Hello,

I'm developing a multigrid (FAS, on the outer iterations) finite-volume incompressible Navier-Stokes code (using SIMPLE) with k-epsilon turbulence modeling. The single grid version of the code and the multigrid version with no turbulence modeling have been validated, with the convergence rate expected from a multigrid method in the last case. When adapting the multigrid scheme to the turbulence equations I have a problem and a question:

(1) When using a wall-law model for the near-wall nodes, the convergence stops and the residuals oscillate around a value two orders of magnitude smaller than the initial residual. The use of the wall-law in the coarser grids, especially in the epsilon equation, causes a residual "freeze". When I do not apply the wall-law in the coarser grids, or rather, set the multigrid correction to zero in the coarse grid which contains the fine wall-law grids, the convergence seems to be reasonable at first, but ceases to decay at a value four orders of magnitude smaller than the initial residual. The code without turbulence modeling achieves a residual decay to machine precision. I am using a wall-law model which modifies the variables in the control volumes adjacent to the wall (as described in "Computational Methods in Fluid Mechanics", Peric & Ferziger), in contrast to methods which do not grid or represent the region next to the wall, as normally done in finite element codes. This has the negative effect that the wall-law matching to the simulated field is always carried out at a different point at every mesh, farther away from the wall in coarse meshes and closer in finer meshes in the multigrid cycle. I have found a large number of papers which describe the successful simulation of turbulent flows using multigrid methods with wall-laws, but have failed to gain any insight to solving my problem. Is it necessary to apply multigrid only outside of the region where the wall-law is used as a boundary condition?

(2) When using a low Reynolds model, what is the limit when coarsening the grid? A very fine grid is necessary to resolve the equations near the wall, won't the coarse grids used in the multigrid hamper the convergence of the method?

I would appreciate any comments or ideas on applying multigrid acceleration to turbulence modeling.

Thank you,

Paulo Zandonade

(1). It is a very complex question, but I will try to simplify it first. (2). It is good that you have validated the code for the laminar flows. I mean the single grid case. (3). The turbulent flow calculation is very different from the laminar flow calculation. This is because the viscosity (eddy viscosity in this case) is not constant throughout the flow field and must be obtained from k-epsilon equations. (4). And there is also a wall layer with sharp gradient, which you are replacing it by the wall-function treatment. (5). At this point, I would say that the first priority is to focus on the solution of the turbulent flow. Try to get a good handle of it in single grid. (6). Once you have a single grid turbulent flow result, you can perform some parametric study of the mesh effect by using different single grids. This will give you the information you need whether the coarse grid is giving you the trouble. (7). If you can pass this single grid turbulent flow calculation, then you can start exploring the multi-grid approach. Since I don't use multi-grid myself, it is difficult to advice you in this area. But I think, if your method is stable under various grid configurations and the method is iterative, then you should have no problem in using any of the grids at any time during iteration. (8). My experience with commercial CFD codes tells me that even if the multi-grid option is there, there is no guarantee that the multi-grid solution will converge. This is because multi-grid is a control issue, and it depends on the problem, the exact procedure used. When the converging problem exists, the simple fix is to disable the multi-grid option first. (9). I am sure that you can do some experiments to include/ or not to include the wall region in the multi-grid process. (10). As for the low Reynolds number model (k-epsilon model), the convergence rate could be a probem if the equations are not solved properly. This also depends on the particular form of the k-epsilon model used. In this case both the form of the model and the numerical procedure have great impact on the convergence of solution. (11). Since this is a complex research area, I don't think people will print everything in the journal. What you read is probably not exactly what they used. (12). If you can obtain turbulent flow solution in single grid, it is already a great accomplishment by itself. (13). Multi-grid approach is great for simple problems, we normally turn it off in real life, unless the method used is very stable for any grid.

John,

Thank you for answering my message. I have also validated the code for some turbulent flows (simple flows only: flat plate and straight 2d duct, I have compared the solution of a backward facing step and the results have been comparable with other classic k-e simulations --> underprediction of the reattachment length.) I am actually following your no. (5) suggestion and using the code without multigrid and the code works as expected (since my thesis is not the application of multigrid but rather the use of explicit algebraic Reynolds tensor models the implementation of multigrid is not a must, but rather a bonus). The code is stable, but some of explicit algebraic models (mostly those developed at UMIST) require the use of a low Reynolds model, hence any acceleration in convergence would be extremely valuable. The models which use wall-laws can be calculated with single grid procedures in a matter of minutes, since the grid can be relatively coarse (if compared with the low Reynolds grids, and with grid independent solutions checked by comparing the final solution with a grid twice as fine). Before using the multigrid method on a turbulent simulation I checked the single grid convergence on each one of the grids. The multigrid method also works with a coupled NS-heat transfer solution when no turbulent model is used. I believe there must be a specific grid transfer procedure to account either for the high gradients of k and epsilon near the wall or the use of wall-law boundary conditions. I tried to find a similar method applied to the flow variables in the case of a shock wave (similar gradient problems) but could not find a method other than bilinear interpolation or inverse-distance interpolation being used in multigrid finite-volume.

