[lsamuel]

Hi all,
I am new to CFD and have been working on a project to compare OpenFoam to Fluent. I have imported a gambit file to openFoam and done a checkMesh. However, while the checkMesh says that the mesh is OK. I need to change my calculation time as for any time I have the programs says there is no mesh. Please provide me with some hints as to what I may be doing incorrectly.
I really need to view this mesh. I also need to learn how to put in boundary conditions for viscosity, mass flow and density. I've tried what is suggested but the fields specification menu won't appear. I know these may be simple questions. Thanks alot for any assistance you can give

L

[ariorus]

Hello,

did you try fluent3DMeshToFoam?
It should work fine on your problem, you don't have to use splitMesh utilities either.

[dmoroian]

Well, it doesn't work better, it just changes the complain from checkMesh:

checkMesh ./ testInternal
...
Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
wall 902 491 ok (not multiply connected)
internal_walls 496 144 multiply connected surface (shared edge)
outlet 228 135 ok (not multiply connected)
inlet 226 134 ok (not multiply connected)
<<Writing 144 conflicting points to set nonManifoldPoints
...

Still, I'm confused! If I try to run the case, it still works without complaints. I thought that all boundary conditions should be put on faces connected to only one cell, but in my case it works for internal faces (with cells on both sides).
How is that possible? How is the wall function applied in this case?

Dragos

[dinonettis]

Hi everyboy!
I've just created a mesh in gambit for a 2D naca profile and I used fluentmeshtofoam to import it in FoamX. This is the message that I obtain when I run the checkmesh Utility. Everything seems to be ok, but the check fails. Could it be a considerable problem in solving my case, or can I neglect this message since most of it is OK??

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 142742
edges: 491969
faces: 488155
internal faces: 210005
cells: 138928
boundary patches: 3
point zones: 0
face zones: 0
cell zones: 0

Number of cells of each type:
hexahedra: 3520
prisms: 135408
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
freestream 72 144 ok (not multiply connected)
wing 222 444 ok (not multiply connected)
frontAndBackPlanes 277856 142742 ok (not multiply connected)

Checking geometry...
Domain bounding box: (-22.5 -22.5 -0.636396) (22.5 22.5 0.636396)
Boundary openness (-2.19138e-19 -1.1285e-18 0) OK.
***High aspect ratio cells found, Max aspect ratio: 2621.3, number of cells 452
<<Writing 452 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 1.07929e-06. Maximum face area = 3.69135. Face area magnitudes OK.
Min volume = 1.37371e-06. Max volume = 3.89378. Total volume = 2577.17. Cell volumes OK.
Mesh non-orthogonality Max: 36.1795 average: 4.1525
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.783093 OK.
Min/max edge length = 0.000999746 2.9002 OK.
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All face flatness OK.

Failed 1 mesh checks.

End


PS: I didn't understand why I found in this forum that it is necessary to import the mesh in ascii format from gambit. This option is not available in the export menu of gambit. I noticed that it is available in the fluent export menu, but when I try to import the mesh in fluent from gambit, and then to export it in ascii the checkmesh result is really a mess!!!!
Please help me
Thank you in advance

dino

[dmoroian]

I think it's safe enough for you to just ignore the "High aspect ratio cells found" message and start the computation.

Dragos

[danielle]

Hi Bernhard,
my geometry is 2d with 3 zones and with internal walls. when I use splitMeshWithSets (http://openfoamwiki.net/index.php/Contrib_SplitMe shWithSets) after the conversion of my mesh (fluent mesh) with only -writeSets, It work good but if I use -writeZones and -writeSets I have this error:
FOAM FATAL ERROR : Already 3 faceZones existing
From function splitMeshWithSets
in file splitMeshWithSets.C at line 269.

I need the Zones with the internal walls.
how can I do this ?
thank you for help

[gschaider]

Hi Danielle!

Right now the splitMeshWithSets-util can't deal with existing zones. Try to convert the mesh with -writeSets, use the util, then use the setsToZones-util to convert the cellSets to cellZones

Bernhard

[podallaire]

Hi Bernhard,

I have a very similar problem. I created a geometry with gmsh and
with the help of Takuya (http://www.cfd-online.com/OpenFOAM_D...tml?1213278563), I was able to convert a faceZone to an internal wall (shell) using createBaffles.

