refine in = 0.05 s
Selected for internal refinement : 4204 cells (out of 73632)
Edge intersection testing:
    Number of edges             : 334730
    Number of edges to retest   : 108544
    Number of intersected edges : 18230
Refined mesh in = 0.58 s
[1] 
[1] 
[1] --> FOAM FATAL ERROR: 
[1] You are trying to use ptscotch but do not have the ptscotchDecomp library loaded.
This message is from the dummy ptscotchDecomp stub library instead.

Please install ptscotch and make sure that libptscotch.so is in your LD_LIBRARY_PATH.
The ptscotchDecomp library can then be built in $FOAM_SRC/parallel/decompose/ptscotchDecomp
[1]

[wyldckat]

Yeah, that's one of those crazy bugs I thought that they had fixed that in 2.1.0, but I haven't confirmed this yet.

You might want to report this on the bug tracker: http://www.openfoam.com/mantisbt/ - I haven't reported it because I keep forgetting about it

[ChrisPro]

ok!
just reported it!

[wyldckat]

Hi Christian,

OK, I've managed to solve the problem with running motorBike in parallel, namely the problem you had in post #7.

The attached case has only been tested with OpenFOAM 2.0.x. Basically the problem is that decomposePar does not preserve the regular expressions that are present in the original boundaries (p, U, k, omega, nut). So the solution that I implemented resorts to changeDictionary to reinstate the missing boundaries, as well as add ones that were missing from the decomposition and parallel meshing.
It's not the perfect solution, but it's a start.

As for the ptscotch problem, I've seen your report and I'am wandering which were the steps you took for installing OpenFOAM. Was is it the Debian packages one? (this one: http://www.openfoam.org/download/ubuntu.php)

Best regards,
Bruno

[ChrisPro]

Oh yeah Bruno! you're my man!
I tested it on openfoam 2.1.0 and it works!!
Thanks a lot!!

But how do you reconstruct the Case?

when i use reconstructPar the following Error message is displayed:

Create time

Create mesh for time = 0

Time = 100

Reconstructing FV fields



--> FOAM FATAL ERROR: 
Size of maps does not correspond to size of mesh for processor 0
faceProcAddressing : 1112 nFaces : 276200
cellProcAddressing : 320 nCell : 86070
boundaryProcAddressing : 7 nFaces : 74

    From function fvFieldReconstructor::fvFieldReconstructor
(
   fvMesh&,
   const PtrList<fvMesh>&,
   const PtrList<labelIOList>&,
   const PtrList<labelIOList>&,
   const PtrList<labelIOList>&
)
    in file fvFieldReconstructor.C at line 66.

FOAM exiting

I tried the additional options of reconstructPar, but no one of them worked.


I downloaded the file ptscotch library from:
http://packages.debian.org/sid/libptscotch-5.1

greets
Christian

[wyldckat]

Hi Christian,

The problem is rather simple when we think about it: since we generated the mesh in parallel, said mesh doesn't exist in reconstructed form!

The following commands are meant to be placed at the end of Allrun:

runApplication reconstructParMesh -mergeTol 1e-6 -constant
runApplication reconstructPar

The other reason why I didn't bother thinking about reconstructing the case was because I usually use ParaView's internal reader:

paraFoam -builtin

The internal reader provides an option for showing the decomposed results

By the way, you might also be interested in the new tutorial available for 2.1.0: "incompressible/pisoFoam/les/motorBike/motorBike" - this is another variant of the "motorBike" case we know, but it is meshed in parallel with 8 cores with a higher mesh resolution and is quite the memory eater. 2.7GiB of RAM weren't enough to feed this beast of a mesh!

edit: I forgot to ask - Which version of Linux and architecture are you using? For the architecture, you can check by running:

uname -m

And which exact instructions did you use to install OpenFOAM? This way it'll be easier to try and figure out why you didn't have a working ptscotch library, since if we know which steps you took, we can try them out ourselves and check what might have happened.

Best regards,
Bruno

[ChrisPro]

First: Happy New Year!!

oh thanks a lot!!! that worked fine, with your motorbike example.

but what exaclty is procBoundary? and why did you set the velocity in the changeDictionaryDict file for procBoundary?

