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

error running potentialFoam

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

Like Tree7Likes
  • 1 Post By wyldckat
  • 1 Post By blackbirdinapie
  • 4 Post By cm_jubayer
  • 1 Post By CFDelix

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 25, 2011, 15:32
Default error running potentialFoam
  #1
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 16
cm_jubayer is on a distinguished road
Hi,

I am getting the following error while running potentialFoam. Can someone please tell me the probable reason for that.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam171/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#3 Foam::Istream& Foam:perator>><Foam::Vector<double> >(Foam::Istream&, Foam::List<Foam::Vector<double> >&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#4 Foam::Field<Foam::Vector<double> >::Field(Foam::word const&, Foam::dictionary const&, int) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#5 Foam::fvPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam::fixedValu eFvPatchField<Foam::Vector<double> > >::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam171/lib/linux64GccDPOpt/libfiniteVolume.so"
#6 Foam::fvPatchField<Foam::Vector<double> >::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#7 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricB oundaryField(Foam::fvBoundaryMesh const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#8 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::dictionary const&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#9 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#10 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#11
in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
#12 __libc_start_main in "/lib64/libc.so.6"
#13
in "/opt/openfoam171/applications/bin/linux64GccDPOpt/potentialFoam"
Aborted
cm_jubayer is offline   Reply With Quote

Old   August 25, 2011, 15:37
Default
  #2
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 16
cm_jubayer is on a distinguished road
The first portion of the error...

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.x |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.x-3776603e4c6c
Exec : potentialFoam
Date : Aug 25 2011
Time : 15:13:51
Host : pkgst1
PID : 7636
Case : /home/sysadmin/OpenFOAM/sysadmin-1.7.1/run/tutorials/basic/potentialFoam/Solarpanels
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

Reading field p

Reading field U



--> FOAM FATAL ERROR:
Attempt to cast type N4Foam5token8CompoundINS_4ListIdEEEE to type N4Foam5token8CompoundINS_4ListINS_6VectorIdEEEEEE

From function dynamicCast<To>(From&)
in file /home/opencfd/OpenFOAM/OpenFOAM-1.7.x/src/OpenFOAM/lnInclude/typeInfo.H at line 93.
cm_jubayer is offline   Reply With Quote

Old   August 25, 2011, 15:47
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings Jubayer,

There is some strange crazy stuff going on there, which is why it's crashing!

#2 and #3 from the 1st post indicate that it crashed when it was trying to output an error message (#2), which occurred when reading from some file (#3).
From the 2nd post, there is an error that the compiler would never have allowed to happen!
To top that, it looks like you have two versions of OpenFOAM overlapping each other! Namely 1.7.1 and 1.7.x! This should never happen... unless one knows what one is doing!

Additionally, running a tutorial that is not from the official list of tutorials will increase the probability of error! "Solarpanels" is not a tutorial from the list of tutorials distributed with OpenFOAM!

Best regards,
Bruno
aow likes this.
__________________
wyldckat is offline   Reply With Quote

Old   August 26, 2011, 10:23
Default
  #4
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 16
cm_jubayer is on a distinguished road
Hello Bruno,

Thanks for your prompt reply. That really helps.

Regards,
Jubayer
cm_jubayer is offline   Reply With Quote

Old   January 26, 2012, 14:42
Default
  #5
New Member
 
Join Date: Oct 2011
Posts: 10
Rep Power: 14
blackbirdinapie is on a distinguished road
Hi, I am facing a similar problem. Did anyone solve this strange error?

--> FOAM FATAL ERROR:
Attempt to cast type N4Foam5token8CompoundINS_4ListIdEEEE to type N4Foam5token8CompoundINS_4ListINS_6VectorIdEEEEEE
eternityboy likes this.
blackbirdinapie is offline   Reply With Quote

Old   January 26, 2012, 15:42
Default
  #6
Member
 
Jubayer
Join Date: Oct 2009
Location: The University of Western Ontario, London, Ontario
Posts: 42
Blog Entries: 1
Rep Power: 16
cm_jubayer is on a distinguished road
Hi blackbirdinapie,

potentialFoam only works if the velocity and pressure are fixedValues, not a profile. For my case, I had a velocity profile at the inlet which caused the error. Hope this helps.

Jubayer
wyldckat, aow, saladbowl and 1 others like this.
cm_jubayer is offline   Reply With Quote

Old   March 28, 2018, 05:16
Default problems with funkyDoCalc for groovyBC type inlet
  #7
New Member
 
Felix S
Join Date: Jun 2017
Posts: 11
Rep Power: 8
CFDelix is on a distinguished road
Hi all,

I recieve the same Error
Code:
Attempt to cast type N4Foam5token8CompoundINS_4ListIdEEEE to type N4Foam5token8CompoundINS_4ListINS_6VectorIdEEEEEE
when trying to use funkyDoCalc on a simulation with an inlet defined by groovyBC type boundary.

I defined one 0/U file with different variables to change the inlet boundary condition. Otherwise I use the same simulation every time.
The problem is that funkyDoCalc works for most of the results while a few of them are causing this error.
For me there is no resonable pattern when the error occurs.
Bana likes this.
CFDelix is offline   Reply With Quote

Old   March 28, 2018, 10:04
Default I found the source to the error
  #8
New Member
 
Felix S
Join Date: Jun 2017
Posts: 11
Rep Power: 8
CFDelix is on a distinguished road
Hi,

in my case something strange happens for some of the inlet bcs.

Apparently the groovyBC inlet information is taken over into the result-files. Converting them into ascii shows that the groovyBC inlet suddenly has
Code:
boundaryField
{
    inpipe
    {        
        refValue        uniform (0 3.347407 6.694814);
        refGradient     uniform (0 0 0);
        valueFraction   uniform 1;
        value           uniform (0 3.347407 6.694814);
...
all these values that are usually used with mixed bcs. I don't understand why that happens because a gradient is not needed when the fraction is 1, right?

The problem with some of my calculations though is that the refValue and refGradient become lists of scalar values except of vectors.
This causes funkyDoCalc to crash with the mentioned error.

I solved the problem for my purporses by putting something uniform like in the example above since my evaluated patch has nothing to do with the inlet conditions.
edit: it is also possible to change the inlet type from groovyBC to fixedValue. That is an easy search and replace approach and the solution-field stays correct.

I am still interested of how the error occured in the first place.
I also had troubles with reconstructPar for the exact calculations, which was made possible by deleting the groovybc.so from the libs in the controlDict (that is a known problem: https://bugs.openfoam.org/view.php?id=1234).
CFDelix is offline   Reply With Quote

Reply

Tags
error, potentialfoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Using potentialFoam with simpleBuoyantFoam lasb OpenFOAM Running, Solving & CFD 5 August 28, 2015 12:32
Boundary conditions for potentialFoam doubtsincfd OpenFOAM 7 May 17, 2011 04:11
potentialFoam around a sphere ; mesh by Gmsh eliam OpenFOAM Running, Solving & CFD 12 January 26, 2011 03:02
potentialFOAM with non-zero pressure @outlet muellea OpenFOAM 2 September 12, 2010 23:34
PotentialFoam fails bastil OpenFOAM Running, Solving & CFD 0 April 17, 2009 09:43


All times are GMT -4. The time now is 07:47.