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

Waves2Foam Related Topics

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

Like Tree123Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2014, 08:48
Default
  #721
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Nick,

There seems to be a problem with the relaxation zone, please do verify that it is correctly specified. You could e.g. use the relaxationZoneLayout utility to do that.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 22, 2014, 13:39
Default
  #722
New Member
 
Nick Krgs
Join Date: Jan 2014
Posts: 13
Rep Power: 4
Nick_civ is on a distinguished road
Hi Niels ,

Thank you for your instant reply. The problem was the orientation of the relaxation zone. I corrected and it started to run but it stopped after a few seconds printing the following message :


#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::sampledSurfaceElevation::sampleIntegrateAndW rite(Foam::sampledSurfaceElevation::fieldGroup<dou ble>&) in "/home/nikos/OpenFOAM/nikos-2.2.2/platforms/linux64GccDPOpt/lib/libwaves2FoamSampling.so"
#4 Foam::OutputFilterFunctionObject<Foam::sampledSurf aceElevation>::execute(bool) in "/home/nikos/OpenFOAM/nikos-2.2.2/platforms/linux64GccDPOpt/lib/libwaves2FoamSampling.so"
#5 Foam::functionObjectList::execute(bool) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::Time::run() const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7
in "/home/nikos/OpenFOAM/nikos-2.2.2/platforms/linux64GccDPOpt/bin/waveFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/home/nikos/OpenFOAM/nikos-2.2.2/platforms/linux64GccDPOpt/bin/waveFoam"

It seems to be something about Surface Elevation and i am trying to figure out what 's going on. I used as a basis the waveFlume. Is the stl object which causes the failure? i tried to reduce the number of gauges but it didn't work. Could you help me?

Thank you in advance.
Nick
Attached Files
File Type: txt log waveFoam.txt (32.6 KB, 18 views)
Nick_civ is offline   Reply With Quote

Old   February 23, 2014, 04:08
Default
  #723
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Nick,

I tried it on my OF2.2.0 installation (do not have OF2.2.2), and everything was running correctly.

The only thing I can think of (if you have not modified the case, since it was uploaded) is some cross-version compatibility issue. I would be glad, if you can track down the issue.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 23, 2014, 11:50
Default
  #724
New Member
 
Nick Krgs
Join Date: Jan 2014
Posts: 13
Rep Power: 4
Nick_civ is on a distinguished road
Hi Niels,

It was a cross-version compatibility issue indeed which has to do with SurfaceElevation and WaveGaugesNProbes. I think the problem stems from these lines in the surfaceElevation.C code :

#if OFVERSION<220
fileName dict("surfaceElevationDict");
#else
fileName dict("system/surfaceElevationDict");
#endif.

I managed to run the case in 2 different ways :

1. I deleted the last four lines from system/controlDict file
functions
{
#includeIfPresent "../waveGaugesNProbes/surfaceElevationAnyName_controlDict";
}
(running without surfaceElevation)

2. After typing waveGaugesNProbes in the terminal and before setwavefields, I copied the directory waveGaugesNProbes (which was created) inside the system directory in order for controlDict to read the appropriate file. (changing #includeIfPresent "../waveGaugesNProbes/surfaceElevationAnyName_controlDict"; to "../surfaceElevationAnyName_controlDict")

But the surfaceElevation and Postprocesswaves2foam apps don't work and i 'll try to figure out how to modify the codes in order to put the files into appropriate directories.

I think that this issue concerns all after-Openfoam 2.2.0 users and I would appreciate it if you guided me how to have these useful tools at my disposal.

Thank you for your help.

Kind regards,
Nick

Last edited by Nick_civ; February 23, 2014 at 14:48.
Nick_civ is offline   Reply With Quote

Old   February 23, 2014, 15:27
Default
  #725
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Nick,

This sounds really strange. I am going to have a busy week, so I do not know, whether I will have a chance to look into it; especially because I need also to get a 2.2.2 running.

Also, the point you are referring to with the pre-processing statements might not be the reason, as I could get things running in 2.2.0, and the statement refers the versions prior to 2.2.0.

What do you mean with postProcessWaves2Foam does not work?

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 23, 2014, 16:23
Default
  #726
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Nick,

Also, I just ran your test in OF2.2.1, and I do not experience any problems what so ever. I can sample in run-Time and postProcessWaves2Foam executes without any problems.

Kind regards,

Niels

P.S. It should be said that I am executing the test without the breakwater, i.e. the simple blockMesh-mesh.
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 23, 2014, 18:38
Default
  #727
New Member
 
Nick Krgs
Join Date: Jan 2014
Posts: 13
Rep Power: 4
Nick_civ is on a distinguished road
Hi Niels,

I ran the case without copying the waveGaugesNProbes Directory into system directory as I mentioned above but modifying #includeIfPresent "../waveGaugesNProbes/surfaceElevationAnyName_ controlDict"; to #includeIfPresent "../surfaceElevationAnyName_ controlDict";.

