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

OF 15 FLUENT Mesh with interfaces

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 10, 2009, 04:08
Default Dear all, I am struggling t
  #1
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Dear all,

I am struggling to run meshes imported from FLUENT including interfaces. AFAIK there are two options:

1. stitchMesh -> use 1.5-dev
2. ggi -> use 1.5-dev

First option works on some vanilla cases but fails on my real life geometries with various errors and large memory consumption. Could not get it running on all types of my interfaces. So I tried ggi and I am struggling:

Starting time loop

[node013:00375] *** Process received signal ***
[node013:00375] Signal: Floating point exception (8)
[node013:00375] Signal code: (-6)
[node013:00375] Failing at address: 0xb5a00000177
[node013:00375] [ 0] /lib64/libc.so.6 [0x2b57acb3ec10]
[node013:00375] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x2b57acb3eb95]
[node013:00375] [ 2] /lib64/libc.so.6 [0x2b57acb3ec10]
[node013:00375] [ 3] /opt/OpenFOAM/OpenFOAM-1.5-dev/lib/linux64GccDPOpt/libOpenFOAM.so(_ZN4Foam6divid eERNS_5FieldIdEERKNS_5UListIdEES6_+0xa1) [0x2b57ac2f0c
71]

This is a simpleFOAM job in parallel. I guess I have to make sure interface is on one CPU? May this be the problem? How can I ensure this?

Are there furter options to handle FLUENT interfaces?

Regards
bastil is offline   Reply With Quote

Old   March 10, 2009, 04:21
Default Things to add after some more
  #2
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Things to add after some more tries:

- I also get a Floating point exception when running in seriell
- I do not know what "bridgeOverlap" is good for but I see the same behaviour if I turn it on or not.

Maybe some ggi-expert can provide me with some hints.

Regards
bastil is offline   Reply With Quote

Old   March 10, 2009, 05:16
Default Ok, I oriented on the mixerGgi
  #3
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Ok, I oriented on the mixerGgi-tutorial and gave the ggi initial values. This does not seem to be essential. If I skip that it is running in serial but it still fails in parallel. I guess this to be a decomposition problem? How can this be solved?

Regards
bastil is offline   Reply With Quote

Old   March 10, 2009, 05:46
Default > I guess I have to make sure
  #4
Member
 
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 8
josp is on a distinguished road
> I guess I have to make sure interface is on one CPU
Try:

preservePatches( patch1 patch2 ..)
preserveFaceZones( facezone1 faceZone2 ..)

in decomposeParDict

/Johan
josp is offline   Reply With Quote

Old   March 10, 2009, 05:58
Default Thanks Johan, I can not get
  #5
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Thanks Johan,

I can not get it running. How does decomposePar exactly have to look like? Is there an example hanging around somewhere? I always get:

ill defined primitiveEntry starting at keyword 'preservePatches(patch1' on line 19 and ending at line 62

Regards
bastil is offline   Reply With Quote

Old   March 10, 2009, 06:17
Default BastiL, I don't know if there
  #6
Member
 
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 8
josp is on a distinguished road
BastiL, I don't know if there are examples. There should be a ; at the end of the line aswell:
preservePatches(patch1 ..);

Could you post your dictionary?
josp is offline   Reply With Quote

Old   March 10, 2009, 06:34
Default Yes, I currently have: /*--
  #7
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Yes, I currently have:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

numberOfSubdomains 32;

method hierarchical;
//method metis;

preservePatches( patch1 patch2 );

simpleCoeffs
{
n (6 1 1);
delta 0.001;
}

hierarchicalCoeffs
{
n (32 1 1);
delta 0.001;
order xyz;
}

metisCoeffs
{
//processorWeights
//(
// 1
// 1
// 1
// 1
//);
}

manualCoeffs
{
dataFile "";
}

distributed no;

roots
(

);

// ************************************************** *********************** //


And I get:
Create time

Time = 0
Create mesh

Calculating distribution of cells
Selecting decompositionMethod hierarchical


keyword hierarchicalCoeffs is undefined in dictionary "/path/to/case/system/decomposeParDict"

file: /path/to/case/system/decomposeParDict from line 17 to line 27.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 271.

FOAM exiting

Must it be placed somewhere else?
bastil is offline   Reply With Quote

Old   March 10, 2009, 06:40
Default Ok, miving it to the end (afte
  #8
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Ok, miving it to the end (after roots ();) i get:

ill defined primitiveEntry starting at keyword 'preservePatches(patch1' on line 58 and ending at line 62
bastil is offline   Reply With Quote

Old   March 10, 2009, 08:08
Default I did not have access to my Op
  #9
Member
 
Johan Spång
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 35
Rep Power: 8
josp is on a distinguished road
I did not have access to my OpenFOAM installation earlier today.

