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

Any update on mixerGgiFvMesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 13, 2009, 00:19
Default Hello again Christina, Base
  #41
Senior Member
 
Martin Beaudoin
Join Date: Mar 2009
Posts: 330
Rep Power: 13
mbeaudoin will become famous soon enough
Hello again Christina,

Based on your test case (rotor2Dggi.rar) and on the syntax used for the ggi patches definition in your boundary file, I can affirm right away that you are using a slightly outdated version of OF-1.5-dev.

So the best solution I can propose to you is this:

Either

svn update

or

svn co https://openfoam-extend.svn.sourceforge.net/svnroot/openfoam-extend/trunk/Core/O penFOAM-1.5-dev OpenFOAM-1.5-dev

Recompile this new version and take your test case out for a new spin.

After a necessary modification to the ggi patch definition, your test case ran flawlessly on my system, from beginning to end, without any floating point errors.

And some of the early intermediary velocity solutions I computed are looking a lot like the little picture you posted on the IMVT Web site.

So if you plan on working with the GGI and OF-1.5-dev, I would strongly suggest that you keep your copy of OF-1.5-dev in sync with the latest version available on openfoam-extend.

You will benefit right away from a high quality version of OF, and also from all of the new GGI stuff that will be made available in the months to come.

Cheers,

Martin
mbeaudoin is offline   Reply With Quote

Old   February 18, 2009, 05:19
Default Hi My name is Fredrik Hells
  #42
New Member
 
Fredrik Hellstrom
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 9
Rep Power: 8
fredrikh is on a distinguished road
Hi

My name is Fredrik Hellstrom and I have been using FOAM 1.4.1-dev for a while. I'm performing LES computations of the flow in a radial turbine with a rotating wheel, and hence, I'm using the mixerGgiFVMesh. It works well, both in serial and parallel mode. I have recently changed to version to 1.5-dev (date:090202). The simulations with the turbine (with a rotating wheel) are working fine in serial mode, but not in parallel. At the stage when the flux should be calculated for the first point, I'm getting floating point error on all sub-domains, expect the one where the sliding interface is located (I have both sides of the sliding interface located on the same processor).

Do I do any thing wrong or is the mixerGgi function not implemented in a way that does work in parallel?


Thanks in advanced for any help or tips.


Fredrik
fredrikh is offline   Reply With Quote

Old   February 18, 2009, 07:46
Default Can you try the debug version
  #43
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Can you try the debug version and give me the traceback please?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 18, 2009, 09:28
Default Hi Hrv Here is the output (
  #44
New Member
 
Fredrik Hellstrom
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 9
Rep Power: 8
fredrikh is on a distinguished road
Hi Hrv

Here is the output (if I manage to attach the file)!



I hope it will help you!

Best regards

Fredrik
fredrikh is offline   Reply With Quote

Old   February 18, 2009, 09:38
Default Hi I will try again to uplo
  #45
New Member
 
Fredrik Hellstrom
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 9
Rep Power: 8
fredrikh is on a distinguished road
Hi

I will try again to upload the file.
slurm-401560.out

/Fredrik
fredrikh is offline   Reply With Quote

Old   February 18, 2009, 09:47
Default That won't help: I need the de
  #46
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
That won't help: I need the debug traceback with line numbers.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 18, 2009, 11:37
Default Hello Fredrik, Your trace f
  #47
Senior Member
 
Martin Beaudoin
Join Date: Mar 2009
Posts: 330
Rep Power: 13
mbeaudoin will become famous soon enough
Hello Fredrik,

Your trace file is informative enough.

Basically, we can see the 18 out of your 24 processors are crashing in a low-level GGI method used for computing the GGI weights (rescaleWeightingFactors).

This means that your GGI is spread out on more than one processor, which is currently big NO NO.

For a parallel simulation involving GGIs, you should expect to see messages related to the evaluation of the GGI weighting factors coming from only 1 out of your 'n' processors.

So I would suggest you revisit your parallel decomposition...

Martin
mbeaudoin is offline   Reply With Quote

Old   February 19, 2009, 04:04
Default Hello Martin, thanks for ha
  #48
New Member
 
Christina Smuda
Join Date: Mar 2009
Location: Germany
Posts: 12
Rep Power: 8
christinasmuda is on a distinguished road
Hello Martin,

thanks for having a look at my case. I thought my OpenFoam version was up to date because I downloaded the last update from powerlab.fsb.hr on February 2.

