|
[Sponsors] |
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 24, 2009, 02:45 |
|
#41 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,902
Rep Power: 37 |
Hi Luther
The problem is not related to groovyBC but to /system/fvSolution, as stated in the error message. Try to copy e.g. the /system/fvSolution from /tutorials/interFoam/damBreak and see if it does not solve the problem, as it should be working with interFoam. Best regards, Niels |
|
May 24, 2009, 03:13 |
|
#42 | |
New Member
Luther Terblanche
Join Date: May 2009
Posts: 15
Rep Power: 17 |
Quote:
Yes I have changed the two preconditioners it was complaining about in the fvSolution file to preconditioner DIC. And then it worked. Would have to read up on what it entails. Thank you for the post. Regards Luther |
||
May 26, 2009, 04:53 |
|
#43 |
New Member
Luther Terblanche
Join Date: May 2009
Posts: 15
Rep Power: 17 |
Hallo Bernard (or anyone else that would be able to help),
First of all, thank you for the help. I have managed to get the groovyBC case working for simulating a wave in a 2D flume. I have now been trying to apply it to a 3D case. I have made a mesh in gmsh and converted it using gmshToFoam. With the conversion I got a warning message saying it found a number of undefined faces in the mesh and are adding them to the default patch. However, when I look in the constant/polyMesh/boundary file it generated I find: defaultFaces { type patch; nFaces 0; ..... } Would that mean there is 0 default Faces? If I choose to ignore it and set everything up pretty much the same as in the groovyWaveTank example I find that the simulation crashes near the start. The Courant numbers grow out of control. Here is the massage: MULES: Solving for gamma Liquid phase volume fraction = 0.4197596 Min(gamma) = -1.1716894e-19 Max(gamma) = 1.0015516 MULES: Solving for gamma Liquid phase volume fraction = 0.41975964 Min(gamma) = -4.9807421e-20 Max(gamma) = 1.0000001 MULES: Solving for gamma Liquid phase volume fraction = 0.41975967 Min(gamma) = -1.271157e-19 Max(gamma) = 1.097679 GAMG: Solving for pd, Initial residual = 0.89005896, Final residual = 0.029750488, No Iterations 3 GAMG: Solving for pd, Initial residual = 0.99557433, Final residual = 0.033653032, No Iterations 3 DICPCG: Solving for pd, Initial residual = 0.99572845, Final residual = 9.8705723e-08, No Iterations 324 time step continuity errors : sum local = 0.0010253293, global = -8.0769936e-07, cumulative = -8.0897217e-07 ExecutionTime = 63.5 s ClockTime = 64 s Courant Number mean: 5588.1394 max: 64637244 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0xb8034400] #3 Foam::Time::adjustDeltaT() in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #4 Foam::Time::setDeltaT(double) in "/home/luther/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #5 main in "/home/luther/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interFoam" #6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/luther/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/interFoam" Floating point exception Then when I have a look at the few results generated it seems like the initial gamma field is set everywere except at the inlet face, where the groovyBC is defined. I use setFields and interFoam. Am I doing something wrong? Anybody with some advice I will really appreciate it. I attach the case I am playing around with if you would like to have a look yourself. Here is the case file: http://dip.sun.ac.za/~luther/OF/poles.tar.gz Kind regards Luther |
|
May 26, 2009, 07:24 |
|
#44 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,902
Rep Power: 37 |
Hi Luther
Have you added the libGroovyBC (or what it is called), to the controlDict? If not, then it will not execute the Groovy with setFields, and thus the inlet boundary face will be empty. Look at the wiki on how to add it. Niels |
|
May 26, 2009, 07:59 |
|
#45 | |
New Member
Luther Terblanche
Join Date: May 2009
Posts: 15
Rep Power: 17 |
Quote:
Thank you for your reply. I did remember to add the line " libs("libgroovyBC.so"); " to the bottom of controlDict. Let me know if you think of anything else by any chance. Kind Regards Luther |