So it should be

preservePatches (patch1 patch2); and not:
preservePatches(patch1 patch2);

Posted the decomposePar and output of a testcase below:

Good luck!

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: dev |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 32;

method hierarchical;
//method metis;

preservePatches (fan inlet);
preserveFaceZones (fanvol);

simpleCoeffs
{
n (6 1 1);
delta 0.001;
}

hierarchicalCoeffs
{
n (32 1 1);
delta 0.001;
order xyz;
}

metisCoeffs
{
//processorWeights
//(
// 1
// 1
// 1
// 1
//);
}

manualCoeffs
{
dataFile "";
}

distributed no;

roots
(

);

// ************************************************** *********************** //
~


On my system this gives
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5-extend |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : decomposePar
Date : Mar 10 2009
Time : 12:56:13
Host : linux3
PID : 9741
Case : Ggi
nProcs : 1

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

Time = 0.00688181
Create mesh

Calculating distribution of cells
Keeping owner and neighbour of faces in patches
2
(
fan
inlet
)
on same processor
Keeping owner and neighbour of faces in zones
1
(
fanvol
)
on same processor
Selected 1183862 faces whose owner and neighbour cell should be kept on the same processor
Selecting decompositionMethod hierarchical

Finished decomposition in 0.44 s

Calculating original mesh data

Distributing cells to processors

Distributing faces to processors

Calculating processor boundary addressing

Distributing points to processors

Constructing processor meshes

Processor 0
Number of cells = 5654
Number of faces shared with processor 1 = 1229
Number of processor patches = 1
Number of processor faces = 1229
Number of boundary faces = 1743

Processor 1
Number of cells = 5654
Number of faces shared with processor 0 = 1229
Number of faces shared with processor 2 = 1689
Number of processor patches = 2
Number of processor faces = 2918
Number of boundary faces = 1050

...
josp is offline   Reply With Quote

Old   March 10, 2009, 09:33
Default Thanks looks good. Seems to wo
  #10
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Thanks looks good. Seems to work now for my purposes. Only thing I am struggling with is a GGicheck-Function that makes my calculation crashing after iteration 1, Withaiut that it seems to run fine.

Regards.
bastil is offline   Reply With Quote

Old   March 11, 2009, 18:18
Default Ok I have run some tests, most
  #11
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Ok I have run some tests, most run fine some are struggling. I guess this has to do with tolerances I get warnings (will post one later) How can tolerance be controlled? And I am still wondering about the bridgeOverlap parameter - what is it good for?
bastil is offline   Reply With Quote

Old   March 12, 2009, 04:09
Default Ok on a non running case i get
  #12
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Ok on a non running case i get something like this:

Evaluation of GGI weighting factors:
--> FOAM Warning :
From function Foam::SutherlandHodgman::lineSegmentIntersection()
in file algorithms/polygon/clipping/SutherlandHodgman.C at line 109
ua does not match with ub: delta: 1.83103e-15 : epsilon: 1e-15

and:

Evaluation of GGI weighting factors:

From function void GGIInterpolation<masterpatch,>::rescaleWeightingFa ctors() const
in file /opt/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/GGIInterpolationWeights.C at line 531
Uncovered faces found: on master:0 on slave: 165
Largest slave weighting factor correction : 0.998995 average: 0.0234367
Largest master weighting factor correction: 0.0314782 average: 0.00255351

I expect at least one of these to be the problem why this case is not running. How can I find out which of my ggis cause the problem? Secnd warning sounds like there is no suport for partial ggi so far? Thanks for clarification.

Regards
bastil is offline   Reply With Quote

Old   March 12, 2009, 05:07
Default Hello all, Bastil, I am just
  #13
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 8
sponiar is on a distinguished road
Hello all,
Bastil, I am just preparing very simple testing case with ggi. This test may help me to understand how to set up case with interfaces / ggi.

This testing case looks like cavity with upper mowing wall. The cavity domain is split into the 3 blocks (see Figure 1, 2).

Fig 1.: 3 blocks, split with ggi


__________


Fig 2.: 3 blocks with mesh looks like


__________


After sucessfull runnig case, I would like use ggi with more complex geometry, where I have to use retriangulation interface which is neighbour to the side of the prismatic layer (see Figure 3)

Fig 3.: complex geometry with quad and tri interface (source TGrid mesh)


__________


Attach simple case with gambit mesh.




May I ask you for helping me with set-up case.
David
sponiar is offline   Reply With Quote

Old   March 12, 2009, 05:14
Default I hope in sucessful picture at
  #14
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 8
sponiar is on a distinguished road
I hope in sucessful picture attach.