This morning I got the last version from SourceForge and installed it. I tried running the same case with the new version. The first thing I noticed is the missing definition of a pressure value at the ggi. Why do I have to define a pressure value at the interfaces?
These values are also missing in the mixerGgi tutorial.

Running my case I still have the same problems as before. The calculation and the flow field looks pretty good during the first timesteps until about 0.0025 s. At this point the flow field starts deverging. Increasing the number of correctors in the PISO loop I would expect the number of necessary iterations to decrease with each loop. But this doesn't happen during the calculation. The number of iterations remains at about 600.
I tried to decrease the number of correctors and non orthogonal correctors and the the floating point error comes up. Do I really need so many corrector steps for the calculation?

Do you have any idea what else I could change in order to make this case run?

Thank you very much for you help,
Christina
christinasmuda is offline   Reply With Quote

Old   February 19, 2009, 15:16
Default Hi Hrvoje and Martin My cas
  #49
New Member
 
Fredrik Hellstrom
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 9
Rep Power: 8
fredrikh is on a distinguished road
Hi Hrvoje and Martin

My case is correct decomposed; the GGI interface is on one processor.

If I delete the definition of the GGI boundary (insideSlider and outsideSlider) in each of the boundary files (processor*/constant/polyMesh/boundary) for each processor that does not contain any sliding interface it works. Of course I also have to change the number of defined boundaries in each boundary file.

I have compiled the DEBUG version, but it gives no further information than I posted few days ago. I have to check the debugSwitches in controlDict.

What do you think; can this problem be solved by modifying the decomposer or is it better to change the ggi-algorithm.

Kindly regards

Fredrik
fredrikh is offline   Reply With Quote

Old   February 22, 2009, 01:19
Default Hello Fredrik, Found the pr
  #50
Senior Member
 
Martin Beaudoin
Join Date: Mar 2009
Posts: 330
Rep Power: 13
mbeaudoin will become famous soon enough
Hello Fredrik,

Found the problem. It is now fixed.

Just update your local 1.5-dev installation from the svn repository on openfoam-extend.

Thank you for your patience.

Martin
mbeaudoin is offline   Reply With Quote

Old   February 22, 2009, 01:49
Default Hello Christina, > The firs
  #51
Senior Member
 
Martin Beaudoin
Join Date: Mar 2009
Posts: 330
Rep Power: 13
mbeaudoin will become famous soon enough
Hello Christina,

> The first thing I noticed is the missing definition of a pressure value at the ggi. Why do I have to define a pressure value at the interfaces?
>These values are also missing in the mixerGgi tutorial.

Yea, this is new. And the tutorial is not updated.

We need to explicitly specify an initial value for the ggi boundary fields because otherwise, they will all be set to 0 by default at first use.

This was causing a division by zero error when using the k-epsilon turbulence model and the GGI.

Basically, just set this initial value to the same value as the internal field.

About your simulation blowing up: can't help you much here.

I am about to run some simple ggi validation test cases in order to check if I do get strange problems as well. I will keep you posted.

Martin
mbeaudoin is offline   Reply With Quote

Old   February 22, 2009, 13:52
Default Hi Martin Thanky you, I wil
  #52
New Member
 
Fredrik Hellstrom
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 9
Rep Power: 8
fredrikh is on a distinguished road
Hi Martin

Thanky you, I will do so! I'll come back if I found any more problems.

Best regards

Fredrik
fredrikh is offline   Reply With Quote

Old   March 7, 2009, 07:08
Default Hallo, all, I am just beginn
  #53
Member
 
Hai Yu
Join Date: Mar 2009
Location: OvgU, Magdeburg
Posts: 65
Rep Power: 8
yuhai is on a distinguished road
Hallo, all,
I am just beginning to transfer from doing a 2d geometry on one computer, to a 3d geometry on a cluster.
I am wondering about how to set up the interface for turbDyMFoam in a 3D model.
Can anyone post the tutorial "mixer3D" for me? actually, I don't know where to find it. I am very grate for it.

thx in advance.
Hai Yu
yuhai is offline   Reply With Quote

Old   March 7, 2009, 08:31
Default http://powerlab.fsb.hr/ped/ktu
  #54
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 200
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/run/
louisgag is offline   Reply With Quote

Old   March 7, 2009, 08:43
Default http://wiki.uni-due.de/OpenFOA
  #55
New Member
 