I adapted this example to my case. It works and i get a good residual. But in my case I simulate the flow through a rather complex geometrie where all boundaries are given by stl files, even the inlet and the outlet. I set the pressure at the inlet and outlet and the velocity is calculated with "pressureDirectedInletVelocity". The pressure at the inlet is 10Pa and at the outlet 0Pa.

when I calculate this the normal way, with only a single processor, everithing is fine. But in parallel the starting (Time 0) boundary conditions are so that there is a pressure of 10Pa at the inlet and outlet.
The changeDictionaryDict has exactly the same adjustments as the single files for p, U,... except for the additional procBoundary

dictionaryReplacement
{
    p
    {
        boundaryField
        {
            "wall_.*"
            {
                type            zeroGradient;
            }

			"inlet_.*"
			{
				type			fixedValue;
				value			uniform 10;	
			}
			
			"outlet_.*"
			{
				type            fixedValue;
        		value           uniform 0;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    U
    {
        boundaryField
        {
            "inlet_.*"
			{
				type			pressureDirectedInletVelocity;
				value			(0 0 0);
				inletDirection	uniform (0 -1 0);
			}

			"outlet_.*"
			{
				type			pressureInletOutletVelocity;
				value           uniform (0 0 0);
			}

			"wall_.*"
			{
				type            fixedValue;
				value           uniform (0 0 0);
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform (0 0 0);
            }
        }
    }


    omega
    {
        boundaryField
        {
            "wall_.*"
            {
                type            omegaWallFunction;
                value           1.78;
            }

			"outlet_.*"
			{
				type            inletOutlet;
				inletValue      1.78;
				value           1.78;
			}

			"inlet_.*"
			{
				type  			fixedValue;
				value 			1.78;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 1.78;
            }
        }
    }

    nut
    {
        boundaryField
        {
            "wall_.*"
            {
                type            nutkWallFunction;
                value           uniform 0;
            }

			"inlet_.*"
			{
				type            calculated;
				value           uniform 0;
			}

			"outlet_.*"
			{
				type            calculated;
				value           uniform 0;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    k
    {
        boundaryField
        {
            "wall_.*"
            {
                type            kqRWallFunction;
                value           0.24;
            }

			"outlet_.*"
			{
				type            inletOutlet;
				inletValue      0.24;
				value           0.24;
			}

			"inlet_.*"
			{
				type  fixedValue;
				value 0.24;
			}


            "procBoundary.*"
            {
                type            processor;
                value           uniform 0.24;
            }
        }
    }
}

// ************************************************************************* //

what do I make wrong?


Yes the pisoForm motorbike example looks quite interesting, but I still get this dam ptscotch error which we talked about some posts before.
Maybe I really made something wrong installing OpenFoam but I excactly followed the instructions on OpenFoam.com for Ubuntu http://www.openfoam.org/download/ubuntu.php
So I'm using Ubuntu 10.04LTS on a x86_64

How did you install the ptscotch library? and where are the correct files to download?

regards
Christian

[wyldckat]

Hi Christian,

Originally Posted by ChrisPro

First: Happy New Year!!

Happy New Year

Originally Posted by ChrisPro

but what exaclty is procBoundary? and why did you set the velocity in the changeDictionaryDict file for procBoundary?

potentialFoam complained that these boundaries didn't exist. They basically define the boundaries for the interfacing zones between processors, aka parallel processes. All of the values in "changeDictionaryDict" were collected from the files at "0.org" and "processor0/0/". It looked like this dictionary can't handle the "#include" functionality, so that is why I had to hard-code those values as new.
Oh, and these values between processors seem to be the same as the initial internal fields.

Originally Posted by ChrisPro

I adapted this example to my case. It works and i get a good residual. But in my case I simulate the flow through a rather complex geometrie where all boundaries are given by stl files, even the inlet and the outlet. I set the pressure at the inlet and outlet and the velocity is calculated with "pressureDirectedInletVelocity". The pressure at the inlet is 10Pa and at the outlet 0Pa.

when I calculate this the normal way, with only a single processor, everithing is fine. But in parallel the starting (Time 0) boundary conditions are so that there is a pressure of 10Pa at the inlet and outlet.
The changeDictionaryDict has exactly the same adjustments as the single files for p, U,... except for the additional procBoundary

dictionaryReplacement
{
    p
    {
        boundaryField
        {
            "wall_.*"
            {
                type            zeroGradient;
            }

            "inlet_.*"
            {
                type            fixedValue;
                value            uniform 10;    
            }
            
            "outlet_.*"
            {
                type            fixedValue;
                value           uniform 0;
            }

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    U
    {
        boundaryField
        {
            "inlet_.*"
            {
                type            pressureDirectedInletVelocity;
                value            (0 0 0);
                inletDirection    uniform (0 -1 0);
            }

            "outlet_.*"
            {
                type            pressureInletOutletVelocity;
                value           uniform (0 0 0);
            }

            "wall_.*"
            {
                type            fixedValue;
                value           uniform (0 0 0);
            }

            "procBoundary.*"
            {
                type            processor;
                value           uniform (0 0 0);
            }
        }
    }


    omega
    {
        boundaryField
        {
            "wall_.*"
            {
                type            omegaWallFunction;
                value           1.78;
            }

            "outlet_.*"
            {
                type            inletOutlet;
                inletValue      1.78;
                value           1.78;
            }