Fig 1.: 3 blocks, split with ggi

__________


Fig 2.: 3 blocks with mesh looks like

__________


Fig 3.: complex geometry with quad and tri interface (source TGrid mesh)

__________

Attach simple case with gambit mesh:


sponiar is offline   Reply With Quote

Old   March 12, 2009, 05:53
Default Hello again, Mattijs wrote me
  #15
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 8
sponiar is on a distinguished road
Hello again,
Mattijs wrote me, that discusion board is some time full and the web browser does not responce to the attaching files.

So I attach all picture and testing case here:
http://drop.io/dsponiar

I hope this would be functional - it is for me for the first time, what I attach file any at the "on-line space".

Ragards,
David
_____
sponiar is offline   Reply With Quote

Old   March 12, 2009, 07:24
Default All of these GGIs will work wi
  #16
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,762
Rep Power: 21
hjasak will become famous soon enough
All of these GGIs will work without any trouble. For a really cool (and really new) one, have a look at: OpenFOAM: VOF + 6-DOF + GGI


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

Old   March 12, 2009, 07:56
Default Hello Hrvoje, thanks for shar
  #17
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 8
sponiar is on a distinguished road
Hello Hrvoje,
thanks for sharing nice animation. I think for me, it is so far to simulate this complex phenomenom.

Yesterday, I was building the newest OF release and testing GGI.
When I start simulation with cavity (mesh prepare in Gambit) split into the 3 blocks, I found this log:

Exec : simpleFoam -case 18-GGI_interface_OF-1.5-dev
Date : Mar 12 2009
Time : 12:45:01
Host : sponiar
PID : 29352
Case : ./18-GGI_interface_OF-1.5-dev
nProcs : 1

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

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Evaluation of GGI weighting factors:
Largest slave weighting factor correction : 1.19209e-07 average: 8.34465e-08
Largest master weighting factor correction: 1.19209e-07 average: 4.76837e-08

Evaluation of GGI weighting factors:
Largest slave weighting factor correction : 1.19209e-07 average: 1.19209e-08
Largest master weighting factor correction: 1.19209e-07 average: 1.78814e-08

Evaluation of GGI weighting factors:
Largest slave weighting factor correction : 1.19209e-07 average: 2.98023e-08
Largest master weighting factor correction: 1.78814e-07 average: 5.07743e-08

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model laminar

Starting time loop

Creating ggi check
Time = 1

PBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.52828e-06, No Iterations 8
PBiCG: Solving for Uy, Initial residual = 1, Final residual = 7.84278e-06, No Iterations 7


Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Specified mass inflow : 5.25403e-07
Specified mass outflow : 0
Difference : 5.25403e-07
Adjustable mass outflow : 5.25403e-07


From function adjustPhi
(
surfaceScalarField& phi,
const volVectorField& U,
const volScalarField& p
)
in file cfdTools/general/adjustPhi/adjustPhi.C at line 128.

FOAM exiting


I tried to set up ggi with some initialization value for velocity and pressure, but the same error occured.

Any hint?
Regards,
David
______
sponiar is offline   Reply With Quote

Old   March 12, 2009, 08:22
Default Hallo Hrv, thanks for these
  #18
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Hallo Hrv,

thanks for these hints. What about my two warnings? I found out that removing the second warning " Uncovered faces found" makes my simulation to run. this seems to be caused by "partial" interfaces, right? Are there plans to implement partial interfaces?
What about first warning?

Thanks BastiL
bastil is offline   Reply With Quote

Old   March 12, 2009, 12:23
Default If you have uncovered faces, y
  #19
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,762
Rep Power: 21
hjasak will become famous soon enough
If you have uncovered faces, you need to use bridging, otherwise their values are undefined. Regarding the other warning, it is to do with the accuracy of your geometry - 1e-15 does not sound too bad. Martin and I will probably re-tune the tolerances once we get enough experience with the real cases.

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

Old   March 12, 2009, 12:37
Default Thanks Hrv for this explanatio
  #20
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Thanks Hrv for this explanation,

so I only use brigding if I get this warning? Or always? I don't really understand what bridging is intended for?
The GGIs with "uncovered faces" are definitely partial once. Will this work with bridging turned on? Thanks once more.

Regards BastiL
bastil 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
Partioning of Mesh having nonconformal interfaces Saji FLUENT 0 July 15, 2006 04:58
Grid interfaces in Fluent Omar Qazi FLUENT 1 January 28, 2006 19:55
Fluent - discontinuous grid interfaces Simon Archen FLUENT 2 November 16, 2001 10:52
Sliding mesh interfaces Karl Kevala FLUENT 1 February 20, 2001 05:31
Periodic grid-interfaces in FLUENT 5 tom Main CFD Forum 8 May 13, 1999 20:27


All times are GMT -4. The time now is 13:14.