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

Issues with mapFields

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 6, 2010, 12:03
Default Issues with mapFields
  #1
New Member
 
Austin French
Join Date: Aug 2010
Location: Adelaide, Australia
Posts: 1
Rep Power: 0
BlackBoatNavArch is on a distinguished road
Hi all.

I'm trying to use the mapFields utility to go from a coarser mesh to a finer one. I'm interested in refining the mesh around a body and have been using refinement regions in snappyHexMesh. The surface refinement on the body isn't changing at all, so the body meshes should be ~identical.

After solving my coarser mesh to 1000 steps, I run the mapFields two different ways and get two different problems.

Using -consistent, I get a target folder at the correct time in my new finer mesh. The interpolation has some issues but seemingly not near regions that are newly refined. Namely, I get small regions decreasing velocity to 0, which isn't ideal, but I think running the solution should get rid of them. The problem is I also get negative values of omega at those regions. This trips the bounding omega in the log file when I try to solve and the solver crashes. The error message has a lot about turbulence models and FPE's but I certainly don't find it particularly helpful.

Using the mapFieldDict method, I get the following output.

Code:
xxx@XXX-linux:~/OpenFOAM/xxx-1.7.1/run/domain_1b$ mapFields ../domain_1a
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-320803922ee1
Exec   : mapFields ../domain_1a
Date   : Nov 07 2010
Time   : 01:30:07
Host   : XXX-linux
PID    : 13179
Case   : /home/xxx/OpenFOAM/xxx-1.7.1/run/domain_1b
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Source: ".." "domain_1a"
Target: "/home/xxx/OpenFOAM/xxx-1.7.1/run" "domain_1b"

Create databases as time

Source time: 1000
Target time: 1000
Create meshes

Source mesh size: 1130080    Target mesh size: 1824109


Mapping fields for time 1000


End
Again the times line up, and the meshes are correct. But the fields aren't interpolated at all and I do not get a new folder for time = 1000. I think it might be my mapFieldDict file, but I've followed the advice of other threads and the OpenFOAM manual.

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      mapFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

patchMap        
(
    inboard inboard
    outboard outboard
    inlet inlet
    outlet outlet
    bottomAndTop bottomAndTop    
    hull_BL_A_O hull_BL_A_O
);

cuttingPatches  
(
    
);


// ************************************************************************* //
The mapFieldsDict method runs through all the interpolate fields if I have already run -consistent, but the second interpolation doesn't change the values at all. I'm using OpenFoam 1.7.1 which doesn't require a target field as was noted in at least one other thread and attempting to put one in gives an argument error as expected.

So, I'm not entirely sure what to do. Obviously, not having to solve the whole 1.8mil mesh would be nice since its just a mesh refinement. I'm finding this problem is intermittent. Sometimes I am able to use -consistent and don't get the negative omega values. It varies with the mesh refinement that I am starting with and what I add to it. Which is all very frustrating.
BlackBoatNavArch is offline   Reply With Quote

Old   January 13, 2011, 06:09
Default
  #2
Senior Member
 
Matthias Voß
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 441
Rep Power: 11
mvoss is on a distinguished road
hi,

i am having the same problem. mapFields running without error but also without creating something.

Did you found a solution?
mvoss is offline   Reply With Quote

Old   January 16, 2011, 14:12
Default
  #3
Member
 
Usit McCarra
Join Date: Oct 2010
Posts: 51
Blog Entries: 2
Rep Power: 6
McCarra is on a distinguished road
In my case it works executing:

mapFields directory_example/case_directory -sourceTime latestTime

I left patchMap and cuttingPatches subDicts blank in the mapFieldsDict, but I created beforehand the temporal directory.

Have a look at your time directory named "100" (latest time) because it should exist. Your simulation should reach the latest time to map the results and write it. If it is not created check the writing interval in controlDict.

