CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Sample utility problems (http://www.cfd-online.com/Forums/openfoam-solving/59748-sample-utility-problems.html)

msrinath80 January 2, 2007 13:10

For a large case (approx 11 mi
 
For a large case (approx 11 million cells) is it normal to expect the sample utility to take over 6 hours just to get some velocity values along a line?

msrinath80 January 2, 2007 13:10

Oh, and it's still not done af
 
Oh, and it's still not done after 6 hours.

mattijs January 2, 2007 13:38

Seems bit excessive. - Chec
 
Seems bit excessive.

- Check that your line is not along an edge or face of the mesh. This might cause tracking to fail.

- See if using a 'cloud' sampleSet instead of 'uniform' works. Cloud in your sampleDict takes a pointField:

cloud
{
points ((x y z) .. (x y z))
}

Either way I'd be interested in what the outcome is.

hannes January 3, 2007 04:12

Hello, I have experienced s
 
Hello,

I have experienced similar problems with the sample utility. The utility starts, the mesh is created and then it hangs.

When I kill it using Ctrl-C, the following stack trace is output:

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : sample .. F2LES_ini2 -latestTime
Date : Jan 03 2007
Time : 08:48:02
Host : palamedes.fms.uni-rostock.de
PID : 12428
Root : ..
Case : F2LES_ini2
Nprocs : 1
Create time

Create mesh for time = 1.01555

Time = 1.01555
Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::sigInt::sigIntHandler(int)
/lib64/libc.so.6 [0x39fea30210]
Foam::particle<foam::passiveparticle>::findFaces(F oam::Vector<double> const&)
Foam::particle<foam::passiveparticle>::trackToFace (Foam::Vector<double> const&, double&, bool)
sample [0x465596]
sample [0x466288]
sample [0x466c23]
sample [0x467751]
Foam::sampleSet::addwordConstructorToTable<foam::u niformset>::New(Foam::polyMesh const&, Foam::meshSearch&, Foam::dictionary const&)
sample [0x45cde7]
sample [0x43e854]
sample [0x41ad4c]
__libc_start_main
__gxx_personality_v0

It seems to get stuck in some kind of search procedure (Foam::particle<foam::passiveparticle>::findFaces) .

The problem first occured on a large case (16 Mio cells) but today also with a smaller one (500k cells).
Furthermore, the problem occurs only on 64bit machines. On 32bit computers, sample is working with the small case. (I could not try the large one, since we have only 64bit computers with enough memory for the 16 Mio case)

Regards, Hannes

mattijs January 3, 2007 16:46

This sounds as if your samplin
 
This sounds as if your sampling line is along a face. Just offset it a bit or do the cloud suggestion above and please let me know the outcome.

msrinath80 January 3, 2007 21:11

Apologies for the delayed repl
 
Apologies for the delayed reply Mattijs. Your cloud suggestion worked without any problems. It appears that the sample utility does not like my wall boundary located at y = 0.02 even when using cloud. Instead y = 0.0199999999 works. And yes, it took only 4 odd minutes now. The uniform option is however still not happy with y = 0.0199999999.

Thanks very much for your help Mattijs!

mattijs January 4, 2007 05:05

Move your sampling points a bi
 
Move your sampling points a bit more. Having y=0.0199999999 still sounds as if you've perturbed it by only a tiny amount. Think e.g. 0.1% of cell dimension.

hans_jonas April 10, 2007 21:35

Is there a way to sample data
 
Is there a way to sample data from moving walls?

I am working on fluid-structure interactions and I would like to plot the pressure distribution of an elastically-mounted cylinder (free moving in y direction with damping and spring). From the stationary cylinder case I use the sample utility with a cloud of points on the body surface but that does not work any more when the body is moving freely.

So I am looking for sample boundary patches or dumping it directly into a log-file (so fare I have not managed to write the pressure of the body patch).

hjasak April 11, 2007 01:27

Would writing all the face pre
 
Would writing all the face pressures from the moving patch be an option? The thing is that in a moving patch it is not easy to grab anything geometrically - because the patch is moving :-)

If you'd like the data from your patch, you can do something like (I am looking for a patch called "piston"):

label pistonPatchID =
mesh.boundaryMesh().findPatchID("piston");

if (pistonPatchID > -1)
{
Info << "face values" << p.boundaryField()[pistonPatchID] << endl;

else
{
Info << "Error: patch not found" << endl;
}
}

Hope you can follow this,

Hrv

mattijs April 11, 2007 17:25

Alternatively you could try th
 
Alternatively you could try the sampleSurface utility with constantPatch or interpolatedPatch. (see the sample dictionary in $FOAM_UTILITIES/postProcessing/miscellaneous/sampleSurface)

It should be able to handle moving meshes (not really tested though)

leonardo.morita April 30, 2009 09:32

Problem sampling UPrime2Mean
 
Hello,

In order not to create a new thread, I decided to ask for your help in this one, even though it's quite old...

My problem is the following: after having run the channelOodles tutorial, I'm trying to post-process it using the sample utility. Almost everything works fine until now, except the probe of UPrime2Mean...I receive the following error message:

m::error::printStack(Foam::Ostream&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::writer<Foam::SymmTensor<double> >::New(Foam::word const&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#4 void Foam::sampledSets::sampleAndWrite<Foam::SymmTensor <double> >(Foam::sampledSets::fieldGroup<Foam::SymmTensor<d ouble> >&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#5 Foam::sampledSets::write() in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#6 Foam::sampledSurfaces::read(Foam::dictionary const&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/sample"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::regIOobject::write() const in "/model/giampani/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/sample"
Incident de segmentation

Does anybody know what the cause of the problem may be?
Thank you.

Regards,

Leonardo

leonardo.morita May 12, 2009 11:08

Any suggestion?

cyang December 21, 2012 06:51

Leonardo, I met the same problem. Have you solved it?

Quote:

Originally Posted by leonardo.morita (Post 214776)
Hello,

In order not to create a new thread, I decided to ask for your help in this one, even though it's quite old...

My problem is the following: after having run the channelOodles tutorial, I'm trying to post-process it using the sample utility. Almost everything works fine until now, except the probe of UPrime2Mean...I receive the following error message:

m::error::printStack(Foam::Ostream&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::writer<Foam::SymmTensor<double> >::New(Foam::word const&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#4 void Foam::sampledSets::sampleAndWrite<Foam::SymmTensor <double> >(Foam::sampledSets::fieldGroup<Foam::SymmTensor<d ouble> >&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#5 Foam::sampledSets::write() in "/model/giampani/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#6 Foam::sampledSurfaces::read(Foam::dictionary const&) in "/model/giampani/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/sample"
#7 __libc_start_main in "/lib64/libc.so.6"
#8 Foam::regIOobject::write() const in "/model/giampani/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/sample"
Incident de segmentation

Does anybody know what the cause of the problem may be?
Thank you.

Regards,

Leonardo



All times are GMT -4. The time now is 05:44.