            "inlet_.*"
            {
                type              fixedValue;
                value             1.78;
            }

            "procBoundary.*"
            {
                type            processor;
                value           uniform 1.78;
            }
        }
    }

    nut
    {
        boundaryField
        {
            "wall_.*"
            {
                type            nutkWallFunction;
                value           uniform 0;
            }

            "inlet_.*"
            {
                type            calculated;
                value           uniform 0;
            }

            "outlet_.*"
            {
                type            calculated;
                value           uniform 0;
            }

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    k
    {
        boundaryField
        {
            "wall_.*"
            {
                type            kqRWallFunction;
                value           0.24;
            }

            "outlet_.*"
            {
                type            inletOutlet;
                inletValue      0.24;
                value           0.24;
            }

            "inlet_.*"
            {
                type  fixedValue;
                value 0.24;
            }


            "procBoundary.*"
            {
                type            processor;
                value           uniform 0.24;
            }
        }
    }
}

// ************************************************************************* //

what do I make wrong?

Mmm, I'd check what values decomposePar distributed for "procBoundary0to1" and similar name at "processor*/0/".

Originally Posted by ChrisPro

Yes the pisoForm motorbike example looks quite interesting, but I still get this dam ptscotch error which we talked about some posts before.
Maybe I really made something wrong installing OpenFoam but I excactly followed the instructions on OpenFoam.com for Ubuntu http://www.openfoam.org/download/ubuntu.php
So I'm using Ubuntu 10.04LTS on a x86_64

How did you install the ptscotch library? and where are the correct files to download?

That's the thing, it should be installed automatically when you install the "openfoam210" package! The "libptscotch" package is one of the required packages and should have been installed directly and automatically from Ubuntu's repositories, without the need to resort to Debian's repositories

I'm checking this in a virtual machine with the same version of Ubuntu 10.04 x86_64 to confirm what's going on... I'll edit this post after I have results.

edit: preliminary tests indicated that the relevant package is only recommended. Said package still needs to be installed manually, at least for 10.04:

sudo apt-get install libptscotch-dev

You'll probably need to remove the one you currently have from Debian.

edit 2: OK, now I understand why you went to Debian for the package. And wouldn't you know it, since there is no "libptscotch-dev" for 10.04, then there is no "libptscotchDecomp.so" for "openmpi-system"! Here are the commands for a possible proper installation:

1. Add the old FEniCS PPA and install their scotch libraries:

   sudo add-apt-repository ppa:fenics-packages/fenics-old
   sudo apt-get update
   sudo apt-get install libptscotch-dev

2. We'll have to go into root mode and build the essential packages:

   sudo -s
   . /opt/openfoam210/etc/bashrc
   src
   cd parallel
   ./Allwmake

3. If all goes well, you are ready to go!!

Best regards,
Bruno

[ChrisPro]

Hey!!
Yeah I managed to install the ptscotch library! Thank you!!

now, openmpi works really well.

I'm running all functions now with the keyword mpirun, because there one has the option to make a "machines" file, where all computers and their cpus which are used for the calculations are listed.

Thats how my "Allrun" flie looks like now:

#!/bin/sh
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions

# copy flange surface from resources folder
#cp $FOAM_TUTORIALS/resources/geometry/flange.stl.gz constant/triSurface/

cp -r 0.org 0 > /dev/null 2>&1

runApplication blockMesh

runApplication surfaceFeatureExtract -includedAngle 150 -writeObj constant/triSurface/Wall.stl wall

runApplication decomposePar

runApplication mpirun --hostfile machines -np 4 snappyHexMesh -overwrite -parallel

#log Datei umbenennen:
mv log.mpirun log.snappyHexMesh

find . -type f -iname "*level*" -exec rm {} \;

ls -d processor* | xargs -i cp -r 0.org/* ./{}/0/ $1

#renumberMesh
runApplication mpirun --hostfile machines -np 4 renumberMesh -overwrite -parallel
mv log.mpirun log.renumberMesh
#potentialFoam
runApplication mpirun --hostfile machines -np 4 potentialFoam -initialiseUBCs -noFunctionObjects -parallel
mv log.mpirun log.potentialFoam
#simpleFoam
runApplication mpirun --hostfile machines -np 4 `getApplication` -parallel
mv log.mpirun log.simpleFoam

runApplication reconstructParMesh -mergeTol 1e-6 -constant
runApplication reconstructPar

Thanks again for your very useful help!!!
Christian

[xiaow_g]

Hi, Christian,
I have been working on the use on snappyHexMesh. About the running of motobike case, I have some problems:
In the "OpenFOAM-2.1.0/tutorials/incompressible/pisoFoam/les/motorBike/motorBike" directory, I didn't change anything. Then I run the commands according to the Allrun file, the commands list is as below:
"blockMesh",
"cp system/decomposeParDict.hierarchical system/decomposeParDict","decomposePar",
"cp system/decomposeParDict.ptscotch system/decomposeParDict",
"mpirun -np 8 snappyHexMesh -overwrite -parallel"
then it just got stuck at:

Overall mesh bounding box : (-5 -4 0) (15 4 8)
Relative tolerance : 1e-06
Absolute matching distance : 2.29783e-05


In fact I have tested many cases in OpenFOAM-2.1.0, all of them were stuck somewhere during their running, while they got stuck at different points. Do you know what's wrong with it?

