CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Problem with running chtMultiRegionFoam after using setSet utility

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

Like Tree2Likes
  • 2 Post By maddalena

Reply
 
LinkBack Thread Tools Display Modes
Old   November 19, 2009, 05:24
Default Problem with running chtMultiRegionFoam after using setSet utility
  #1
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 6
Victor is on a distinguished road
Hi at all,

as a Open-FOAM-beginner, i tried to use chtMultiregionFoam-solver as it is used in the HeatTransfer Tutorial Case. In my case,there is a part in the middle of the body that is cut out by the setSet utility in order to simulate a solid. After running blockMesh, setSet, setsToTones, splitMeshRegions without any errors the case allways stops,when running the chtMultiRegionFoam solver:

/OpenFOAM-1.6/bin/tools/RunFunctions: line 38: 615 Aborted $APP_RUN $* > log.$APP_NAME 2>&1

the log-file:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-f802ff2d6c5a
Exec : chtMultiRegionFoam
Date : Nov 19 2009
Time : 10:34:59
Host : pag
PID : 615
Case : /nfs/home/fleischer/OpenFOAM/fleischer-1.6/run/Tube1/Test2_4
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region Fluid for time = 0.0001

Create solid mesh for region Stack for time = 0.0001

*** Reading fluid mesh thermophysical properties for region Fluid

Adding to thermoFluid

Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Adding to rhoFluid

Adding to KFluid

Adding to UFluid

Adding to phiFluid

Adding to gFluid

Adding to turbulence

Selecting turbulence model type laminar
Adding to DpDtFluid

*** Reading solid mesh thermophysical properties for region Stack

Adding to rhos

Adding to cps

Adding to Ks

Adding to Ts

Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006
Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006



request for objectRegistry region0 from objectRegistry Test2_4 failed
available objects of type objectRegistry are

2
(
Stack
Fluid
)
#0 Foam::error:rintStack(Foam::Ostream&) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#3 Foam:bjectRegistry const& Foam:bjectRegistry::lookupObject<Foam:bjectReg istry>(Foam::word const&) const in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::OutputFilterFunctionObject<Foam:robes>::st art() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libsampling.so"
#5 Foam::functionObjectList::read() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#6 Foam::Time:perator++() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 main in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116


From function objectRegistry::lookupObject<Type>(const word&) const
in file db/objectRegistry/objectRegistryTemplates.C at line 140.

FOAM aborting


Does anybody know where this problem comes from?
You'll find the packed Case in the attachment
Attached Files
File Type: gz Test2_4.tar.gz (7.4 KB, 23 views)
Victor is offline   Reply With Quote

Old   November 19, 2009, 06:40
Default
  #2
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 7
kawuppdich is on a distinguished road
Hi Victor
I havent looked in your case but I would say there is something wrong with your coupled regions.
Did you customize them? (for example in 0.001/T)
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 07:10
Default
  #3
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 7
kawuppdich is on a distinguished road
no thats not
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 07:22
Default
  #4
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 6
Victor is on a distinguished road
Hi kawuppdich,

i have already looked at the boundary conditions for several times and cannot find any problem. And all log-files don't show any errors. So I don't know why there is a message "request for objectRegistry region0" in the chtMultiRegionFoam!?
I searched for similar problems, but there are only problems like "request for uniformDimensionedVectorField g from objectRegistry region0 failed"!?
Victor is offline   Reply With Quote

Old   November 19, 2009, 07:26
Default
  #5
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 7
kawuppdich is on a distinguished road
the problem is there is no region0. normaly it should be fluid or Stack. I donīt know where it comes from. I had the same error and my problem was that iīve forgot to customize the boundary
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 07:46
Default
  #6
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 7
kawuppdich is on a distinguished road
all looks fine but same error here
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 08:32
Default
  #7
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 6
Victor is on a distinguished road
hmm, i don't find it either....
But thanks a lot for your helpkawuppdich!!
Victor is offline   Reply With Quote

Old   November 23, 2009, 07:26
Default
  #8
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 6
Victor is on a distinguished road
I have an idea where the problem could come from. After setting up a similar case with setSet, setsToZones,splitMeshRegions for the chtMultiregionFoam everything worked fine.
But when i tried to use the probes() function the problem we discussed above ocurred again.
Does anybody know if this could be the reason?
Or does anybody know an alternative for the probes() function without saving the whole data accumulated during the simulation?

here the additional part of the controlDict-File:


functions
{
probesTest
{
// Type of functionObject
type probes;

// Where to load it from (if not already in solver)
functionObjectLibs ("libsampling.so");
outputControl timeStep;
outputInterval 1;