In my case the mesh size is the same but the geometry is different because it is a dynamic mesh problem. I have not tried with meshes of other sizes.
McCarra is offline   Reply With Quote

Old   February 12, 2011, 15:24
Default
  #4
Member
 
Mohammad.R.Shetab
Join Date: Jul 2010
Posts: 49
Rep Power: 6
mrshb4 is on a distinguished road
Hi
Is it possible to map all the time directories of a case, to another one?!
I mean map data from directories 0, 0.01, 0.02, 0.03, ..... of case 1 into directories 0, 0.01, 0.02, 0.03, ..... of case 2, all with one command?!!
mrshb4 is offline   Reply With Quote

Old   April 12, 2011, 13:07
Default
  #5
New Member
 
Mark Beal
Join Date: Feb 2011
Posts: 24
Rep Power: 6
msbealo is on a distinguished road
Did you ever solve this? I'm having exactly the same problem. If I use -consistent I get negative omega values and my solver gives up, if I use mapFieldsDict (with blank entries) I don't get an output.

I'm trying to map between a coarse and a medium mesh where the mesh density has only been changed by upping the values in blockMeshDict before running snappyHexMesh.

I've tried:

Code:
mapFields ../Coarse -consistent
(negative values and solver problems)
Code:
mapFields ../Coarse -sourceTime 10
(no output, "10" is the last time step)
Code:
mapFields ../Coarse -sourceTime 0
(nothing)
Code:
mapFields ../Coarse -sourceTime latestTime
(nothing)

For each of the the cases I get a similar shell output of

Code:
Build  : 1.7.x-131caa989cd3
Exec   : mapFields ../Coarse -sourceTime latestTime
Date   : Apr 12 2011
Time   : 18:01:07
Host   : msbealo-desk
PID    : 7678
Case   : /home/msbealo/OpenFOAM/msbealo-1.7.1/run/Medium
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Source: ".." "Coarse"
Target: "/home/msbealo/OpenFOAM/msbealo-1.7.1/run/" "Medium"

Create databases as time

Source time: 10
Target time: 10
Create meshes

Source mesh size: 274765    Target mesh size: 495044


Mapping fields for time 10


End
My mapFieldsDict looks like:

Code:
patchMap ( );

cuttingPatches  ( );
I've also tried explicitly stating which patches to copy using (inlet inlet etc) with not change.

Any help please? I know it's probably something pretty silly.

Mark
msbealo is offline   Reply With Quote

Old   April 12, 2011, 14:26
Default
  #6
Member
 
Usit McCarra
Join Date: Oct 2010
Posts: 51
Blog Entries: 2
Rep Power: 6
McCarra is on a distinguished road
maybe mapFields is not able to interpolate between meshes of different sizes. I'll try to figure it out.
McCarra is offline   Reply With Quote

Old   April 13, 2011, 08:14
Default
  #7
Member
 
Mohammad.R.Shetab
Join Date: Jul 2010
Posts: 49
Rep Power: 6
mrshb4 is on a distinguished road
Hi

I think you should make a temporary folder in the case and initial files of fields you want to map should be there.
For example:
if you want to map field omega from time 5 of coarse mesh to omega field from time 5 of fine mesh you should:

1- make a directory of time 5 in fine mesh case.
2- in that folder you should have a dictionary of omega that indicate boundary conditions ( the same as dictionary that you write in your 0 dictionary)
3-In your controlDict of case fine, change startTime to 5.
4- run the command "mapFields ../Coarse"

It will map field omega from folder 5 of case coarse to folder 5 of case fine.

Thats it!
Mohammadreza
codder likes this.
mrshb4 is offline   Reply With Quote

Old   April 13, 2011, 08:58
Default
  #8
New Member
 
Mark Beal
Join Date: Feb 2011
Posts: 24
Rep Power: 6
msbealo is on a distinguished road
Mohammadreza

Thanks! That seems to be working. I'm currently running something in the background so I can't test it fully but it does run using your suggestions.

Regards,

Mark
msbealo is offline   Reply With Quote

Old   June 10, 2011, 10:24
Default
  #9
New Member
 
Grim
Join Date: Mar 2011
Posts: 6
Rep Power: 6
Opxah is on a distinguished road
Yes, it seems mapFields works (only) when the source time and target time are the same.
Opxah is offline   Reply With Quote

Old   February 10, 2012, 12:18
Default
  #10
Member
 
Join Date: Sep 2011
Posts: 45
Rep Power: 5
ic3wall is on a distinguished road
Quote:
Originally Posted by BlackBoatNavArch View Post
Using -consistent, I get a target folder at the correct time in my new finer mesh. The interpolation has some issues but seemingly not near regions that are newly refined. Namely, I get small regions decreasing velocity to 0, which isn't ideal, but I think running the solution should get rid of them.
Did you figure out the problem ?

