|
[Sponsors] |
May 8, 2012, 08:23 |
|
#81 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Hello Everyone,
Have been stuck with AMI implementation for some time now and require some help guys. Review of Problem: trying to solve rotating square in regular fluid domain. Case file here: http://db.tt/59ubLm1j Error: See after few iteration the delta T becomes irrelevant ( controlDict) and solver selects depending on courent number i suppose do not know why? Note 1: "NAN" is last value that solver gets and stops. GAMG: Solving for p, Initial residual = nan, Final residual = nan, No Iterations 50 time step continuity errors : sum local = nan, global = nan, cumulative = -nan PIMPLE: iteration 2 smoothSolver: Solving for Ux, Initial residual = nan, Final residual = nan, No Iterations 1000 smoothSolver: Solving for Uz, Initial residual = nan, Final residual = nan, No Iterations 1000 --> FOAM FATAL IO ERROR: wrong token type - expected Scalar, found on line 3 the word 'nan' file: /home/chandra/OpenFOAM/chandra-2.1.x/run/roCube/system/data::solverPerformance::U at line 3. From function operator>>(Istream&, Scalar&) in file lnInclude/Scalar.C at line 91. FOAM exiting Note 2: If you see the AMI line i.e this line . We see 0 source face and 0 target faces. Is it right or wrong ? Really no idea. I thought some faces should be there to transfer values. .AMI: Creating addressing and weights between 0 source faces and 0 target faces Any idea people, ????? Commands i executed. 1.blockMeah 2 snappyHexMesh 3 mergeMeshes rotor/ stator/ (above 2 steps were repeated separately for rotar and stator.) 4 topoSets 5 ChangeDirectory 6 pimpleDyFoam
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better Last edited by kid; May 8, 2012 at 09:28. Reason: few more questios |
|
May 8, 2012, 23:16 |
|
#82 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
Look in your boundary file
Code:
AMI1_patch0 { type cyclicAMI; nFaces 0; startFace 23605; matchTolerance 0.0001; neighbourPatch AMI2_patch0; transform noOrdering; } AMI2_patch0 { type cyclicAMI; nFaces 0; startFace 23605; matchTolerance 0.0001; neighbourPatch AMI1_patch0; transform noOrdering; } also your changeDictionary Code:
dictionaryReplacement { boundary { AMI1_patch0 { type cyclicAMI; nFaces 0; startFace 24985; neighbourPatch AMI2_patch0; transform noOrdering; surface { } } AMI2_patch0 { type cyclicAMI; nFaces 0; startFace 24985; neighbourPatch AMI1_patch0; transform noOrdering; surface { } } } }
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 9, 2012, 02:00 |
|
#83 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Hi linnemann,
Thank you for reply. Same case after modification you suggested is here: http://dl.dropbox.com/u/70019943/roCube2.tar.gz Yes you are right i do not need changeDict file (silly on my part even after understanding i tried to use it as it made Solver to run ). Now when i change manually : splitMeshRegions -makeCellZones -overwrite This gives error as under. Now the good part is this "weights between 1380 source faces and 1504 target". Is there something i am terribly missing???? HTML Code:
Reading volScalarField cellToRegion
Reading volScalarField p
AMI: Creating addressing and weights between 1380 source faces and 1504 target faces
--> FOAM FATAL ERROR:
Unable to set source and target faces
From function void Foam::cyclicAMIPolyPatch::setNextFaces(label&, label&, const primitivePatch&, const primitivePatch&, const boolList&, labelList&, const DynamicList<label>&) const
in file lnInclude/AMIInterpolation.C at line 878.
FOAM aborting
#0 Foam::error::printStack(Foam::Ostream&) in "/home/chandra/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better |
|
May 9, 2012, 03:53 |
|
#84 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
If you had spent just 2min on viewing the case in paraview and enabling the two AMIs like in the screenshot you will see why you have an error.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 9, 2012, 04:04 |
|
#85 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Sir ,
Is it because of tooth edges on AMI1_patch0. Really sorry if this question is too trivial.
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better Last edited by kid; May 9, 2012 at 04:09. Reason: spell |
|
May 9, 2012, 04:38 |
|
#86 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
also that, but also because one of the sides of the AMI contains the top and bottom faces.
The ami should be 1:1 geometry wise, not mesh, but the extend and size must be the same.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 9, 2012, 04:46 |
|
#87 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Sir,
" because one of the sides of the AMI contains the top and bottom faces" This is not clearly understood by me. Could you elaborate? Also geometry should be 1:1 . What this means ?
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better |
|
May 9, 2012, 05:00 |
|
#88 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
The regions on each side of the AMI Connections are not allowed to be of different sizes and have non-overlap regions.
