
[Sponsors] 
Approximate Deconvolution model for wall bounded flows channeloodles 

LinkBack  Thread Tools  Display Modes 
September 19, 2006, 04:00 
Hi all,
I am currently tryi

#1 
New Member
Johann Turnow
Join Date: Mar 2009
Posts: 12
Rep Power: 8 
Hi all,
I am currently trying to implement a Model called "Approximate deconvolution model (ADM)" for wall bounded flows. The ADM model for large eddy simulations has been proposed by S. Stolz and N.Adams. The main ingredient is an approximation of the nonfiltered Field by truncated series expansion of the inverse Filter operator. Therefore the momentum equation in the channeloodles solver becomes explicit. After running the code for 10  15 timesteps (deltaT = 0.5e03) the simulation becomes instable and i get pressure peaks in the corners of the discretized channel. Here is modified channelOodles solver // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; for(runTime++; !runTime.end(); runTime++) { Info<< "Time = " << runTime.timeName() << nl << endl; # include "CourantNo.H" # include "readPISOControls.H" //sgsModel>correct(); autoPtr<lesfilter> gridFilterPtr_ ( LESfilter::New(U.mesh(),sgsModel>LESmodelProperties()) ); LESfilter& gridFilter_(gridFilterPtr_()); dimensionedScalar Xsi ( "Xsi", dimensionSet(0, 0, 1, 0, 0), 1.0 ); //the deconvolved field Ustar = 3.0*(U)  3.0*(gridFilter_(U)) + gridFilter_(gridFilter_(U)); fvVectorMatrix UEqn ( fvm::ddt(U) + fvc::div(gridFilter_(Ustar * Ustar)(), "div(phi,U)")  fvc::div(nu*dev(symm(fvc::grad(U))), "div(diss,U)")  Xsi*(gridFilter_(Ustar)  U) == flowDirection*gradP ); if (momentumPredictor) { solve(UEqn == fvc::grad(p)); } # include "continuityErrs.H" //  PISO volScalarField rUA = 1.0/UEqn.A(); for (int corr=0; corr<nCorr; corr++) { U = rUA*UEqn.H(); phi = (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rUA, U, phi); for (int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix pEqn ( fvm::laplacian(rUA,p) == fvc::div(phi) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); if (nonOrth == nNonOrthCorr) { phi = pEqn.flux(); } } # include "continuityErrs.H" U = rUA*fvc::grad(p); U.correctBoundaryConditions(); } Please don't look at the programstyle, I am still working on it. Thanks for your help. J. Turnow 

September 19, 2006, 10:06 
Have you tried adding some imp

#2 
Member
E. David Huckaby
Join Date: Mar 2009
Posts: 57
Rep Power: 8 
Have you tried adding some implicitness to the momentum equation ? i.e. "fvm" instead of "fvc" for the viscous term and replacing the relaxation term:
 Xsi*(gridFilter_(Ustar)  U) with Xsi*gridFilter_(Ustar) + fvm::Sp(Xsi,U) 

September 19, 2006, 10:55 
Hi
for the visous term
"gr

#3 
New Member
Johann Turnow
Join Date: Mar 2009
Posts: 12
Rep Power: 8 
Hi
for the visous term "grad(U)" is not possible for fvm:: ? Maybe you have an idea to avoid using fvm::grad(U)? Furthermore I corrected the convective term in the momentum equation to + fvc::div(fvc::interpolate(gridFilter_(Ustar * Ustar)) & mesh.Sf()) I also tried a new explicit pressure correction, but I got still pressure peaks at the corners of the channel. volVectorField flux = fvc::div(fvc::interpolate(gridFilter_(Ustar * Ustar)) & mesh.Sf()); for (int corr=0; corr<nCorr; corr++) { fvScalarMatrix pEqn ( fvm::laplacian(p) == fvc::div(flux + Xsi*(U  gridFilter_(Ustar))) ); pEqn.setReference(pRefCell, pRefValue); pEqn.solve(); } Thanks for all your help. J. Turnow 

September 19, 2006, 12:09 
Are you using a plane channel

#4 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
Are you using a plane channel test case? If so, try changing the side boundaries to walls.
What happens if you make your timestep 10 times smaller? I can't see anything obviously wrong, although I must admit I don't know the method. 

September 19, 2006, 13:41 
You are quite right about fvm:

#5 
Member
E. David Huckaby
Join Date: Mar 2009
Posts: 57
Rep Power: 8 
You are quite right about fvm::grad.
I meant something along lines of the following: fvm::laplacian(nu,U) + fvc::div(nu*dev(fvc::grad(U)) ) which is similar to the code for the divR() function in "turbulenceModels/incompressible/laminar/laminar.C" Dave 

September 20, 2006, 03:07 
thanks eugene and dave,
Yes

#6 
New Member
Johann Turnow
Join Date: Mar 2009
Posts: 12
Rep Power: 8 
thanks eugene and dave,
Yes I am using the plane channel test case. I changed the side boundary's to walls. But nothing happend. Again my pressure values blow up to 300 in the first 2 timesteps. By reducing the time step to 0.5e04 it is the same game. Also using the implicitness for the viscous term " fvm::laplacian(nu, U)  fvc::div(nu*dev(fvc::grad(U)().T()))" the simulations is getting instable. I am wondering also about the term pEqn.setReference(pRefCell, pRefValue); When using the term my pressure is blowing up to 300, but by neglecting the reference term the pressure rises up to 3.47146e+13. Another point is the velocity field. Here it is not effected by the high pressure values. In addition I compared the convective terms from the ADM solver and the original channelOodles solver. The values are in the same range. If you have access the Journal "Physics of Fluids" and you would like to read more about the ADM model, there's a good articel: "An approximate deconvolution model for largeeddy simulation with application to incompressibe wall bounded flows" ( Volume 13, Number 4, April 2001// page 9971015) 

September 20, 2006, 05:49 
Hmm, I seem to recall there wa

#7 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
Hmm, I seem to recall there was an issue with the reference cell being located adjacent to a cyclic boundary. Try moving the reference cell to somewhere in the middle of the domain.
On the other hand, the fact that it happens at all the corners seems to indicate that the origin of the issue is elsewhere. If the above doesn't work, you will have to start stripping stuff out until you are left with the minimum system that reproduces the problem. The first step would be to rewrite the standard channelOodles explicitly to see if you get the same issue. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Mesh in wall bounded flow  krishh  FLUENT  1  December 3, 2007 02:09 
approximate factorisation  sebed  Main CFD Forum  0  October 19, 2005 18:18 
Law of the Wall in FreeSurface Flows  V. G. Ferreira  Main CFD Forum  5  December 15, 2000 05:47 
BB model for Wall Bounded Shear Flows  Jian Xia  Main CFD Forum  0  November 15, 2000 02:11 
CFD2000 and wall function for turbulent flows.  jens  Main CFD Forum  0  April 12, 1999 08:09 