Thank you,

Paulo Zandonade

Hi there,

According to what you said and to my (limited) experience with multigrid methods, it really seems that the problem comes from the boundary condition. If there is a non-trivial treatment of the boundaries, then this has somehow to be (say) 'restricted' and 'prolonged' to the coarser and finer grids or it has to appear somehow either in the 'relaxing part' of the multigrid or when computing the 'operator'. I am not quite sure what it the wall-laws so it is difficult to say more.

PG.

From my understanding, the k-e transport equation are source-dominated equations, and contain a few derivative term, which may difficult to obtain stable convergence while solving the k-e equations.

What about trying solving the k-e model on finest grid and using multigrid method to solve the remaining governing equations.

If one try to use the method while solving k-e model, it also interesting to see the value of k and e at coarser grid after restriction and prolongation process, which should always give positive values

AAJ

(1). The issue seems to be the convergence rate problem, so, I think, you need to identify the exact area(location) which is creating the problem. (2). Some commercial codes can track the field variation between iterations. I think, the simplest method to use is to print out the computed variable itself at several different locations as a function of iteration number, especially the slow convergent area. In this way, you will be able to see the whole picture, that is the rate of convergence at each point. In old days, I used to run the calculation untill the printed variable becomes identical after certain number of iterations. In this way, you can define the problem area for your multi-grid approach. If this is a problem for the whole flow field, then you probably have made a mistake somewhere. Otherwise, once you have narrowed down the problem location, it should be easier to find the answer.

Hello,

I am afraid I can't provide much useful comments for the original question. Rather I have another question which I think is related to the the orginal question posted by Paulo Zandonade. I hope I can get some help from this group of people. You seem to be knowledgable on multi-grid for finite volume method.

My question is about general multigrid method for FV method in incompressible flow. I myself is working with a steady imcompressible flow code for steel casting. Since the number of grids is around a million or more, single grid seems to have a very slow convergence. So, I want to use multigrid to accelerate the convergence. I have the experience to use multi-grid on a finite difference equations. Everything seems just straightforward there. However, when comes to the finite volume, things seem to be a lot more complicated. I managed to figure out the multigrid scheme for the pressure poisson equations. It seems to work fine. In my case, 900,000 grid takes 150 iteration to get down to machine accuracy. However, I don't know how to apply multi-grid mehtod for velocity corrections. Mainly, the upwind/hybrid scheme troubles me. Because, from a fine grid to a coarse grid, Peclet number increases by a factor two. So, a center difference may become a upwind. So, I don't know what is the suitable approximate operator for coarser grids. Besides, since u, v, w are located on differenent staggered points, application of multi-grid mehtod is not a staightforward matter for me. I mean, difficult to figure it out by myself.

Therefore, I would like to know some literatures about multi-grid mehtod for FV velocity updating (like SIMPLER). I have looked up some text books, and I have not found any direct answers. I would be very grateful to get some help here.

Best regards, Jin Li

Hello,

It appears you are using the multigrid method only in the internal iterations of the SIMPLE method. However, multigrid is normally used only in the pressure equation when applied to the internal iterations. The reason for this is that the velocity equations do not need to be solved as accurately as the pressure equation. A residual reduction of 1 to 3 orders of magnitude is normally sufficient (per INTERNAL iteration), which can be achieved rapidly by SIP or GS. The use of multigrid in the pressure equation can accelerate the code by as much as 2x (only?). Fortunately the multigrid method can be applied to the external iterations, where order of magnitude accelerations of convergence can be attained. Here the "smoother" of the multigrid method is the SIMPLE method itself. You can find more information at the following websites:

http://www.mgnet.org/

http://www.tfd.chalmers.se/~lada/

http://mecheng1.uwaterloo.ca/~fslien/

or in the following books:

"Computational Methods for Fluid Dynamics"; Joel H. Ferziger & Milovan Peric; Springer-Verlag

"Handbook of Computational Fluid Mechanics"; ed. Roger Peyret; Academic Press

"Computational Techniques for Complex Transport Phenomena"; W. Shyy, S.S. Thakur, H. Ouyang, J.Liu, and E. Blosch; Cambridge University Press

"Multi-grid Methods and Applications"; W. Hackbush; Springer

Hope it helps!

Paulo Zandonade

I don't use multigrid myself. But I want to use it for combustion space modeling in furnaces. One suggestion from a conference that I have joined (Computational Heat and Mass Transfer, Kibris, April 26-29, 1999, Non-staggered grid arrangements to solve incompressible flow problems with SIMPLE algorithms by A.A. Mohamad): The disadvantage of staggered grid arrangement is extensive coding effort in application with multi-grid solver. Multi-grid solving strategy can be easily coded with non-staggared (colocated )grid arrengament.

Further ref: "Computational Methods for Fluid Dynamics"; Joel H. Ferziger & Milovan Peric; Springer-Verlag

Hi Jin Li,

You should only consider the Peclet number (or any other qunatities) only on the fine grid, since you are not solving the same equations on the coarser grids. On the coarser grids you solve for the errors of the equations of the previous finer grid. On the coarser grids you are smoothing out the errors of the previous set of equations. THe coarser the grid, the longer the wavelength of the smoothing. So the shortest wavelength errors are smoothed out on the finest grid and the largest on the coarsest one. The implementation in speed comes from the fact that smoothing out long wavelengths on the fine grid would take too many iterations, therefore it is wise to smooth them out on coarser grids.

P.G.