However, I'm experiencing big divergence problems and I suspect that the wallFunctions might be wrong with my shell. Instead of using createBaffles, I tried to use the procedure (http://openfoamwiki.net/index.php/Howto_importing_fluent_mesh_with_internal_wall s) with SplitMeshWithSets in order to have 2 boundaries for the shell. It almost worked :

...
Determining visibility from point 90
Determining visibility from point 247
Determining visibility from point 250
Allready zones existing in the mesh

--> FOAM FATAL ERROR : Already 1 faceZones existing

From function splitMeshWithSets
in file splitMeshWithSets.C at line 269.

FOAM exiting


What to do next ? I tried to use cellSet and setsToZones but setsToZones is not successfull ...

Any suggestion ?

Regards,

Pierre-Olivier

[gschaider]

Hi Pierre-Oliver!

@the wall fuinhction: have you checked that the created patches have "type wall;" in the constant/polyMesh/boundary-file? Only then will the turbulence-model calculate wallFunctions there

@failing of splitMesh: check whether ther is a file constant/polyMesh/faceZones. Remove that and try again

Bernhard

[mgz1985]

eureka...everything works now....for the time being...thanx everybody

[mahendra]

Hello Dear Foamers,

I am caught in a problem where i am having a mesh created in Gambit with internal walls.
I followed the procedure explained on wiki, using <splitmeshwithsets> and ended up with this error. Can anybody please guide me to resolve the error.

Error:

Exec : splitMeshWithSets VA_wall VA_wall_top VA_wall_bottom
Date : Oct 23 2008
Time : 12:48:55
Host : linux
PID : 31461
Case : /home/ms.wankhede/OpenFOAM/ms.wankhede-1.5/CFD_Projects/VA_20mm/VA_trial
nProcs : 1

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

Create polyMesh for time = 0



Expected a ')' or a '}' while reading PtrList, found on line 62 the word 'VA_wall_top'

file: /home/ms.wankhede/OpenFOAM/ms.wankhede-1.5/CFD_Projects/VA_20mm/VA_trial/constan t/polyMesh/boundary at line 62.

From function Istream::readEndList(const char*)
in file db/IOstreams/IOstreams/Istream.C at line 159.

FOAM exiting


Thanking you,
Mahendra

[mahendra]

Here is my constant/polymesh/boundary file:

7
(
wall
{
type wall;
nFaces 8640;
startFace 459444;
}
outer_wall
{
type wall;
nFaces 8220;
startFace 468084;
}
wall_out
{
type wall;
nFaces 4020;
startFace 476304;
}
wall_in
{
type wall;
nFaces 2820;
startFace 480324;
}
control_inlet
{
type patch;
nFaces 100;
startFace 483144;
}
VA_outlet
{
type patch;
nFaces 496;
startFace 483244;
}
VA_inlet
{
type patch;
nFaces 1696;
startFace 483740;
}
VA_wall_top // Line number 62.
{
type wall;
nFaces 0;
startFace ;
}
VA_wall_bottom
{
type wall;
nFaces 0;
startFace ;
}
)

Regards,
Mahendra.

[mahendra]

Ok i got the Problem I replaced the number 7 with number 9 since i added two more patches to the boundary file.

Now it gives segmentation fault with using <splitmeshwithsets>.
I do not want to recompile the openFOAM again, any hints to resolve this??

And after using <splitmesh> I am getting the following error:

Constructed topologyModifier:

Splitter
{
type attachDetach;
faceZoneName membraneFaces;
masterPatchName VA_wall_top;
slavePatchName VA_wall_bottom;
triggerTimes 1(0);
manualTrigger off;
active on;
}


Attempt to cast type polyMesh to type fvMesh#0 Foam::error::printStack(Foam:stream&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam:stream& Foam::operator<<>(Foam:stream&, Foam::errorManip<foam::error>) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"
#3 Foam::probes::read(Foam::dictionary const&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#4 Foam::probes::probes(Foam::word const&, Foam::objectRegistry const&, Foam::dictionary const&, bool) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#5 Foam:utputFilterFunctionObject<foam::probes>::start() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libsampling.so"
#6 Foam::functionObjectList::start() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#7 Foam::Time::operator++() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#8 main in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"
#9 __libc_start_main in "/lib64/libc.so.6"
#10 Foam::regIOobject::write() const in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"


From function refCast<to>(From&)
in file /home/dm2/henry/OpenFOAM/OpenFOAM-dev/src/OpenFOAM/lnInclude/typeInfo.H at line 106.

FOAM aborting


Again any hints to resolve the problem??


Regards,
Mahendra.

[gschaider]

Hi Mahendra!

This is an old problem with functionObjects and mesh-utilities. The mesh utilities generate polyMeshes, the function objects expect fvMesh and fails (something along these lines). The solution is to go to the controlDict and comment the whole functions-entry out. Then run the utility. Then uncomment the stuff.

