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

Problems using reconstructPar on a case involving AMI

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 24, 2012, 02:46
Default Problems using reconstructPar on a case involving AMI
  #1
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
Hello.

I've set up a case using 3 AMIs and MRFSimpleFOAM. It runs fine on one processor, it even runs fine on multiple processors. But I am running into trouble when I try to piece it back together after a parrallel run.

Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 100

Time = 100

Reconstructing FV fields

    Reconstructing volScalarFields

        p
AMI: Creating addressing and weights between 1628 source faces and 1071 target faces
--> FOAM Warning : 
    From function AMIInterpolation<SourcePatch, TargetPatch>::checkPatches(const primitivePatch&, const primitivePatch&)
    in file lnInclude/AMIInterpolation.C at line 146
    Source and target patch bounding boxes are not similar
    source box span     : (8.5e-10 0.55 0.55)
    target box span     : (1.07e-09 0.0576107 0.238538)
    source box          : (0.0423665 -0.275 -0.275) (0.0423665 0.275 0.275)
    target box          : (0.042366 0.217361 -0.136582) (0.042366 0.274972 0.101956)
    inflated target box : (0.0300962 0.205091 -0.148852) (0.0546358 0.287242 0.114226)


--> FOAM FATAL ERROR: 
Unable to set source and target faces

    From function void Foam::cyclicAMIPolyPatch::setNextFaces(label&, label&, const primitivePatch&, const primitivePatch&, const boolList&, labelList&, const DynamicList<label>&) const
    in file lnInclude/AMIInterpolation.C at line 878.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   at cyclicAMIPolyPatch.C:0
#3  Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::update(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#4  Foam::AMIInterpolation<Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> >, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > >::AMIInterpolation(Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::PrimitivePatch<Foam::face, Foam::SubList, Foam::Field<Foam::Vector<double> > const&, Foam::Vector<double> > const&, Foam::autoPtr<Foam::searchableSurface> const&, Foam::faceAreaIntersect::triangulationMode const&, bool) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#5  Foam::cyclicAMIPolyPatch::resetAMI() const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#6  Foam::cyclicAMIPolyPatch::AMI() const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#7  Foam::tmp<Foam::Field<double> > Foam::cyclicAMIPolyPatch::interpolate<double>(Foam::tmp<Foam::Field<double> > const&) const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#8  Foam::cyclicAMIFvPatch::makeWeights(Foam::Field<double>&) const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#9  Foam::surfaceInterpolation::makeWeights() const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#10  Foam::surfaceInterpolation::weights() const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#11  Foam::fvPatch::weights() const in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::coupledFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#13  Foam::cyclicFvPatchField<double>::cyclicFvPatchField(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#14  Foam::fvPatchField<double>::adddictionaryConstructorToTable<Foam::cyclicFvPatchField<double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#15  Foam::fvPatchField<double>::New(Foam::fvPatch const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#16  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricBoundaryField(Foam::fvBoundaryMesh const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::dictionary const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#17  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readField(Foam::dictionary const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#18  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#19  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#20  
 in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#21  
 in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#22  
 in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
#23  __libc_start_main in "/lib64/libc.so.6"
#24  
 in "/software/openfoam-2.1.0/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/reconstructPar"
I used scotch to decompose it, which worked on a previous case, set up analogous to the propeller-tutorial. This mesh however has been generated using ICEM and CFX. My first guess was that OF210 can't handle multiple AMIs, but fusing them using createPatch led to the pretty much the same error. Can anyone point me in the right direction?
Kaskade is offline   Reply With Quote

Old   April 30, 2012, 03:27
Default
  #2
Senior Member
 
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,211
Blog Entries: 1
Rep Power: 17
nimasam is on a distinguished road
maybe you need first use reconstructParMesh for each time step then using reconstructPar
Bernhard likes this.
nimasam is offline   Reply With Quote

Old   April 30, 2012, 04:23
Default
  #3
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
I'll try but I didn't need to use it before.

I used createPatch to make some patches periodic, which created a polyMesh-Directory in timestep 0. Does this maybe cause problems?
Kaskade is offline   Reply With Quote

Old   June 23, 2012, 05:32
Default
  #4
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
Update to OF211 fixed the issue.
Kaskade is offline   Reply With Quote

Old   June 29, 2012, 10:50
Default
  #5
Member
 
supercommandodhruv
Join Date: Sep 2011
Posts: 57
Rep Power: 7
dhruv is on a distinguished road
Quote:
Originally Posted by Kaskade View Post
Update to OF211 fixed the issue.
Hi,

Did you manage to solve the problem? I am having the same issue in my Geometry.