Best wishes,
xiaow_g.

Originally Posted by ChrisPro

First: Happy New Year!!

oh thanks a lot!!! that worked fine, with your motorbike example.

but what exaclty is procBoundary? and why did you set the velocity in the changeDictionaryDict file for procBoundary?

I adapted this example to my case. It works and i get a good residual. But in my case I simulate the flow through a rather complex geometrie where all boundaries are given by stl files, even the inlet and the outlet. I set the pressure at the inlet and outlet and the velocity is calculated with "pressureDirectedInletVelocity". The pressure at the inlet is 10Pa and at the outlet 0Pa.

when I calculate this the normal way, with only a single processor, everithing is fine. But in parallel the starting (Time 0) boundary conditions are so that there is a pressure of 10Pa at the inlet and outlet.
The changeDictionaryDict has exactly the same adjustments as the single files for p, U,... except for the additional procBoundary

dictionaryReplacement
{
    p
    {
        boundaryField
        {
            "wall_.*"
            {
                type            zeroGradient;
            }

			"inlet_.*"
			{
				type			fixedValue;
				value			uniform 10;	
			}
			
			"outlet_.*"
			{
				type            fixedValue;
        		value           uniform 0;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    U
    {
        boundaryField
        {
            "inlet_.*"
			{
				type			pressureDirectedInletVelocity;
				value			(0 0 0);
				inletDirection	uniform (0 -1 0);
			}

			"outlet_.*"
			{
				type			pressureInletOutletVelocity;
				value           uniform (0 0 0);
			}

			"wall_.*"
			{
				type            fixedValue;
				value           uniform (0 0 0);
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform (0 0 0);
            }
        }
    }


    omega
    {
        boundaryField
        {
            "wall_.*"
            {
                type            omegaWallFunction;
                value           1.78;
            }

			"outlet_.*"
			{
				type            inletOutlet;
				inletValue      1.78;
				value           1.78;
			}

			"inlet_.*"
			{
				type  			fixedValue;
				value 			1.78;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 1.78;
            }
        }
    }

    nut
    {
        boundaryField
        {
            "wall_.*"
            {
                type            nutkWallFunction;
                value           uniform 0;
            }

			"inlet_.*"
			{
				type            calculated;
				value           uniform 0;
			}

			"outlet_.*"
			{
				type            calculated;
				value           uniform 0;
			}

            "procBoundary.*"
            {
                type            processor;
                value           uniform 0;
            }
        }
    }

    k
    {
        boundaryField
        {
            "wall_.*"
            {
                type            kqRWallFunction;
                value           0.24;
            }

			"outlet_.*"
			{
				type            inletOutlet;
				inletValue      0.24;
				value           0.24;
			}

			"inlet_.*"
			{
				type  fixedValue;
				value 0.24;
			}


            "procBoundary.*"
            {
                type            processor;
                value           uniform 0.24;
            }
        }
    }
}

// ************************************************************************* //

what do I make wrong?


Yes the pisoForm motorbike example looks quite interesting, but I still get this dam ptscotch error which we talked about some posts before.
Maybe I really made something wrong installing OpenFoam but I excactly followed the instructions on OpenFoam.com for Ubuntu http://www.openfoam.org/download/ubuntu.php
So I'm using Ubuntu 10.04LTS on a x86_64

How did you install the ptscotch library? and where are the correct files to download?

regards
Christian

[ChrisPro]

Hey!

when snappyHexMesh says something like: "aborted" or "killed"
then probably your memory is to low for that case. :/

greets
christian

[wyldckat]

Greetings to all!

@xiaow_g: I know I've had a similar problem, where snappyHexMesh kept running at 100% in parallel and wouldn't continue, but I can't remember what the problem was. It might be a memory issue like Chris said, but it could also be a bug you might be triggering somehow.

It would be useful to know the Linux distribution and architecture (uname -m) you are using, as well how much RAM is available to your Linux installation (in case you are running it inside a virtual machine).

The other possibility is that you need to upgrade to OpenFOAM 2.1.x. Several bugs have been fixed since 2.1.0 was released and I vaguely remember having problems with snappyHexMesh in parallel with one versions that wasn't from git...

Best regards,
Bruno