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

Problem with running chtMultiRegionFoam after using setSet utility

Register Blogs Community New Posts Updated Threads Search

Like Tree9Likes
  • 9 Post By maddalena

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 19, 2009, 06:24
Default Problem with running chtMultiRegionFoam after using setSet utility
  #1
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17
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, 44 views)
Victor is offline   Reply With Quote

Old   November 19, 2009, 07:40
Default
  #2
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17
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, 08:10
Default
  #3
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17
kawuppdich is on a distinguished road
no thats not
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 08:22
Default
  #4
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17
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, 08:26
Default
  #5
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17
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, 08:46
Default
  #6
New Member
 
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17
kawuppdich is on a distinguished road
all looks fine but same error here
kawuppdich is offline   Reply With Quote

Old   November 19, 2009, 09:32
Default
  #7
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17
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, 08:26
Default
  #8
New Member
 
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17
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, 09:36
Post
  #9
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23
maddalena will become famous soon enough
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
maddalena is offline   Reply With Quote

Old   July 1, 2010, 08:30
Default
  #10
Member
 
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17
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, 10:30
Default
  #11
Senior Member
 
Bernhard Linseisen
Join Date: May 2010
Location: Heilbronn
Posts: 183
Blog Entries: 1
Rep Power: 16
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

Old   March 22, 2023, 20:41
Default
  #12
Senior Member
 
Desh
Join Date: Mar 2021
Location: Sydney
Posts: 118
Rep Power: 5
dasith0001 is on a distinguished road
Hi,

I am running into the same problem but trying to calculate 'wallHeatFlux' from the 'topSolid' region in the patch called ' maxZ'.

OpenFOAM version is 10.

my 'wallHeatFlux' function looks like

Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  10
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "system";
    object      sample;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

type            surfaces; //sets; //surfaces
functionObjectLibs           ("libsampling.so");

region           topSolid; 

//libs            ("fieldFunctionObjects");
//region           topSolid;

writeControl         writeTime;
interpolationScheme  cellPointFace;
setFormat            raw; //vtk

fields          ( wallHeatFlux ); //U p

surfaces
(
    surfaces1
    {
        type         plane;
        patchName    maxZ;
    }

);
and I am getting the error of

PHP Code:
[0] --> FOAM FATAL ERROR:
[
0]
    
request for objectRegistry region0 from objectRegistry V07processor0 failed
    available objects of type objectRegistry are

10
(
midAir
seal
bottomSolid
thermalB
topSolid
heater
wallSolid
heaterZ2
stand
wallSolid2

Would you guys be able to direct me in the right way, relatively new, specially to OF10. help is hugely appreciated.

Thanks,
Dasith
dasith0001 is offline   Reply With Quote

Old   March 24, 2023, 01:01
Default
  #13
Senior Member
 
Desh
Join Date: Mar 2021
Location: Sydney
Posts: 118
Rep Power: 5
dasith0001 is on a distinguished road
found the answer at

HTML Code:
https://www.cfd-online.com/Forums/openfoam-solving/248597-wallheatflux-openfoam-version-10-a.html
dasith0001 is offline   Reply With Quote

Reply


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
RSH problem for parallel running in CFX Nicola CFX 5 June 18, 2012 19:31
Problem setting with chtmultiregionFoam Antonin OpenFOAM 10 April 24, 2012 10:50
Problem running paraFoam on OpenFOAM 1.5 sonny OpenFOAM 3 June 6, 2009 21:24
Statically Compiling OpenFOAM Issues herzfeldd OpenFOAM Installation 21 January 6, 2009 10:38
problem in running FoamX in Open FOAM Gaurav Main CFD Forum 3 May 10, 2006 06:06


All times are GMT -4. The time now is 15:48.