Or (beware: advertising) use a recent version of pyFoamRunner.py where the --remove-functions-option does the commenting (and uncommenting) for you

Bernhard

[mahendra]

No Luck Bernhard .....
I tried commenting the function objects...still there is error of this sort...

Determining visibility from point 50740
Adding point and face zones

Constructed topologyModifier:

Splitter
{
type attachDetach;
faceZoneName membraneFaces;
masterPatchName VA_wall_top;
slavePatchName VA_wall_bottom;
triggerTimes 1(0);
manualTrigger off;
active on;
}


Problem : Patch VA_wall_top starts at 0
Current face counter at 485436
Are patches in incremental order?#0 Foam::error::printStack(Foam:stream&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::polyTopoChange::addMesh(Foam::polyMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::List<int> const&, Foam::List<int> const&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#3 Foam::polyTopoChange::polyTopoChange(Foam::polyMes h const&, bool) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#4 Foam::polyTopoChanger::topoChangeRequest() const in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#5 Foam::polyTopoChanger::changeMesh(bool, bool, bool, bool) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#6 Foam::attachPolyTopoChanger::attach(bool) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libdynamicMesh.so"
#7 main in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"
#8 __libc_start_main in "/lib64/libc.so.6"
#9 Foam::regIOobject::write() const in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"


From function polyTopoChange::polyTopoChange(const polyMesh& mesh, const bool strict)
in file polyTopoChange/polyTopoChange/polyTopoChange.C at line 2332.

FOAM aborting

Bythe way I am using OpenFOAM 1.5

Mahendra.

[gschaider]

Hi Mahendra!

I'm not sure, but as I remember it the implicit startFace ("startFace ;") stopped working in v1.4 or so and this might be your problem (he starts the new patches a face 0 which is an internal face). You will have to set it to after the last face for the two empty faces ("startFace 485436;" judging from your output. Could be +/- 1, try)

Bernhard

[mahendra]

Dear Bernhard

I tried your suggestion; I replaced the startFace with the number prompted 485436.. and it worked. It created a directroy "1" containing 'polymesh" directory and in it contained the dictionary named "meshmodifiers".

But i do not which polymesh will OpenFoam use during simulation !

anyways I have launched the case and now the simulation is running. I will get back with the results.

Thanks.
Mahendra.

[mahendra]

Dear Bernhard hi !

I am still facing problems with gambit mesh having internal faces as walls.

Here is the error.....
Please help.......

Determining visibility from point 69065
Adding point and face zones


point, face or cell zone already exists#0 Foam::error::printStack(Foam:stream&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::polyMesh::addZones(Foam::List<foam::pointzon e*> const&, Foam::List<foam::facezone*> const&, Foam::List<foam::cellzone*> const&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 main in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"
#4 __libc_start_main in "/lib64/libc.so.6"
#5 Foam::regIOobject::write() const in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"


From function void addZones
(
const List<pointzone*>& pz,
const List<facezone*>& fz,
const List<cellzone*>& cz
)
in file meshes/polyMesh/polyMesh.C at line 871.

FOAM aborting

Aborted
ms.wankhede@linux:~/OpenFOAM/ms.wankhede-1.5/CFD_Projects/Disk_Imp>

[mahendra]

Dear Bernhard,

My problem is solved,

I did fluentMeshToFoam -writeSets
earlier i was doing fluentMeshToFoam -writeSets -writeZones

Thanks,
Mahendra.

[mahendra]

Dear Bernhard hello..........

As i mentioned earlier, I am having problems with converting a gambit mesh with internal faces as walls to OpenFOAM.

This is mesh having internal walls as well as a MRF zone.

I first created the MRF zones using

fluentMeshToFoam <meshfile> -writeSets -writeZones

then, when I am creating walls using splitMesh command I am getting into trouble...

This the error it gives...


Determining visibility from point 69065
Adding point and face zones


point, face or cell zone already exists#0 Foam::error::printStack(Foam::-Ostream&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::polyMesh::addZones(Foam::List<foam::pointzon e*> const&, Foam::List<foam::facezone*> const&, Foam::List<foam::cellzone*> const&) in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 main in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"
#4 __libc_start_main in "/lib64/libc.so.6"
#5 Foam::regIOobject::write() const in "/home/ms.wankhede/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/splitM esh"


From function void addZones
(
const List<pointzone*>& pz,
const List<facezone*>& fz,
const List<cellzone*>& cz
)
in file meshes/polyMesh/polyMesh.C at line 871.

FOAM aborting


Now can u please help me resolving this error?

Regards,
Mahendra.