As suggested by Kaskade, I updated my OF version to 2.1.1, but it is still giving me the same message.

Code:
AMI: Creating addressing and weights between 11909 source faces and 12860 target faces
--> FOAM Warning : 
    From function AMIInterpolation<SourcePatch, TargetPatch>::checkPatches(const primitivePatch&, const primitivePatch&)
    in file lnInclude/AMIInterpolation.C at line 146
    Source and target patch bounding boxes are not similar
    source box span     : (9.4 0 2.729063)
    target box span     : (9.4 0 2.729063)
    source box          : (2.35 3 -2.753594) (11.75 3 -0.02453125)
    target box          : (2.3594 60.6 -2.753594) (11.7594 60.6 -0.02453125)
    inflated target box : (1.869993 60.11059 -3.243001) (12.24881 61.08941 0.464876)


--> FOAM FATAL ERROR: 
Unable to find initial target face

    From function void Foam::AMIInterpolation<SourcePatch, TargetPatch>::calcAddressing(const primitivePatch&, const primitivePatch&, label, label)
    in file lnInclude/AMIInterpolation.C at line 1009.
In the boundary mesh, the number of faces for the patches which are in cyclic AMI are different. It is strange because, it works for one another case I have, which also has a difference between the number of faces.

Could anyone help me in this regard. I have to have cyclic boundary condition on these patches.

Thanks,
Dhruv.
dhruv is offline   Reply With Quote

Old   June 29, 2012, 12:51
Default
  #6
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
The difference in the number of faces should not be a problem, since part of an AMIs job is to mediate between meshes with different levels refinement.

Are you sure everything else is set up correctly? CofG, Rotational Axis? Are the meshes really correctly positioned or is there a gap or an overlap?

What did you use to create the mesh?
Kaskade is offline   Reply With Quote

Old   July 2, 2012, 06:32
Default
  #7
Member
 
supercommandodhruv
Join Date: Sep 2011
Posts: 57
Rep Power: 7
dhruv is on a distinguished road
Quote:
Originally Posted by Kaskade View Post
The difference in the number of faces should not be a problem, since part of an AMIs job is to mediate between meshes with different levels refinement.

Are you sure everything else is set up correctly? CofG, Rotational Axis? Are the meshes really correctly positioned or is there a gap or an overlap?

What did you use to create the mesh?

Yes, the number of faces should not be a problem, since this is what AMI is used for. For your questions:

1. Where can I find the information regarding the CofG, Rotational Axis, etc.?
2. The two faces in the mesh are at a distance of 9.4 units from each other in the x direction. So, the patches which have cyclic AMI in the boundary file looks like this

Code:
Out
{
        type            cyclicAMI;
        nFaces          12860;
        startFace       5101486;
        faces           ( ( 1 2 6 5 ) );
        matchTolerance  0.0001;
        neighbourPatch  In;
        transform       translational;
        separationVector (-9.4 0 0);
    }

In
    {
        type            cyclicAMI;
        nFaces          11909;
        startFace       5055469;
        faces           ( ( 0 3 7 4 ) );
        matchTolerance  0.0001;
        neighbourPatch  Out;
        transform       translational;
        separationVector (9.4 0 0);
    }
3. I am using snappyHexMesh to create the mesh. I also changed the matchTolerance to vary between 1e-05 to 1 to see, if it has to do anything with the tolerance levels, but everytime the same error pops up. Any suggestions?

Regards,
Dhruv.
dhruv is offline   Reply With Quote

Old   July 2, 2012, 08:53
Default
  #8
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
1. In the dynamicMeshDict. I thought maybe something was rotating the wrong way.

2. Why do you have 'faces', 'transform' and 'separationVector' in yours. The last two are for cyclic not cyclicAMI. Mine look like this.
Code:
    
   AMI2
    {
        type            cyclicAMI;
        nFaces          7268;
        startFace       2103511;
        matchTolerance  0.0001;
        neighbourPatch  AMI1;
        transform       noOrdering;
    }
    AMI1
    {
        type            cyclicAMI;
        nFaces          34254;
        startFace       2110779;
        matchTolerance  0.0001;
        neighbourPatch  AMI2;
        transform       noOrdering;
    }

3. In some other thread they solved some problem with their AMI by increasing the refinement of their mesh near the AMI, I think. Maybe SHM is generating a mesh that is not curved enough.
Kaskade is offline   Reply With Quote

Old   July 2, 2012, 09:27
Default
  #9
Member
 
supercommandodhruv
Join Date: Sep 2011
Posts: 57
Rep Power: 7
dhruv is on a distinguished road
Quote:
Originally Posted by Kaskade View Post
1. In the dynamicMeshDict. I thought maybe something was rotating the wrong way.

