|
[Sponsors] |
attachDetach Topology Modifier: Proper Turbulent Boundary Conditions |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 2, 2012, 20:13 |
attachDetach Topology Modifier: Proper Turbulent Boundary Conditions
|
#1 |
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 740
Rep Power: 28 |
Hello Foamers!
I've been playing around with the attachDetach topology modifier and have been itching to get it working with turbulence. I've got two cases that I've tried with laminar flow, both of which work well (in the sense that they don't crash) which I've uploaded with this thread. They are based on the TJunction case for pimpleFoam, with the extra feature of a "valve" that closes off flow into one of the branches. I would be more than happy to make this a wiki page once I get it working to help other users. This is for OF21x, but the procedure is the same for anything since 16ext as well To run both cases (TJunctionClosedFirst and TJunctionOpenFirst) under 21x, you'll need to unpack attachDetachFvMesh.tar.gz to $FOAM_SRC/topoChangerFvMesh and add Code:
attachDetachFvMesh/attachDetachFvMesh.C Both cases use pimpleDyMFoam, and have a Allrun script that creates the meshes and run the simulations. TJunctionClosedFirst has to merge two meshes (unless there is an easier way of creating walls for the valve), so after the simulation has run there will be a new directory TJunction which contains the actual data. Run both cases as-is to see the laminar behaviour, which proves the topology modifier works as it should. To run turbulent, change the appropriate line in constant/RASProperties (for TJunctionClosedFirst, you'll need to change it in TJunction1/constant/RASProperties). The error occurs somewhere in the turbulence->correct() call after the faces go from being internal to boundary patches. This seems to be related to values of k or epsilon being zero somewhere: Code:
Courant Number mean: 0.220134 max: 0.499147 deltaT = 0.000298507 Time = 2 bool attachDetach::changeTopology() const for object valve : Triggering attach/detach topology change. Current time: 2 current trigger time: 2 trigger index: 0 Modifier 0 named valve morphing void attachDetach::detachInterface(polyTopoChange& ref) const for object valve : Detaching interface void attachDetach::detachInterface(polyTopoChange& ref) const for object valve : Finished detaching interface DILUPBiCG: Solving for Ux, Initial residual = 0.00368108, Final residual = 1.66437e-06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.00279846, Final residual = 1.53383e-06, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.00188171, Final residual = 4.48494e-07, No Iterations 2 GAMG: Solving for p, Initial residual = 0.520347, Final residual = 0.214301, No Iterations 1000 time step continuity errors : sum local = 0.00113155, global = -1.20446e-05, cumulative = -1.37368e-05 GAMG: Solving for p, Initial residual = 0.135724, Final residual = 0.0419013, No Iterations 1000 time step continuity errors : sum local = 0.000493047, global = -2.032e-05, cumulative = -3.40569e-05 #0 Foam::error::printStack(Foam::Ostream&) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #5 Foam::incompressible::RASModels::RNGkEpsilon::correct() in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #6 in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" #7 __libc_start_main in "/lib/libc.so.6" #8 at /usr/src/packages/BUILD/glibc-2.11.3/csu/../sysdeps/i386/elf/start.S:122 Code:
Courant Number mean: 0.22037 max: 0.498308 deltaT = 0.000299285 Time = 2 bool attachDetach::changeTopology() const for object valve : Triggering attach/detach topology change. Current time: 2 current trigger time: 2 trigger index: 0 Modifier 0 named valve morphing void attachDetach::detachInterface(polyTopoChange& ref) const for object valve : Detaching interface void attachDetach::detachInterface(polyTopoChange& ref) const for object valve : Finished detaching interface DILUPBiCG: Solving for Ux, Initial residual = 0.0038858, Final residual = 1.30384e-06, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.00278652, Final residual = 1.56476e-06, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.00193932, Final residual = 4.80674e-07, No Iterations 2 GAMG: Solving for p, Initial residual = 0.52962, Final residual = 0.243818, No Iterations 1000 time step continuity errors : sum local = 0.00127258, global = 8.9244e-07, cumulative = 8.88314e-07 GAMG: Solving for p, Initial residual = 0.126708, Final residual = 0.0158993, No Iterations 1000 time step continuity errors : sum local = 0.000205975, global = -1.05775e-05, cumulative = -9.6892e-06 bounding k, min: -1.5986e-51 max: 1.44949 average: 0.190389 bounding epsilon, min: -1.59926e-51 max: 152.799 average: 15.3409 correct RASModel Create new G field Update G at wall Dissipation equation DILUPBiCG: Solving for