I have exactly the same issue, I have many regions where mapFields attributes 0 values which is really bad... I guess it's a question of interpolation, but did anybody find a solution ?
ic3wall is offline   Reply With Quote

Old   February 14, 2012, 09:22
Default
  #11
Member
 
Join Date: Sep 2011
Posts: 45
Rep Power: 5
ic3wall is on a distinguished road
No one found why mapFields outputs 0 values ?
ic3wall is offline   Reply With Quote

Old   February 14, 2012, 13:52
Default
  #12
New Member
 
Mark Beal
Join Date: Feb 2011
Posts: 24
Rep Power: 6
msbealo is on a distinguished road
ic3wall,

For me, I followed Mohammadreza advise (above) and it works fine. I guess the obvious question is are you mapping the right time directory from the source to the target? You're not mapping the '0' folder?

Make sure your target controlDict has the startTime of the last time of the source case. So, if you ran the first simulation to 10 seconds and then want to map this to the next case, copy the '0' time to '10' (to set up the right files), change the startTime to 10 in the target case and run mapFields.

Post the output of mapFields if you still get something strange.

Mark
__________________
Dynamic Fluid Design
www.dynamic-fluid-design.com
msbealo is offline   Reply With Quote

Old   February 14, 2012, 15:58
Default
  #13
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 725
Rep Power: 18
mturcios777 will become famous soon enough
Quote:
Originally Posted by Opxah View Post
Yes, it seems mapFields works (only) when the source time and target time are the same.
You can map inconsistent geometry as is documented in the user manual, which is what cuttingPatches and mappingPatches entries are for. When the new mesh is within the domain of the old one you still have values from which you can map fields and patches (the cavity tutorials in the manual show this clearly), but if your new domain has parts that are outside your old domain, then the default value mapFields gives those regions is 0.

I've experienced stability issues when refining meshes and wrote a utility to deal with it. The basic algorithm is:

1) Create a field with uniform value 1 in the mesh you want map FROM, call it "mark" or something
2) Create a field with uniform value -1 in the mesh you want to map TO, with the same name ("mark" in this general example)
3) Do your mapping inconsistently, and now
4) Now run through the the new "mark field", and whenever you find a cell (I restricted myself to cells) that has mark == -1, you should replace all field values (U, T, etc) for that cell with interpolations from valid nearby cells (those whose value of "mark" is 1)

How you do the interpolation is up to you. Because the differences in geometry are so small in our case, we just directly copied valid field values. If the differences are larger you should do some kind of weighted interpolation.
hua1015 likes this.
mturcios777 is offline   Reply With Quote

Old   February 14, 2012, 16:14
Default
  #14
Member
 
Join Date: Sep 2011
Posts: 45
Rep Power: 5
ic3wall is on a distinguished road
Quote:
Originally Posted by mturcios777 View Post
You can map inconsistent geometry as is documented in the user manual, which is what cuttingPatches and mappingPatches entries are for. When the new mesh is within the domain of the old one you still have values from which you can map fields and patches (the cavity tutorials in the manual show this clearly), but if your new domain has parts that are outside your old domain, then the default value mapFields gives those regions is 0.

I've experienced stability issues when refining meshes and wrote a utility to deal with it. The basic algorithm is:

1) Create a field with uniform value 1 in the mesh you want map FROM, call it "mark" or something
2) Create a field with uniform value -1 in the mesh you want to map TO, with the same name ("mark" in this general example)
3) Do your mapping inconsistently, and now
4) Now run through the the new "mark field", and whenever you find a cell (I restricted myself to cells) that has mark == -1, you should replace all field values (U, T, etc) for that cell with interpolations from valid nearby cells (those whose value of "mark" is 1)

How you do the interpolation is up to you. Because the differences in geometry are so small in our case, we just directly copied valid field values. If the differences are larger you should do some kind of weighted interpolation.
I'm mapping values from a very large field on a smaller one (which is envoloped by the bigger one) with a different mesh resolution. It is an inconsistent mapping. The zero values are scattered in the new field, this is the weird thing. The new mapped field looks like a checkerboard.

