|
[Sponsors] |
June 25, 2007, 06:10 |
I have implemented (with the h
|
#1 |
New Member
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
I have implemented (with the help of you all) rotating wall boundary conditions and single reference frame for simpleFoam. Now i want to implement Multiple Reference Frame (rotor / stator). I don't need topological change, just one mesh is rotating and the other is static.
Thanks for your hints. Bests Gabriel |
|
June 25, 2007, 06:50 |
Hello Gabriel,
it's already i
|
#2 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
Hello Gabriel,
it's already implemented in OF 1.4. See OpenFOAM-1.4/tutorials/MRFSimpleFoam Regards, A.
__________________
Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
June 26, 2007, 08:47 |
Sorry, thanks. I just looked i
|
#3 |
New Member
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
Sorry, thanks. I just looked in FoamX.
Regards, Gabriel |
|
February 7, 2008, 07:06 |
Hi, everyone!
I've tried to r
|
#4 |
Member
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 17 |
Hi, everyone!
I've tried to run tutorial-case MixerVessel2D (MRFSimpleFoam), but I've got an Error message --> FOAM FATAL ERROR : cannot find MRF faceZone rotor From function Foam::MRFZone::MRFZone(const fvMesh& , const dictionary&) in file cfdTools/general/MRF/MRFZone.C at line 71. FOAM exiting thanks, Paul. |
|
February 7, 2008, 09:22 |
Hi,
I think you have to exe
|
#5 |
Member
Jason Dale
Join Date: Mar 2009
Location: UK
Posts: 80
Rep Power: 17 |
Hi,
I think you have to execute the mixerVessel2D\makeMesh script first. This builds the mesh and sets up the case before you can run it. Regards Jason |
|
February 12, 2008, 06:31 |
Hallo,
the question may be qu
|
#6 |
Member
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 17 |
Hallo,
the question may be quite stupid, but how can I execute makeMesh-script? I've tried allready simple double-click, but that does not lead to any positive results - MRF face Zone were not found... |
|
February 12, 2008, 06:42 |
I'M sorry,
I ran setsToZones
|
#7 |
Member
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 17 |
I'M sorry,
I ran setsToZones .. mixerVessel2D -noFlipMap manually, and error message disapeared. But instead of that following mistake comes: Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0404075, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0403676, No Iterations 2 #0 Foam::error::printStack(Foam:stream&) in "/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: [0x110420] #3 Foam::MRFZone::relativeFlux(Foam::GeometricField<d ouble,>&) const in "/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so" #4 Foam::MRFZones::relativeFlux(Foam::GeometricField< double,>&) const in "/home/plmauk/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libfiniteVolume.so" #5 main in "/home/plmauk/OpenFOAM/plmauk-1.4.1/applications/bin/linuxGccDPOpt/MRFSimpleFoam " #6 __libc_start_main in "/lib/libc.so.6" #7 Foam::regIOobject::readIfModified() in "/home/plmauk/OpenFOAM/plmauk-1.4.1/applications/bin/linuxGccDPOpt/MRFSimpleFoam " Speicherzugriffsfehler Have anybody an idea, what does it mean? |
|
February 12, 2008, 06:52 |
Hi
Go to the mixerVessel2D
|
#8 |
Member
Jason Dale
Join Date: Mar 2009
Location: UK
Posts: 80
Rep Power: 17 |
Hi
Go to the mixerVessel2D directory and type ./makeMesh it should then run through blockMesh etc automatically. Then go up one directory and type MRFSimpleFoam . mixerVessel2D and it should work Jason |
|
February 12, 2008, 07:05 |
Thank you very much, Jason,
i
|
#9 |
Member
Paul Mauk
Join Date: Mar 2009
Posts: 39
Rep Power: 17 |
Thank you very much, Jason,
it works actually! best regards, Paul. |
|
February 12, 2008, 07:23 |
Great,
One other thing, I d
|
#10 |
Member
Jason Dale
Join Date: Mar 2009
Location: UK
Posts: 80
Rep Power: 17 |
Great,