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 9, 2012, 05:15 |
|
#89 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Well AMI1_patch0 is a cylindrical mesh with square. ( this will have upper and lower faces)
And AMI2_patch0 is the other one that is a hollow cylinder with no top and bottom surface. If not his way what should be the logic to implement both AMI Sir? Or any other pointer? Or If we forget all doubts above . What should be the expected look in paraview on selecting both AMI patchs?
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better |
|
May 9, 2012, 08:05 |
|
#90 |
Senior Member
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17 |
Hi Foamers,
have you tried AMI rotating things using unstructured tetrahedral mesh? In my case I have to use it due to the complexity of my geometry, but I have convergence problems (blowing up pressure fields). Best, A |
|
May 9, 2012, 08:50 |
|
#91 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Hello Attesz,
What tool you used for generating unstructured Mesh? Any OpenSource tool??
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better |
|
May 9, 2012, 08:51 |
|
#92 | |
Senior Member
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17 |
Quote:
Hi, no, i'm using ICEM CFD. |
||
May 9, 2012, 23:02 |
|
#93 |
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 556
Rep Power: 27 |
In your case both the AMI's have to be a hollow cylinder with no top and bottom
__________________
Linnemann PS. I do not do personal support, so please post in the forums. |
|
May 12, 2012, 01:57 |
|
#94 |
Member
Jason Eason
Join Date: Jan 2010
Location: Portage, Michigan
Posts: 45
Rep Power: 16 |
Linneman, what would you suggest to do with the top and bottom? Inlets and outlets or would you change the nfaces to 0? Or would you suggest something else?
__________________
Debian Squeeze - OpenFOAM-2.1.x, Paraview-3.12.0 |
|
May 23, 2012, 15:57 |
Bugreport, please contribute
|
#95 | |
Senior Member
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17 |
Dear all,
I've just created a bugreport on OpenFOAM Mantis (http://www.openfoam.org/bugs/) issue 0000539 in this topic (AMI weight goes down to 0). Please contribute with your observations to solve this bug asap. Best regards, Attesz Quote:
|
||
May 24, 2012, 01:36 |
|
#96 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Hi Attesz,
Its good that you have reported this issue. Also in my case it is lack of my understanding of AMI that is creating problem, i suppose.
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better |
|
May 24, 2012, 03:19 |
|
#97 |
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 314
Rep Power: 18 |
Hi Attesz,
Now for me it works but only when I generate the grid with ICEMCFD Hexa. When I generate the mesh with snappyHexMesh (like propeller tutorial) it crashes. Same error as you. Strange because residuals and convergence history is smooth until the crash. I hope that the AMI robustness will be improved. Regards, Stephane |
|
May 24, 2012, 07:01 |
|
#98 |
New Member
Alexander Tagirov
Join Date: Feb 2011
Location: Moscow, Russia
Posts: 7
Rep Power: 15 |
Hi Attesz,
I've had a lot of trouble with the same issue you posted. You see, when AMI gets zero weights, that means that during the interpolation to one of the faces on one AMI patch it couldn't find any faces on second AMI patch that has a projection to this face. The reason for this could be a bug in search/interpolation algorithm, or not a very good mesh. The AMI patches should be as much identical as possible (I mean the mesh, because geometry should be totally the same) , especially if they are cylindrical. |
|
May 24, 2012, 07:08 |
|
#99 |
Senior Member
cfdkid
Join Date: Mar 2009
Posts: 133
Rep Power: 17 |
Hi All,
SUccess after almost 2 months in using AMI. Though i used "SALOME" mesh imported in OpenFOAM-21x. Also results are not good!! But the weights are getting transfered though. Something like this. AMI: Patch source weights min/max/average = 0.965339, 1.1551, 1.00005 AMI: Patch target weights min/max/average = 0.996065, 1.02292, 1.00278 Next step would be improving mesh again. Thanks everyone specially "linnemann" stephane and lovecraft. And you also guys.
__________________
________________________________________ Regards, CFDkid It never gets easier You just get Better Last edited by kid; May 24, 2012 at 07:32. |
|
May 24, 2012, 08:52 |
|
#100 | |
Senior Member
Attesz
Join Date: Mar 2009
Location: Munich
Posts: 368
Rep Power: 17 |
Ok but how did you manage to make it work?
Quote:
|
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
UDF compiling problem | Wouter | Fluent UDF and Scheme Programming | 6 | June 6, 2012 05:43 |
Gambit - meshing over airfoil wrapping (?) problem | JFDC | FLUENT | 1 | July 11, 2011 06:59 |
natural convection problem for a CHT problem | Se-Hee | CFX | 2 | June 10, 2007 07:29 |
Adiabatic and Rotating wall (Convection problem) | ParodDav | CFX | 5 | April 29, 2007 20:13 |
Is this problem well posed? | Thomas P. Abraham | Main CFD Forum | 5 | September 8, 1999 15:52 |