I'll try to post a picture.
ic3wall is offline   Reply With Quote

Old   February 15, 2012, 10:20
Default
  #15
Member
 
Join Date: Sep 2011
Posts: 45
Rep Power: 5
ic3wall is on a distinguished road
Here it goes, the first picture is the large field and the second one is the result of the mapping on the smaller one. The yellow rectangle in the first picture shows the smaller domain on which I'm mapping.

As you can see on the second picture, there are several zero values scattered everywhere.

Here's a part of the nonuniform List output that corresponds to the mapped field:

25921
(
0.5
0.5
0.25
0
0
0.5
0
0.5
0
0
0
0.5
0.5
0
0.5
0.5
0.5
0.25
0
0.5
0.5
0.5
0
0
0.39767
0
0
0.0518247
0.00227012
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0
0.137366
0.248451
0
0
0.488571
...)
Attached Images
File Type: jpg large.jpg (92.7 KB, 170 views)
File Type: jpg small.jpg (57.0 KB, 162 views)
ic3wall is offline   Reply With Quote

Old   February 15, 2012, 15:22
Default
  #16
Member
 
Join Date: Sep 2011
Posts: 45
Rep Power: 5
ic3wall is on a distinguished road
Problem found!

I was using mapFieldsDict incorrectly, both patches I wanted to map are coincident, so they had to be included in PatchMap(...). CuttingPatches had to be empty.

Basically I was mapping internal fields onto a surface ... which is not I what I wanted.

Thank you for your help!
ic3wall is offline   Reply With Quote

Old   May 24, 2013, 09:46
Default
  #17
New Member
 
ignacio's Avatar
 
Ignacio Gallego
Join Date: Jan 2013
Posts: 25
Rep Power: 4
ignacio is on a distinguished road
Hello all,

I will use this thread to ask another issue with mapFields.

I am using the results from a URANS simulation as initial values for LES. I use mapFields utility for this. Consisten flag on as the geometry and boundary conditions are the same.

1) If I use mapFields with ---> source: Coarse mesh, target: Fine mesh
I get he values that make no sense (Zero pressure, negative k and omega, 1000 velocity...)

2) If I use mapFields with ---> source: Fine mesh, target: Coarse mesh.
Then it works fine!

Can anybody explain me why?? Is is a bug?
I need to use the data from the URANS simulation for LES. Is there any other way I can do it without using mapFields?

Thanks a lot =)
Any idea / comment will be more than welcome
ignacio is offline   Reply With Quote

Old   May 24, 2013, 10:57
Default
  #18
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,055
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Always I am using mapFields everything is working

Code:
 
mapFields -sourceTime latestTime -case ../coarseMeshSimulationName/
The entries in the mapFieldsDict are empty.!

Works perfekt all the time.
Tobi is offline   Reply With Quote

Old   May 24, 2013, 13:27
Default
  #19
New Member
 
ignacio's Avatar
 
Ignacio Gallego
Join Date: Jan 2013
Posts: 25
Rep Power: 4
ignacio is on a distinguished road
Happy to know that it works perfectly for you.

But mine is just so crap at some cells as you can see on the pic
Attached Images
File Type: jpg Temp.jpg (89.8 KB, 96 views)
ignacio is offline   Reply With Quote

Old   April 10, 2014, 01:15
Default Plane normal defined with zero length
  #20
New Member
 
Ripudaman Manchanda
Join Date: May 2013
Posts: 29
Rep Power: 4
ripudaman is on a distinguished road
Hi all,

I am having some problem in using the mapFields utility.
When I map from coarse to fine mesh the utility works fine and gives me a clean result.
However on trying to go from one level of refinement (region refinement using SHM) in one mesh to another level of refinement (refinement close to an imported STL file in SHM) in another mesh mapfields creates problems