Pal Schmitt
Join Date: Mar 2009
Posts: 28
Rep Power: 8
waterboy is on a distinguished road
http://wiki.uni-due.de/OpenFOAM/index.php/Tutorials
waterboy is offline   Reply With Quote

Old   March 8, 2009, 05:49
Default Thank you, Louis, thank you, P
  #56
Member
 
Hai Yu
Join Date: Mar 2009
Location: OvgU, Magdeburg
Posts: 65
Rep Power: 8
yuhai is on a distinguished road
Thank you, Louis, thank you, Pal,
I have followed the tutorial.
I just have one more question, actually, I am experiencing the same problem exectly as Christina.
I am now using 1.5-dev(090202), must I update too?
And, can anybody confirm me that, turbDyMFoam with Sliding Interface doesn't run in parallel?
Very grateful.

Regards.

Hai
yuhai is offline   Reply With Quote

Old   March 8, 2009, 12:18
Default It will run in parallel if the
  #57
Senior Member
 
louisgag's Avatar
 
Louis Gagnon
Join Date: Mar 2009
Location: Québec, QC, Canada
Posts: 200
Rep Power: 9
louisgag is on a distinguished road
Send a message via ICQ to louisgag
It will run in parallel if the GGI interface is contained in one submesh.

As for the floating point errors I can't help you there because I myself get them sometimes and sometimes don't.

-Louis
louisgag is offline   Reply With Quote

Old   March 14, 2009, 10:21
Default Hi all I have a question co
  #58
Member
 
David Hora
Join Date: Mar 2009
Location: Zürich, Switzerland
Posts: 63
Rep Power: 8
david is on a distinguished road
Hi all

I have a question concerning ggiFvPatch::makeDeltaCoeffs. In 1.4.1-dev the following expression was used for dc

dc = (1.0 - weights())/(nf() & fvPatch::delta());

In 1.5-dev the expression was modified to

dc = 1.0/max(nf() & fvPatch::delta(), 0.05*mag(fvPatch::delta()));

which leads to an overestimated dc (as far as I understand the code). What was the reason for this implementation?

Regards
David
david is offline   Reply With Quote

Old   March 14, 2009, 11:56
Default Hello David, You are compar
  #59
Senior Member
 
Martin Beaudoin
Join Date: Mar 2009
Posts: 330
Rep Power: 13
mbeaudoin will become famous soon enough
Hello David,

You are comparing pieces of code between a GGI implementation that works and a GGI implementation that did not. So you should not be surprised in seeing bug fixes here and there.

For the code snippet you are interested in, it might be easier to understand the code if you just put yourself in the situation where your GGI patches are totally conformal.

In all cases, the GGI cell to surface interpolation scheme needs to behave exactly like the basic OpenFOAM surface interpolation code.

Now take a look at the implementation of surfaceInterpolation::makeDeltaCoeffs(). You should find something quite familiar.

And for surfaceInterpolation::makeDeltaCoeffs(), there is obviously no problem in comparing the source code implementation between 1.4.1-dev and 1.5-dev; it is identical.

Cheers!

Martin
mbeaudoin is offline   Reply With Quote

Old   March 16, 2009, 06:07
Default
  #60
Member
 
David Hora
Join Date: Mar 2009
Location: Zürich, Switzerland
Posts: 63
Rep Power: 8
david is on a distinguished road
Hi Martin

I agree that the GGI cell to surface interpolation scheme needs to behave exactly like the basic OpenFOAM surface interpolation code. But I think that we introduce an error with the current implementation.

Example: pressure distribution for a 1D flow with a conformal GGI in the centre, simulated with potentialFoam

p_orig is the current 1.5-dev implementation
p_modified is calculated with

dc = 1.0/max(nf() & delta(), 0.05*mag(delta()));

As far as I understand the code, this dc should be similar to the dc in 1.4.1-dev.

Regards
david
Attached Images
File Type: png p.png (3.6 KB, 25 views)

Last edited by david; March 16, 2009 at 08:38.
david 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
velocity update fluent_urs FLUENT 6 July 8, 2008 11:41
FLEXlm update or ?? Kasper Skriver CD-adapco 2 March 1, 2007 11:38
IcoTopoFoam update hjasak OpenFOAM Running, Solving & CFD 0 March 28, 2005 21:32
UDF update profile ramesh FLUENT 0 June 29, 2003 14:14
MOUSE - any update? Pei-Ying Hsieh Main CFD Forum 1 March 19, 2001 06:04


All times are GMT -4. The time now is 05:40.