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

DynamicRefineFvMesh dies on snappyHexMesh generated grid

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 29, 2009, 13:10
Default I am building a very much simp
  #1
New Member
 
Christian Trapp
Join Date: Mar 2009
Posts: 7
Rep Power: 8
chtrapp is on a distinguished road
I am building a very much simplified simulation of smoke coming out of a chimney. The case runs fine with interDyMFoam when using a staticFvMesh. Whenever I try to run it with a dynamicRefineFvMesh, the case aborts with the following message:


Starting time loop

Courant Number mean: 0.0877711 max: 0.504
deltaT = 0.25
Time = 0.75

Selected 0 cells for refinement out of 20000.


Only call if constructed with history capability#0 Foam::error::printStack(Foam:: Ostream&) in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::hexRef8::getSplitPoints() const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so"
#3 Foam::dynamicRefineFvMesh::selectUnrefinePoints(do uble, Foam::PackedList<1> const&, Foam::Field<double> const&) const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicFvMesh.so"
#4 Foam::dynamicRefineFvMesh::update() in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicFvMesh.so"
#5 main in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interDyMFoam"
#6 __libc_start_main in "/lib/tls/libc.so.6"
#7 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interDyMFoam"


From function hexRef8::getSplitPoints()
in file polyTopoChange/polyTopoChange/hexRef8.C at line 4666.

FOAM aborting

What am I doing wrong?

Greetings, christian
simplifiedRefining.tar.gz
chtrapp is offline   Reply With Quote

Old   February 1, 2009, 17:38
Default Hi Christian, I don't have
  #2
Member
 
Ola Widlund
Join Date: Mar 2009
Location: Sweden
Posts: 87
Rep Power: 8
olwi is on a distinguished road
Hi Christian,

I don't have the answer to your problem, but I join you in hoping you find some feedback from the forum...

Since both dynamicRefineFvMesh and snappyHexMesh seem to use the same refinement/coarsening tools (i.a. the polyTopoChnager hexRef8), one would think that they are compatible.

I am hoping to use the same approach in a later stage of a current project.

Does anyone else have experience of succesfully combining snappyHexMesh meshes with the dynamicRefineFvMesh class? Any fundamental reasons to believe it wouldn't work?

/Ola
olwi is offline   Reply With Quote

Old   February 3, 2009, 05:48
Default It might work as long as you d
  #3
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
It might work as long as you don't have any layers - they mess up the refinement information (pointLevel, cellLevel). The dynamicRefineFvMesh tries to work out from those two files what cells can be refined.
mattijs is offline   Reply With Quote

Old   February 3, 2009, 10:06
Default I just checked if maybe I had
  #4
New Member
 
Christian Trapp
Join Date: Mar 2009
Posts: 7
Rep Power: 8
chtrapp is on a distinguished road
I just checked if maybe I had forgotten to switch the layer addition off (which would be just me). Dissapointingly I found that it is switched off.

To be sure, I checked the number of cells before and after running snappyHexMesh (and found it to be constant). So I'm a bit sorry here, since it would have been nice if the solution had been to simply remove the layers.

Greetings, christian.
chtrapp is offline   Reply With Quote

Old   March 26, 2009, 06:54
Default
  #5
Senior Member
 
Mark Couwenberg
Join Date: Mar 2009
Location: Netherlands
Posts: 130
Rep Power: 8
markc is on a distinguished road
Hello All,

I get a similar error message on a mesh created with blockMesh and snappyHexMesh. I use turbDyMFoam and want to refine based on the volScalarField epsilon.
It seems like a refinement actually occurs, the log file gives
>>>
Selected 5 cells for refinement out of 59607.
Refined from 59607 to 59642 cells.
<<<
But then the solver crashes, giving the same stacktrace is presented above, with the error message:
>>>
Only call if constructed with history capability
<<<
I played around with settings in the refineMeshDict, without success.

Any comments?


Brgds,

Mark
markc is offline   Reply With Quote

Old   March 26, 2009, 08:05
Default how use refineMeshDict
  #6
gmc
New Member
 
sonia esteban
Join Date: Mar 2009
Posts: 2
Rep Power: 0
gmc is on a distinguished road
Hi all
We read your last comment about how use refineMeshDict

We are working with interDyMFoam recently,using only refineMeshDict and get refined/coarsed our mesh based on the volScalarField Temperature (modified maxRefinement and maxCells ).
But we like more information about the meaning of this parameters:
unrefineLevel 10;
nBufferLayers 1;

Could someone help us find information about the significance of these parameters?
Thanks. Ana and Sonia
gmc is offline   Reply With Quote

Old   January 13, 2011, 00:56
Default
  #7
Member
 
Join Date: Mar 2009
Location: Sydney, New South Wales, Australia
Posts: 42
Rep Power: 8
rassilon is on a distinguished road
Quote:
Originally Posted by chtrapp View Post
I am building a very much simplified simulation of smoke coming out of a chimney. The case runs fine with interDyMFoam when using a staticFvMesh. Whenever I try to run it with a dynamicRefineFvMesh, the case aborts with the following message:


Starting time loop

Courant Number mean: 0.0877711 max: 0.504
deltaT = 0.25
Time = 0.75

Selected 0 cells for refinement out of 20000.