epsilon, Initial residual = 0.00342873, Final residual = 7.04553e-06, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.00850805, Final residual = 7.2587e-08, No Iterations 2 #0 Foam::error::printStack(Foam::Ostream&) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::incompressible::RASModels::nutkWallFunctionFvPatchScalarField::calcNut() const in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #4 Foam::incompressible::RASModels::nutkWallFunctionFvPatchScalarField::updateCoeffs() in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #5 Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" #6 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" #7 Foam::incompressible::RASModels::kEpsilon::correct() in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/lib/libincompressibleRASModels.so" #8 in "/home/mturcios/OpenFOAM/OpenFOAM-2.1.x/platforms/linuxGccDPOpt/bin/pimpleDyMFoam" #9 __libc_start_main in "/lib/libc.so.6" #10 at /usr/src/packages/BUILD/glibc-2.11.3/csu/../sysdeps/i386/elf/start.S:122 Floating point exception Hopefully this is something small that can be dealt with through boundary conditions. Note that I've tried this case in 1.6ext and get similar errors, which again lead me to believe that its a boundary condition problem. Thanks! Last edited by mturcios777; May 3, 2012 at 14:26. Reason: Change in second error message |
|
May 7, 2012, 20:27 |
|
#2 |
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 740
Rep Power: 28 |
Some good news everyone! I found the reason behind the crash. With the change in topology, the viscosity boundary conditions are incorrectly applied/interpolated because I was using a Newtonian viscosity model. One solution is to add the following to the correct() function in $FOAM_SRC/transportModels/incompressible/viscosityModels/Newtonian/Newtonian.H
Code:
nu_ = nu0_; I'm now working on compressible flow (altering rhoPimpleFoam -> rhoPimpleDyMFoam). Thus far it crashes when solving the pressure equation, because of the density field not being remade properly. I think it has to do with updating the BC's with the topology change. If anyone has more experience with the thermo models implementation, it would be greatly appreciated. Last edited by mturcios777; May 8, 2012 at 19:02. Reason: typo |
|
September 12, 2012, 15:18 |
|
#3 |
Senior Member
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 740
Rep Power: 28 |
Wow, 5 months is a long time. I've been working on other projects while taking the occasional eye to getting this to work. I've asked the developers and came to the knowledge that faces created by inflation are swept into position and thus have a mesh flux associated with them. Or at least they should be: I found that the following code needs to be added to the attachDetachFvMesh::update function
[CODE] pointField newPoints = points(); movePoints(newPoints); [CODE] This ensures that the attachDetach faces have the zero mesh flux that is required. I'm not sure why the default values for meshPhi are crazy, but adding this code makes things work. I'm doing some testing to see if the same will work for layer addition and removal, which I've also been working on off and on. |
|
September 13, 2012, 04:24 |
|
#4 |
Senior Member
Join Date: Oct 2009
Posts: 140
Rep Power: 17 |
Hi! I had similar problems with the attach/detach boundaries while using turbulence models.
I am happy that you fixed the problem. Here is the link, how I got rid of this problem. http://www.cfd-online.com/Forums/ope...changes-3.html Do you have experiences with attach/detach boundaries in parallel ? I guess you are also interested in engine simulations. Here is my problem http://www.cfd-online.com/Forums/ope...-parallel.html Peter |
|
September 13, 2012, 04:56 |
|
#5 |
Senior Member
Join Date: Oct 2009
Posts: 140
Rep Power: 17 |
Hi! I had similar problems with the attach/detach boundaries while using turbulence models.
I am happy that you fixed the problem. Here is the link, how I got rid of this problem. http://www.cfd-online.com/Forums/ope...changes-3.html Do you have experiences with attach/detach boundaries in parallel ? I guess you are also interested in engine simulations. Here is my problem http://www.cfd-online.com/Forums/ope...-parallel.html Peter |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Integral boundary conditions turbulent intensitylength boundary conditions | olesen | OpenFOAM Running, Solving & CFD | 0 | July 27, 2006 07:18 |
Turbulent boundary conditions for bubble column | anjai | FLUENT | 12 | October 17, 2005 06:34 |
New topic on same subject - Flow around race car | Tudor Miron | CFX | 15 | April 2, 2004 06:18 |
Please help with flow around car modelling! | Tudor Miron | CFX | 17 | March 19, 2004 19:23 |
Turbulent Mass Injection Boundary Conditions | B. Laubacher | Main CFD Forum | 6 | October 16, 1999 11:56 |