// Locations to be probed. runTime modifiable!
probeLocations
(
( -0.05 0 0)
( -0.04 0 0)
( -0.03 0 0)
( -0.02 0 0)
( -0.01 0 0)
( 0.00 0 0)
( 0.01 0 0)
( 0.02 0 0)
( 0.03 0 0)
( 0.04 0 0)
( 0.05 0 0)
);

// Fields to be probed. runTime modifiable!
fields
(
rho
p
U
T
);
}
};
Victor is offline   Reply With Quote

Old   June 30, 2010, 08:36
Post
  #9
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 11
maddalena is on a distinguished road
Just for information: Victor missed one keyword:
Code:
functions
{ 
  probesTest
    {
    // Type of functionObject
        type probes;

        // Where to load it from (if not already in solver)
        functionObjectLibs ("libsampling.so");
        outputControl   timeStep;                                              
        outputInterval  1;                                                     

        region heater;

        // Locations to be probed. runTime modifiable!
        probeLocations
        (
       ( -0.05 0 0)
       ( -0.04 0 0)    
       ( -0.03 0 0)    
       ( -0.02 0 0)    
       ( -0.01 0 0)    
       ( 0.00 0 0)    
       ( 0.01 0 0)    
       ( 0.02 0 0)    
       ( 0.03 0 0)
       ( 0.04 0 0)
       ( 0.05 0 0)    
    );

        // Fields to be probed. runTime modifiable!
        fields
        (
        rho
        p
        U
        T
    );
     }
};
This entry is not compulsory, as soon as there is only one region in the case. chtMultiRegionFoam, as the name says, is able to manage different regions, thus probes function needs the region name!
Hope this help someone,

mad
Linse and andrejssab like this.
maddalena is offline   Reply With Quote

Old   July 1, 2010, 07:30
Default
  #10
Member
 
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 52
Rep Power: 7
r08n is on a distinguished road
Quote:
Originally Posted by Victor View Post
request for objectRegistry region0 from objectRegistry Test2_4 failed
available objects of type objectRegistry are
2
(
Stack
Fluid
)
Before running the simulation (after `splitMeshRegions`), edit the files 0.001/Stack/polyMesh/boundary: there must be an entry like:

Stack_to_Fluid
{
...
sampleRegion region0;
samplePatch ...
...
}

Change these entries to be

Stack_to_Fluid
{
...
sampleRegion Fluid;
samplePatch Fluid_to_Stack;
...
}

Analogously, in 0.001/Fluid/polyMesh/boundary, there must be this entry:

Fluid_to_Stack
{
...
sampleRegion Stack;
samplePatch Stack_to_Fluid;
...
}

i.e., 'polyMesh/boundary' files of each region contain entries for neighbouring regions
and neighbouring patches.
r08n is offline   Reply With Quote

Old   September 10, 2012, 09:30
Default
  #11
Senior Member
 
Bernhard Linseisen
Join Date: May 2010
Location: Magdeburg/Geneva
Posts: 143
Blog Entries: 1
Rep Power: 6
Linse is on a distinguished road
Quote:
Originally Posted by maddalena View Post
Just for information: Victor missed one keyword:
Code:
functions
{ 
  probesTest
    {
    // Type of functionObject
        type probes;

        // Where to load it from (if not already in solver)
        functionObjectLibs ("libsampling.so");
        outputControl   timeStep;                                              
        outputInterval  1;                                                     

        region heater;

        // Locations to be probed. runTime modifiable!
        probeLocations
        (
       ( -0.05 0 0)
       ( -0.04 0 0)    
       ( -0.03 0 0)    
       ( -0.02 0 0)    
       ( -0.01 0 0)    
       ( 0.00 0 0)    
       ( 0.01 0 0)    
       ( 0.02 0 0)    
       ( 0.03 0 0)
       ( 0.04 0 0)
       ( 0.05 0 0)    
    );

        // Fields to be probed. runTime modifiable!
        fields
        (
        rho
        p
        U
        T
    );
     }
};
This entry is not compulsory, as soon as there is only one region in the case. chtMultiRegionFoam, as the name says, is able to manage different regions, thus probes function needs the region name!
Hope this help someone,

mad
Thanks, Maddalena!

I had the very same problem and it seems to be solved by now!
(Testing the tool, but looking good!)

Cheers,
Bernhard
Linse is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
RSH problem for parallel running in CFX Nicola CFX 5 June 18, 2012 18:31
Problem setting with chtmultiregionFoam Antonin OpenFOAM 10 April 24, 2012 09:50
Problem running paraFoam on OpenFOAM 1.5 sonny OpenFOAM 3 June 6, 2009 20:24
Statically Compiling OpenFOAM Issues herzfeldd OpenFOAM Installation 21 January 6, 2009 09:38
problem in running FoamX in Open FOAM Gaurav Main CFD Forum 3 May 10, 2006 05:06


All times are GMT -4. The time now is 00:16.