I used snappyhexmesh and extrudemesh for the breakwater. I also ran tests with sloped seabed using snappyhexmesh again inside and outside the relaxation zone. All cases ran successfully with the above modification but when i execute postProcessedWaves2Foam i receive the attached output.

Kind regards,
Nick
Attached Files
File Type: txt log postProcessWaves2Foam.txt (2.0 KB, 29 views)
File Type: txt log surfaceElevation.txt (2.8 KB, 28 views)
Nick_civ is offline   Reply With Quote

Old   February 24, 2014, 12:19
Default
  #728
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Nick,

Problem with surfaceElevation is that it cannot find the correct dictionary in <root>/system. You need to "create" that dictionary prior to executing surfaceElevation, but it is actually already in your waveGuagesNProbes directory.

Furthermore, the problem with postProcessWaves2Foam is (probably) that the inputDir that you are pointing to does not exist. It is on my to-do list to actually throw an error message, if the file you are supposed to read does not exist.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 25, 2014, 04:37
Default
  #729
New Member
 
Nick Krgs
Join Date: Jan 2014
Posts: 13
Rep Power: 4
Nick_civ is on a distinguished road
Hi Niels,

First of all, I found out that the problem with waveFoam running was due to extrudeMesh because the gauges' z coordinates were out of the new Mesh. I changed their values according to the after-extrudeMesh z coordinate and all cases ran succesfully without having to change anything from what i mentioned above ( namely, #includeIfPresent "../waveGaugesNProbes/surfaceElevationAnyName_controlDict"; to "../surfaceElevationAnyName_controlDict") which means that everything runs properly in Openfoam 2.2.2.

Secondly, I follow your instructions for surfaceElevation and postProcessedWaves 2Foam and i executed both correctly.

Lastly, I have pinpointed one mistake with pressure values as you can see in paraview. It depicts the p_rgs as if it is the alpha 1 and pressure values are too high. Is it because of my sealevel setting(10.40) and how can I get the right values?

Thank you very much for your guidance. It was very helpful and i have already run several cases.


Kind regards,
Nick
ngj and scator like this.
Nick_civ is offline   Reply With Quote

Old   February 25, 2014, 10:23
Default surfaceElevation probes with dynamic mesh (meshMotion)
  #730
Member
 
Ed Ransley
Join Date: Jul 2012
Posts: 30
Rep Power: 6
Ed R is on a distinguished road
Hi Niels and other waves2Foamers,

I'm struggling to get the surfaceElevation function objects to work when using the dynamic mesh solver waveDyMFoam. the solver works fine and I get good results for the CoM of a floating buoy but I cannot record the surface elevation during run time by the waveGauges and probes or the function objects methods which work fine with waveFoam. Here is the error message I get, I wonder if this make any more sense to you than me. Thanks a lot, Ed

Interface Courant Number mean: 2.65114e-09 max: 0.000190931
Courant Number mean: 6.8222e-07 max: 0.0226919
deltaT = 0.00143023
Time = 0.00262784

[1] #0 Foam::error:rintStack(Foam::Ostream&)[0] #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1 Foam::sigSegv::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #2 in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2 in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #3 Foam::valuePointPatchField<Foam::Vector<double> >::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #4 Foam::displacementLaplacianFvMotionSolver::solve() in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3 Foam::valuePointPatchField<Foam::Vector<double> >::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4 Foam::displacementLaplacianFvMotionSolver::solve() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfvMotionSolvers.so"
[0] #5 Foam::motionSolver::newPoints() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
[0] #6 Foam::dynamicMotionSolverFvMesh::update() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfvMotionSolvers.so"
[1] #5 Foam::motionSolver::newPoints() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
[0] #7
in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicMesh.so"
[1] #6 Foam::dynamicMotionSolverFvMesh::update()[0] in "/home/coast/OpenFOAM/coast-2.2.1/platforms/linux64GccDPOpt/bin/waveDyMFoam"
[0] #8 __libc_start_main in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
[1] #7 in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #9