Only call if constructed with history capability#0 Foam::error:rintStack(Foam:: Ostream&) in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::hexRef8::getSplitPoints() const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so"
#3 Foam::dynamicRefineFvMesh::selectUnrefinePoints(do uble, Foam::PackedList<1> const&, Foam::Field<double> const&) const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicFvMesh.so"
#4 Foam::dynamicRefineFvMesh::update() in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicFvMesh.so"
#5 main in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interDyMFoam"
#6 __libc_start_main in "/lib/tls/libc.so.6"
#7 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/fgtools/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interDyMFoam"


From function hexRef8::getSplitPoints()
in file polyTopoChange/polyTopoChange/hexRef8.C at line 4666.

FOAM aborting

What am I doing wrong?

Greetings, christian
simplifiedRefining.tar.gz

Hi! Did you ever solve this problem? I am hoe encountering the exact same error, and would love to know how/if you overcame it

I am trying to use snappyHexMesh and interDyMFoam together with no success.

Cheers,


R
rassilon is offline   Reply With Quote

Old   April 13, 2011, 05:36
Default
  #8
New Member
 
Mark Beal
Join Date: Feb 2011
Posts: 24
Rep Power: 6
msbealo is on a distinguished road
Any news on this? I'm having similar problems.

Mark
msbealo is offline   Reply With Quote

Old   April 13, 2011, 07:11
Default
  #9
New Member
 
Mark Beal
Join Date: Feb 2011
Posts: 24
Rep Power: 6
msbealo is on a distinguished road
I made a little headway on this and thought I'd share my solution. This is mostly guesswork and following similar threads on here. I was hoping to see how a refinement layer around the water/air interface of a boat in a flow developed using dynamicRefineFvMesh, which I mostly copied from the damBreakWithObstacle case. I set up my case using a simple 20x20x20 (ish) box, used snappyHexMesh to import my hull shape. The case worked well with interFoam before I made the changes. I had similar problems to those described above, so here is my solution.

1) I delete the refinementHistory file from polyMesh folder. This fixed the "Only call if constructed with history capability" problem.

2) Changing the fvSolutions file so that cacheAgglomeration = false for all solvers. I tested this further and just turning the p_rghFinal PCG/GAMG solver to false fixed the problem for the first few iterations. This solved the "field does not correspond to level 0 sizes: field = 19860 level = 10683" problem

3) Also, I turned off the surface layers in the snappyHexMeshDict. This was suggested on here, but I didn't test it's effectiveness.

I'm still not able to run in parallel as I get the following error,

"Number of cells in mesh:2666 does not equal size of cellLevel:10683
This might be because of a restart with inconsistent cellLevel."

but for the purposes of investigating the interface refinement region this might not be necessary.
I hope this helps someone.

Mark
msbealo is offline   Reply With Quote

Old   October 1, 2012, 08:00
Default
  #10
New Member
 
Johan
Join Date: May 2012
Posts: 4
Rep Power: 5
JohanAdam is on a distinguished road
Hi everyone

I am also having the same problem with snappy and dymanicRefineFvMesh. Did anyone perhaps test other mesh generators? If it is only snappy, would a dirty work around by importing and exporting the mesh maybe be possibility?

Johan
JohanAdam is offline   Reply With Quote

Old   October 4, 2012, 06:30
Default
  #11
New Member
 
Johan
Join Date: May 2012
Posts: 4
Rep Power: 5
JohanAdam is on a distinguished road
Hi everyone

To get adaptive mesh refinement working with snappyHexMesh, I found I had to delete the following files from constant/polyMesh after creating the mesh

$ rm constant/polyMesh/cellLevel
$ rm constant/polyMesh/pointLevel
$ rm constant/polyMesh/refinementHistory
$ rm constant/polyMesh/surfaceIndex
$ rm constant/polyMesh/temp*

Cheers
Johan
JohanAdam 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
DynamicRefineFvMesh dies on snappyHexMesh generated grid chtrapp OpenFOAM Running, Solving & CFD 0 January 29, 2009 13:07
How to import grid generated using ICEM/CFD Harry CD-adapco 2 April 17, 2006 00:01
Use of grid generated by GAMBIT ramp Main CFD Forum 5 July 8, 2005 13:24
StarWatch Daemon always dies! Jiaying Xu CD-adapco 14 December 9, 2002 22:52
Dead cells created on edges when a grid file is generated in GAMBIT and imported into FLUENT4 Isaac Manohar Ch. FLUENT 1 June 2, 2000 04:58


All times are GMT -4. The time now is 12:39.