||
May 26, 2009, 08:21 |
|
#46 |
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,902
Rep Power: 37 |
Hi Luther
I have looked at your case file, and several things are off, non of which are related to groovyBC, however let us take it in this tread: 1. You are calculating the surface elevation around z=0 which is also the z-value on one of your boundary patches, even though your setFieldsDict suggest that you want to have the waves averaged around z=2.1. 2. I don't think the mesh resolution is anything near sufficient to resolve the physics you are interested in. Especially because you are having rather large tetrahedrals around the free surface. The scale of which are order of magnitude the wave amplitude. 3. You apply deep water theory, however you are in intermediate waters (0.1 < h/L = 0.4 < (pi or 2 * pi)), thus the applied theory is not correct. These are the things I have noticed would cause you trouble, however I am almost certain that it is (1) which cause the blow-up. Best regards, Niels |
|
May 26, 2009, 08:42 |
|
#47 | |
New Member
Luther Terblanche
Join Date: May 2009
Posts: 15
Rep Power: 17 |
Quote:
Thanks. Regarding (1): I will most certainly try it this evening. I have not been looking out for that and it makes sense that it could be the cause. Regarding (2) and (3): I was not giving any attention to the wave theory or the mesh resolution itself at this stage. I was merely trying to see if I can apply the groovyBC from groovyWaveTank to a 3D case. Thank you very much for the effort of looking into it. Hopefully it would not be too long before I can also make useful contributions to the forum. Regards Luther |
||
October 15, 2009, 11:38 |
|
#48 |
Member
Gautami Erukulla
Join Date: Mar 2009
Posts: 71
Rep Power: 17 |
Hello,
I tried to run the groovyBC movingConeDistorted case from the following link: https://openfoam-extend.svn.sourcefo...roovyBC/Demos/ I did not make any changes to the case,and tried to run it as it is on OpenFOAM 1-5,suse linux 10.3. But I end up getting this error. Not Implemented Trying to construct an genericFvPatchField on patch movingWall of field cellMotionUx#0 Foam::error:rintStack(Foam::Ostream&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Foam::genericFvPatchField<double>::genericFvPatchF ield(Foam::fvPatch const&, Foam:imensionedField<double, Foam::volMesh> const&) in "/home/gali/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so" Can someone please help me. Thankyou, Gautami. |
|
October 16, 2009, 05:36 |
|
#49 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
Check the output of the solver further up Bernhard |
||
October 20, 2009, 11:01 |
|
#50 |
Member
Gautami Erukulla
Join Date: Mar 2009
Posts: 71
Rep Power: 17 |
Hello Mr Gschaider,
Thank you. I could run the distortedmovingcone case without any error. The problem was a small mistake at my end.(sorry) Thankyou, Gautami. |
|
October 23, 2009, 05:56 |
|
#51 |
Member
David GISEN
Join Date: Jul 2009
Location: Germany
Posts: 68
Rep Power: 17 |
Hello Foamers,
has somebody dealt with the groovyWaveTank demo? I wonder how the initial condition for gamma on the inlet patch is been set, as my setFields just writes the List<scalar> for the internalField. The result is, that I get a zero initial condition at the inlet. Does somebody know how to do this? Thanks in advance, David |
|
October 27, 2009, 13:35 |
|
#52 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
Hi Bernhard,
I wonder, if your groovyBC is able to connect two boundary conditions!? E.g. is it possible to get the area averaged value of one patch to another one? Would be great, if this works! Fabian |
|
October 28, 2009, 15:11 |
|
#53 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
Bernhard |
||
November 6, 2009, 02:32 |
|
#54 |
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 17 |
Hi, dear friends, I am trying to update the dambreak case of interPhaseChangeFoam for OF-1.5 to OF-1.6, and just meet the same problem like #40.