Here is when I face the problem:-

I refine a region of my mesh and run my solver. Next I create a different coarse mesh with an STL file in the region of the previous refinement (using shm) and try mapping the results from the latest time of my refined mesh to the coarse mesh. This gives me the following error. I have posted the gdb output here. Please note that the points mentioned in the error output are not near the new STL file.
Code:
(gdb) r ../frac1 -sourceTime 'latestTime'
Starting program: /opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/mapFields ../frac1 -sourceTime 'latestTime'
[Thread debugging using libthread_db enabled]
Using host libthread_db library "/lib/x86_64-linux-gnu/libthread_db.so.1".
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.x-e0d5f5a218ab
Exec   : /opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/mapFields ../frac1 -sourceTime latestTime
Date   : Apr 10 2014
Time   : 00:05:53
Host   : "ubuntu"
PID    : 9303
Case   : /home/ripuvm/OpenFOAM/ripuvm-2.3.x/multiFrac/cases/Consecutive1Well/frac2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Source: ".." "frac1"
Target: "/home/ripuvm/OpenFOAM/ripuvm-2.3.x/multiFrac/cases/Consecutive1Well" "frac2"

Create databases as time
Case   : ../frac1
nProcs : 1

Source time: 133
Target time: 54

Create meshes

Source mesh size: 68670    Target mesh size: 83482


Creating and mapping fields for time 133

Creating mesh-to-mesh addressing for region0 and region0 regions using cellVolumeWeight


--> FOAM FATAL ERROR: 
Plane normal defined with zero length
Bad points:(15.24 -114.3 -22.86) (15.24 -106.68 -22.86) (15.24 -99.06 -22.86)

    From function void plane::calcPntAndVec
(
    const point&,
    const point&,
    const point&
)

    in file meshes/primitiveShapes/plane/plane.C at line 116.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::plane::calcPntAndVec(Foam::Vector<double> const&, Foam::Vector<double> const&, Foam::Vector<double> const&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#3  Foam::tetOverlapVolume::tetTetOverlapVol(Foam::tetPoints const&, Foam::tetPoints const&) const in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#4  Foam::tetOverlapVolume::cellCellOverlapVolumeMinDecomp(Foam::primitiveMesh const&, int, Foam::primitiveMesh const&, int, Foam::treeBoundBox const&) const in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libmeshTools.so"
#5  Foam::meshToMeshMethod::interVol(int, int) const in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#6  Foam::cellVolumeWeightMethod::calculateAddressing(Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, int, int, Foam::List<int> const&, Foam::List<bool>&, int&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#7  Foam::cellVolumeWeightMethod::calculate(Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&, Foam::List<Foam::List<int> >&, Foam::List<Foam::List<double> >&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#8  Foam::meshToMesh::calcAddressing(Foam::polyMesh const&, Foam::polyMesh const&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#9  Foam::meshToMesh::calculate() in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#10  Foam::meshToMesh::meshToMesh(Foam::polyMesh const&, Foam::polyMesh const&, Foam::meshToMesh::interpolationMethod const&, Foam::HashTable<Foam::word, Foam::word, Foam::string::hash> const&, Foam::List<Foam::word> const&) in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libsampling.so"
#11  
 in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/mapFields"
#12  
 in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/mapFields"
#13  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14  
 in "/opt/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/mapFields"

Program received signal SIGABRT, Aborted.
0x00007ffff4260425 in raise () from /lib/x86_64-linux-gnu/libc.so.6
Any help will be highly appreciated.

Thank you.
Regards,
Ripu
ripudaman is offline   Reply With Quote

Reply

Tags
-consistent, mapfields, mapfieldsdict

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
FLUENT Speed Issues on Cluster cfd23 FLUENT 2 April 3, 2010 23:43
mapFields problems andrea.pasquali OpenFOAM 1 February 17, 2010 23:57
mapFields ignores sourceTime for -parallel source andersking OpenFOAM Bugs 2 September 2, 2009 10:38
mapFields between inconsistent meshes nikwin OpenFOAM Pre-Processing 7 July 30, 2009 04:35
MapFields to New Grid For Extreme Grid Deformations due to Body Motion albcem OpenFOAM 0 May 5, 2009 14:17


All times are GMT -4. The time now is 02:19.