[0] in "/home/coast/OpenFOAM/coast-2.2.1/platforms/linux64GccDPOpt/bin/waveDyMFoam"
[COAST:26895] *** Process received signal ***
[COAST:26895] Signal: Segmentation fault (11)
[COAST:26895] Signal code: (-6)
[COAST:26895] Failing at address: 0x3e80000690f
[COAST:26895] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7ff7a2de64a0]
[COAST:26895] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7ff7a2de6425]
[COAST:26895] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7ff7a2de64a0]
[COAST:26895] [ 3] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam20valuePointPatchFieldINS_6 VectorIdEEE12updateCoeffsEv+0x26) [0x7ff7a40506d6]
[COAST:26895] [ 4] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfvMotionSolvers.so(_ZN4Foam35displacementLaplac ianFvMotionSolver5solveEv+0x9d) [0x7ff79a59d2cd]
[COAST:26895] [ 5] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicMesh.so(_ZN4Foam12motionSolver9newPoints Ev+0x1d) [0x7ff7a5ea794d]
[COAST:26895] [ 6] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so(_ZN4Foam25dynamicMotionSolverF vMesh6updateEv+0x2a) [0x7ff7a597c56a]
[COAST:26895] [ 7] waveDyMFoam() [0x4254a1]
[COAST:26895] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7ff7a2dd176d]
[COAST:26895] [ 9] waveDyMFoam() [0x42e1cd]
[COAST:26895] *** End of error message ***
[1] in "/home/coast/OpenFOAM/coast-2.2.1/platforms/linux64GccDPOpt/bin/waveDyMFoam"
[1] #8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #9 --------------------------------------------------------------------------
mpirun noticed that process rank 0 with PID 26895 on node COAST exited on signal 11 (Segmentation fault).
--------------------------------------------------------------------------
Ed R is offline   Reply With Quote

Old   February 27, 2014, 18:04
Default version 2.3
  #731
Member
 
Kevin Maki
Join Date: Mar 2009
Location: Ann Arbor, MI, USA
Posts: 43
Rep Power: 9
kjmaki is on a distinguished road
Hi Niels,

Any plans to extend waves2Foam to version 2.3? I just downloaded waves2fFoam from the svn, and to compile I had to comment out the coordinateRotation in rawVelocityProbes.C, and then I modified the 2.3.x version of interFoam to match waves2Foam, but there appears to be an issue with the alpha1 to alpha.water transition.

Thanks for any help you can provide!

Kevin
kjmaki is offline   Reply With Quote

Old   February 27, 2014, 19:39
Default
  #732
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Hi Kevin,

Yes, I am planning on trying to get it running on 2.3., but it is a sparetime project, so I cannot say anything on the time horizon. I am seriously thinking of only supporting the %d.%d versions and not the sub-version, because they are simply released too often with enough modification to make the compilation somewhat troublesome.

Could you kindly elaborate more on the alpha thing. I do not think that I quite caught that one.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 28, 2014, 07:36
Default Spilling breakers
  #733
New Member
 
Scott
Join Date: Mar 2013
Posts: 2
Rep Power: 0
sb612 is on a distinguished road
Hi Niels,

I have spent quite a lot of time attempting to replicate the surface elevation and undertow results for spilling waves from your paper/thesis using the waves2Foam toolbox with OpenFOAM 2.2.0. I have had a number of problems and any help which you can give would be very much appreciated.

As you pointed out in your thesis, the standard implementation of the k-omega model in OpenFOAM does not perform well. In my experience, the waves do not even seem to break due to excessive damping. Therefore, I have tried adding the changes which you have suggested:

a) The modified production term and new value for alpha
b) The cross diffusion term.
c) Density in each term.

Changes a and b seem to have been implemented correctly but although the simulation runs, the model still does not perform well. On the other hand, change c gives more promising results in the early stages of the simulation but as soon as the first wave breaks, the simulation becomes unstable and soon after crashes. The attached image shows the free surface and turbulent kinetic energy at the start of the first breaking wave (top) and the next write time (bottom). Note that the TKE in the air just above the breaker jumps approximately two orders of magnitude in that time.

Bearing all of this in mind, I have a few of questions:
  1. Did you have any stability problems when running the spilling breakers case? If yes, do you have any suggestions on how to improve it?
  2. How did you include density in the equation? Did you pass rho and rhoPhi from waveFoam to the turbulence model and then include these in each of the terms in the two transport equations?
  3. You say in your thesis that the values for k and omega at the inlet/atmosphere are small fixed values such that nut<<nu. However, I have found that if I choose small fixed values my simulation crashes. To get it to run I have had to use inletOutlet conditions. Is it possible for you to tell me the exact values which you specified on your boundaries?
Many thanks,

Scott
Attached Images
File Type: png unstable-TKE2.png (67.5 KB, 69 views)
lxwd and mo_na like this.
sb612 is offline   Reply With Quote

Old   February 28, 2014, 10:55
Default
  #734
Member
 
Kevin Maki
Join Date: Mar 2009
Location: Ann Arbor, MI, USA
Posts: 43
Rep Power: 9
kjmaki is on a distinguished road
Niels,

Thanks for your reply.