2. Why do you have 'faces', 'transform' and 'separationVector' in yours. The last two are for cyclic not cyclicAMI. Mine look like this.
Code:
    
   AMI2
    {
        type            cyclicAMI;
        nFaces          7268;
        startFace       2103511;
        matchTolerance  0.0001;
        neighbourPatch  AMI1;
        transform       noOrdering;
    }
    AMI1
    {
        type            cyclicAMI;
        nFaces          34254;
        startFace       2110779;
        matchTolerance  0.0001;
        neighbourPatch  AMI2;
        transform       noOrdering;
    }
3. In some other thread they solved some problem with their AMI by increasing the refinement of their mesh near the AMI, I think. Maybe SHM is generating a mesh that is not curved enough.
Thanks for the reply.

1. The case is stationary. So, I dont have a dynamicMeshDict.
2. I tried removing the faces, and making the boundary file like you have posted above, but still I get the same error.
3. I will now try to refine the mesh better to see if it works

Thanks,

Dhruv.

Last edited by dhruv; July 2, 2012 at 09:28. Reason: full explanation
dhruv is offline   Reply With Quote

Old   July 2, 2012, 13:09
Default
  #10
Member
 
Onno
Join Date: Jan 2012
Location: Germany
Posts: 93
Rep Power: 7
Kaskade is on a distinguished road
This board can be pretty annoying, since many questions remain unanswered, so I try to be of help.

Could you maybe send a picture of your mesh? What is the shape of the AMI? Just a flat face or a cylinder like in the propeller case?
Kaskade is offline   Reply With Quote

Old   July 3, 2012, 04:49
Default AMI patches
  #11
Member
 
supercommandodhruv
Join Date: Sep 2011
Posts: 57
Rep Power: 7
dhruv is on a distinguished road
Quote:
Originally Posted by Kaskade View Post
This board can be pretty annoying, since many questions remain unanswered, so I try to be of help.

Could you maybe send a picture of your mesh? What is the shape of the AMI? Just a flat face or a cylinder like in the propeller case?
Hi Kaskade,

Can you send me your mail ID. I cannot post the picture on the forum.

Thanks,
Dhruv.
dhruv is offline   Reply With Quote

Old   January 27, 2013, 16:56
Default
  #12
Member
 
Sherif Kadry
Join Date: May 2009
Posts: 38
Rep Power: 9
sherifkadry is on a distinguished road
You ever get this problem fixed? I have the same issue

Quote:
Originally Posted by dhruv View Post
Hi Kaskade,

Can you send me your mail ID. I cannot post the picture on the forum.

Thanks,
Dhruv.
sherifkadry is offline   Reply With Quote

Old   March 22, 2014, 08:35
Default cyclicAMI is broken in build 2.3.x-9d0ee4591849
  #13
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 77
Rep Power: 6
zordiack is on a distinguished road
I'm having this exactly same problem and I tried to file a bug report but it wouldn't let me (says Forbidden). I'm running the latest git version 2.3.x so this is definitely not fixed.

I tried to run reconstructPar after successful calculation but it crashes. It has worked just fine before.

I have the same case on another computer with build 2.3.x-4ef1b5eeb58d and if the case is run with this version the reconstructPar is working fine. I tried using the older reconstructPar with the case run with newer version but it gives the same error message, therefore the cyclicAMI is somehow broken in the current git version.

The strange thing is that the calculation runs just fine with the new version and based on the cuttingplanes the results also look fine. Only reconstructing the case is not working.

This is a major bug and I wish it's resolved quickly. Could this have something to do with the commit https://github.com/OpenFOAM/OpenFOAM...d2ccf500140c8?



Code:
Reconstructing volVectorFields

        U
AMI: Creating addressing and weights between 6 source faces and 6654 target faces
--> FOAM Warning : 
    From function AMIMethod<SourcePatch, TargetPatch>::checkPatches()
    in file lnInclude/AMIMethod.C at line 57
    Source and target patch bounding boxes are not similar
    source box span     : (0.0022143419 0.00319520457 0.001766738)
    target box span     : (0.3591645372 0.04399999883 0.1611334531)
    source box          : (-0.1433046982 0.03092641575 -0.1791014874) (-0.1410903563 0.03412162032 -0.1773347494)
    target box          : (-0.2179735666 -0.00800000038 0.06686654698) (0.1411909706 0.03599999845 0.2280000001)
    inflated target box : (-0.2377788156 -0.02780524933 0.04706129803) (0.1609962196 0.0558052474 0.2478052491)


--> FOAM FATAL ERROR: 
Unable to find initial target face

    From function void Foam::AMIMethod<SourcePatch, TargetPatch>::initialise(labelListList&, scalarListList&, labelListList&, scalarListList&, label&, label&)
    in file lnInclude/AMIMethod.C at line 149.