The alpha1 setting is Code:
alpha1 { MULESImplicit { maxIter 1000; nLimiterIter 10; maxUnboundedness 1; CoCoeff 0.2; solver { solver PBiCG; preconditioner DILU; tolerance 1e-10; relTol 0; } } } Have a good day! chiven ------------------------------------------------------------------------------------------------------------------------ Starting time loop Courant Number mean: 0 max: 0 deltaT = 2.4e-05 Time = 2.4e-05 Attempt to return dictionary entry as a primitive file: /work/g2/e090012/dambreak/system/fvSolution::solver from line 58 to line 60. From function ITstream& primitiveEntry::stream() const in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83. FOAM aborting #0 _ZN4Foam5error10printStackERNS_7OstreamE-0x1466af0 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #1 _ZN4Foam7IOerror5abortEv-0x1989560 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #2 _ZNK4Foam15dictionaryEntry6streamEv-0x1921900 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #3 _ZNK4Foam10dictionary6lookupERKNS_4wordEbb-0x19476e0 in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/lib/linuxIA64GccDPOpt/libOpenFOAM.so" #4 void Foam::MULES::implicitSolve<Foam:neField, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam:neField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, double, double) in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam" #5 main in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam" #6 __libc_start_main-0x1060880 in "/lib/tls/libc.so.6.1" #7 _start in "/home/g2/e090012/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxIA64GccDPOpt/interPhaseChangeFoam" Abort |
|
November 6, 2009, 04:57 |
|
#55 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
I fail to get the significance of this for this thread. Especially if you look at #41 and #42 where a solution strategy for this was discussed
|
|
November 6, 2009, 05:54 |
|
#56 | |
Senior Member
J. Cai
Join Date: Apr 2009
Posts: 180
Rep Power: 17 |
Quote:
I have tried what #41 and #42 said, but faild. These days I am struggling with this problem. And some other friends in this forums also meet the same problems. Any suggestiohs are precious for us. Best regards, Chiven |
||
November 6, 2009, 13:09 |
|
#57 |
Member
Gautami Erukulla
Join Date: Mar 2009
Posts: 71
Rep Power: 17 |
Hello,
I am trying to simulate a wave tank case in interDyMFoam. I have set the inlet as groovyBC. I want to set the expression for the inlet in pointMotionUx dictionary as follows: if (time>1 and time<=2 expression-1) if (time>2 and time<3 expression-2) else zero. I am trying to do it a follows,but I get an error. valueExpression "toPoint((time()>1 && time()<=2) ? A*w*cos(w*time()) (time()>2 && time()<3) ? B*v*cos(w*time()) : 0 )"; How do I input such expression? ThankYou. Regards, Gautami. |
|
November 6, 2009, 13:36 |
|
#58 |
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 19 |
Hi Bernhard,
thanks for the info! Shouldn't be so hard sounds good ... Fabian |
|
November 9, 2009, 03:33 |
|
#59 |
Senior Member
Arne Stahlmann
Join Date: Nov 2009
Location: Hanover, Germany
Posts: 209
Rep Power: 17 |
Hi, did anybody successfully test and use the groovyBC with OpenFOAM 1.6?
From the errors I get, I guess that a few things have to be changed due to differences in calling of constants etc. between 1.5 and 1.6... Arne |
|
November 9, 2009, 04:56 |
|
#60 | |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Quote:
http://openfoamwiki.net/index.php/Co...ovyBC#Download (nevertheless, the 1.6 URL could have been easily guessed from the 1.5-URL) Bernhard |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Ship resistance shows wiggles when using Overset mesh and dynamic mesh in Fluent | Qingsong | FLUENT | 2 | March 21, 2022 15:08 |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 07:38 |
[ICEM] Dynamic mesh setup with ICEM | David121284 | ANSYS Meshing & Geometry | 0 | April 11, 2014 04:19 |
Dynamic Mesh "Shadow Wall" | thezack | FLUENT | 0 | June 4, 2013 22:09 |
dynamic mesh for drop interface | IndrajitW | FLUENT | 0 | March 30, 2013 08:03 |