I know that your support of the various versions requires a significant amount of effort.

I have compiled your library for 2.3. Here is a very coarse description of the necessary modifications;

* commented out the cooordinateRotation in src/waves2FoamProcessing/postProcessing/postProcessingWave
s/writeRawData/rawVelocityProbes/rawVelocityProbes.C

* commented out the call to compile in src/waves2FoamPorosity in file src/Allwmake

* search and replace alpha1 with alpha.water in all files in src and in applications/utilities

* search and replace phase1 with water and phase2 with air in all files in applications/utilities

The last two bits have to do with the changing to the multiphase naming convention. See more here: http://www.openfoam.org/version2.3.0/multiphase.php.

Best wishes,

Kevin
kjmaki is offline   Reply With Quote

Old   February 28, 2014, 12:58
Default
  #735
New Member
 
behrang chenari
Join Date: Nov 2013
Location: Coimbra, Portugal
Posts: 11
Rep Power: 5
Behrang is on a distinguished road
Send a message via Skype™ to Behrang
Hi Neils,

I would like to know why you considered zeroGradient boundary condition for the outlet's pressure field?
Also can you suggest me a document to know find something in detail about the boundary conditions used in waves2Foam.

Best,
Behrang
Behrang is offline   Reply With Quote

Old   February 28, 2014, 14:09
Default
  #736
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Good evening,

@Kevin: Thank you for the summary. It will prove helpful, even though it sounds bad that you had to turn so many things off.
What is your initial experience with the new VOF method? Does it go faster with an equally good accuracy?

@Behrang: Read sections 1.2, 1.5 and 7 on the wiki. These adress your questions.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   February 28, 2014, 14:45
Default
  #737
Member
 
Kevin Maki
Join Date: Mar 2009
Location: Ann Arbor, MI, USA
Posts: 43
Rep Power: 9
kjmaki is on a distinguished road
Niels,

The changes are not as many, now that I am looking back on them. I have had my own implicit VOF for a while, and the new one is quite nice. I have not done careful testing yet, but some preliminary cases has shown it to deliver as promised. That is I can run with Courant numbers in the range of 2-30, with no problem. For example, the waveFlume tutorial runs great at a Courant number of 15, which is a speed up of 60.

Onward we march......

Kevin
kjmaki is offline   Reply With Quote

Old   February 28, 2014, 14:59
Default
  #738
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Wow! You just convinced me to have fun compiling tomorrow - fingers crossed for a rainy day

And a great weekend to you,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   March 3, 2014, 01:55
Default
  #739
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,713
Rep Power: 27
ngj will become famous soon enoughngj will become famous soon enough
Good morning,

With respect to the sampling issue on moving meshes, which is reported several times in the above, have you tried to substitue the surfaceElevation functionObject with a simple line sampling?

This will help you to narrow down, whether the problem is with the sampling or with the surfaceElevation evaluation.

Kind regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   March 3, 2014, 09:02
Default
  #740
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Location: Singapore
Posts: 340
Rep Power: 8
Phicau is on a distinguished road
Quote:
Originally Posted by kjmaki View Post
Niels,

The changes are not as many, now that I am looking back on them. I have had my own implicit VOF for a while, and the new one is quite nice. I have not done careful testing yet, but some preliminary cases has shown it to deliver as promised. That is I can run with Courant numbers in the range of 2-30, with no problem. For example, the waveFlume tutorial runs great at a Courant number of 15, which is a speed up of 60.

Onward we march......

Kevin
Hi Kevin,

AFAIK this is the maximum Courant that is allowed, can you confirm us that in your simulation the real Co reached such a large value? Remember that dt can also be constrained by 'maxDeltaT' or even by the output interval.

IMHO we should be very careful with this feature, one thing is the underlying numerics, which may allow you to use an infinitely large time step and a very different thing is the physics we are solving. When you are dealing with transient wave simulation most of the times you need a degree of accuracy that can only be achieved by using a Co smaller than 1. See how the damBreak case still uses Co = 1.

Steady-state simulations are a different world (and not usually my field), but it seems to me like this feature was specifically designed for them.

Best regards,

Pablo
Phicau 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
Other Topics at OpenFOAM Workshop Milan 2008 hjasak OpenFOAM 2 October 26, 2013 04:33
Sections / Topics in CFD Wiki Roberthealy1 CFD-Wiki 6 August 23, 2007 17:58
CFD Related Educational Programmes Jonas Larsson Main CFD Forum 3 February 9, 2007 11:11
project topics vivekanand CFX 0 October 27, 2004 05:17
Advanced Topics in Aerodynamics Antonio Filippone Main CFD Forum 0 August 28, 1999 12:16


All times are GMT -4. The time now is 14:37.