Last edited by wyldckat; March 22, 2014 at 11:35. Reason: posts made 1h apart in different forums and merged here to keep a "tight" discussion
zordiack is offline   Reply With Quote

Old   March 22, 2014, 09:55
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Greetings Pekka,

Quote:
Originally Posted by zordiack View Post
I would have reported this through mantis but for some reason it keeps saying forbidden.
Try logging out - http://www.openfoam.org/mantisbt/logout_page.php - and then logging back in.

In the mean time, you can try undoing only that specific commit:
Code:
foam
git revert 8b9a35d3e261e086c5fa20b55bdd2ccf500140c8
./Allwmake
Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   March 22, 2014, 11:07
Default
  #15
Senior Member
 
dkxls's Avatar
 
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 156
Rep Power: 11
dkxls will become famous soon enough
Quote:
Originally Posted by zordiack View Post
I'm having this exactly same problem and I tried to file a bug report but it wouldn't let me (says Forbidden). I'm running the latest git version 2.3.x so this is definitely not fixed.
I cannot comment on your actual bug, but about reporting it.
This "Forbidden" error happens sometimes. For me it occurred mostly when I copy&past larger text/errors logs. Though, I couldn't pinpoint what exactly goes wrong, but happened only 2-3 times.
dkxls is offline   Reply With Quote

Old   March 22, 2014, 13:04
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
For future reference, Pekka has reported this issue here: http://www.openfoam.org/mantisbt/view.php?id=1234
wyldckat is offline   Reply With Quote

Old   March 22, 2014, 16:52
Default
  #17
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
@zordiack: I've finished building the latest OpenFOAM 2.3.x, commit 9d0ee45918 and tried to run the following tutorials:
  • "incompressible/pimpleDyMFoam/mixerVesselAMI2D" - ran Allrun
  • "incompressible/pimpleDyMFoam/oscillatingInletACMI2D" - ran Allrun-parallel
  • "incompressible/pimpleDyMFoam/propeller"- ran Allrun and left it running for a while, stopped and reconstructed it.
And in all of them, everything ran just fine.
It's possible that I'm not using a particular feature that you're using, but since I'm not very familiar with AMI in OpenFOAM, it would be helpful to know which tutorial to test with, to see if the problem is reproducible.
wyldckat is offline   Reply With Quote

Old   March 24, 2014, 03:38
Default
  #18
Member
 
Pekka Pasanen
Join Date: Feb 2012
Location: Finland
Posts: 77
Rep Power: 6
zordiack is on a distinguished road
The problem was not with AMI, it was groovyBC and swak4Foam. I'm using the development version of swak4Foam and once I commented out the libs in controlDict reconstructPar started working again.

So if you're encountering some weird errors regarding decompose/reconstruct, check your libs for any "nonstandard" libs. It still puzzles me how could it run fine and then not recontruct with the libs.
sahas, wyldckat, callmetao and 1 others like this.
zordiack is offline   Reply With Quote

Old   March 21, 2016, 02:31
Default
  #19
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 197
Rep Power: 10
JBeilke is on a distinguished road
The problem was fixed in 3.0.0 but reintroduced in 3.0.x
JBeilke is offline   Reply With Quote

Old   March 26, 2016, 06:01
Default
  #20
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,748
Blog Entries: 39
Rep Power: 103
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quote:
Originally Posted by JBeilke View Post
The problem was fixed in 3.0.0 but reintroduced in 3.0.x
Quick question @JBeilke: Can you please provide more details, namely which tutorial case I can use to test this, so that I can reproduce the problem?
wyldckat 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
Sample utility problems msrinath80 OpenFOAM Running, Solving & CFD 12 December 21, 2012 06:51
Problem with reconstructPar fabianpk OpenFOAM 5 August 14, 2007 09:17
Problems involving interFoam and GCC 410 gschaider OpenFOAM Installation 1 July 30, 2006 19:58
Problems reading a case cavity into paraFoam red hat 9 anton322322 OpenFOAM Pre-Processing 0 April 11, 2005 13:13
High speed flow problems Sawa FLUENT 3 January 14, 2003 02:10


All times are GMT -4. The time now is 13:03.