One other thing, I dont think you need the dynamicMeshDict file in the constant directory (left there by mistake?), you only need the MRFZones file which states the zone which is rotating, an origin point, the axis (at the origin point) which the rotation occurs around and the omega (i think its in rpm but Im not sure). And I think its based on an incompressible solver so you need to multiply the calculated pressure by the density to get the real pressure in Pa. Jason |
|
October 27, 2008, 13:07 |
Hello everyone,
I want to s
|
#11 |
Member
Sebastian Vogl
Join Date: Mar 2009
Location: Munich, Germany
Posts: 62
Rep Power: 17 |
Hello everyone,
I want to simulate the aerodynamics of a car using MRFsimpleFoam. The car computer model is imported as .stl file. It was meshed with snappyHexMesh in OpenFoam 1.5 (that's why it must be an .stl file). The reason why I post my problem here, is that I want to take into consideration the movement of the wheels of the car, as they have a great influence on the aerodynamics of the car. This can be generally done by using a multiple reference frame (MRF) boundary condition. For this reason I need MRFsimpleFoam. My question is, how can I define the wheels of my .stl-car as patches which can be written in the MRFZones input file? Is there a possibility to get the names of the mesh elements which form the wheels and put them together to patches? For your ideas I would be very grateful, Yours Sebastian Vogl |
|
October 29, 2008, 05:46 |
Dear Sebastian,
Seems a bit
|
#12 |
Senior Member
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 17 |
Dear Sebastian,
Seems a bit strange - surely all you need for the wheels is a moving wall, not a separate reference frame? Gavin |
|
October 29, 2008, 13:05 |
Dear Gavin,
thank you very
|
#13 |
Member
Sebastian Vogl
Join Date: Mar 2009
Location: Munich, Germany
Posts: 62
Rep Power: 17 |
Dear Gavin,
thank you very much for your reply. Meanwhile I could solve this problem on my own. Yours, Sebastian |
|
December 5, 2008, 08:27 |
Continuing this nicely named t
|
#14 |
Member
Niklas Wikstrom
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
Continuing this nicely named thread with another topic:
The MRF class reside in the "general" section of cfdTools. However, it seems to me that it must be modified for compressible or possibly multiphase codes. I mean, the relative flux in MRFZone.C is calculated as the volume swept by a face, whereas in the compressible case (rho!=1) where phi is massflux the relative flux should contain rho, right? So, I have overloaded the MRFZone::relativeFlux function to allow const volScalarField& rho in the arguments and calculate phi as phi[facei] -= rhof[facei] * ((Omega ^ (Cf[facei] - origin))) & Sf[facei]; However, the solver bails out (p-solver) after a number of iterations. (Hence this post.) Am I wrong in my assumptions about compressible MRFZones? cheers Niklas |
|
December 5, 2008, 10:30 |
Seems to work if the density i
|
#15 |
Member
Niklas Wikstrom
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
Seems to work if the density is considered in the application code instead for in the MRF. Using the volumetric relative flux from MRFZone I added density in pEqn.H of rhoSimpleFoam as follows:
{ surfaceScalarField phiv = fvc::interpolate(U) & mesh.Sf(); surfaceScalarField rhof = fvc::interpolate(rho); mrfZones.relativeFlux(phiv); phi = phiv*rhof; } No problems with that during test, so far. Niklas |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Multiple reference frame | Lim | FLUENT | 1 | April 19, 2008 11:46 |
Multiple reference frame in centrifugal fan | Peter | Main CFD Forum | 0 | April 8, 2008 06:37 |
Multiple reference frame | H.A.S | FLUENT | 0 | April 18, 2007 12:13 |
Multiple reference frame Boundaries | H.A.S | FLUENT | 0 | April 3, 2007 13:45 |
Multiple reference frame | H.A.S | FLUENT | 2 | April 3, 2007 05:32 |