
[Sponsors] 
October 3, 2005, 11:09 
Scaling of the Adaptive Dissipation for NS Grids

#1 
Guest
Posts: n/a

Hi everybody,
I'm currently developping a finitevolume solver in structured grids for transonic viscous flows. I use the RoeMUSCL scheme (together with the Harten entropy correction) for the mean flow equations, which works well for inviscid flows but does not converge for viscous flows in a case of shockboundary layer interaction. My test case is the classical RAE2822 airfoil, farfield Mach number of 0.73, incidence 2.79 degrees and a Reynolds number of 6.5 millions. I'm trying to rescale the entropy fix parameter for grids with high aspect ratio cells with some functions of cell metric or spectral radii ratio according to the grid directions. But I have been quite unsuccessful so far. Does anyone has some experience about this issue? Thanks in advance. Jessy 

October 4, 2005, 01:52 
Re: Scaling of the Adaptive Dissipation for NS

#2 
Guest
Posts: n/a

Dear Jessy,
The problem of convergence may mostly be related to the grid on which you are making the solution. In case of viscous flows, the residue is seen to oscillate at say 1e4 or 1e5, and not smoothly falling down to say 1e6. However, it must be noted that there is the question of discretisation of the viscous fluxes (VFD), which you have not mentioned in the question. Assuming that you are working with a central differencing for the same and you have a body fitted grid, have you made the necessary transformation when in the computational domain? The VFD is important, it could well be the difference b/w a converged solution and a blown up solution. Also, your inviscid code seems to converge, but the viscous code does not, so it points out to the role of VFD on convergence. If you find that your VFD is proper, then all that can be said is that the residue will oscillate about a mean and set into 'limit' oscillations (if you prefer to call it so) and then we need to call it as the 'converged' solution once such a periodicity in oscillationg residue is seen. You could try also running with lower cfl, though I am not sure to what extent it helps. Also note that your code may converge on a coarser grid but not a finer grid, as possibly you are using here.( This is a turbulent test case, so I presume your y+ ~ 56 , and you have a well to  do turbulence model). Thus inshort, both the grid as well as the VFD are sources which could affect convergence. Limiters are known to spoil convergence and this could also play a major role. And morre so, when you have a finer grid to solve a transonic viscous flow, your observation is by no means a surprise. If you are sure that your procedure is bugfree and you seem to get an oscillating residue plot, you would have to declare convergence after a reasonable amount of oscillations(after some preiodicity). I do not think that tampering the entropy fix could really help in such a case, although of course you can get a converged solution to sufficient accuracy by manipulating the grid to some extent. One of my friends have indeed solved this problem on a Cgrid with around 25000 volumes, with RoeScheme and a Green Gauss based VFD, Venkatakrishnan's limiter and a BaldwinLomax model and got a convergence of upto 1e6 (If I remember right). For more details you can contact him at muni@aero.iisc.ernet.in Hope this helps Regards, Ganesh 

October 4, 2005, 10:12 
Re: Scaling of the Adaptive Dissipation for NS

#3 
Guest
Posts: n/a

Dear Ganesh,
Thanks a lot for your quick and detailed anwswer. You are right, my first post was not complete. Actually, and this confirm the experience of your friend you mentioned at the end of your message, I have no convergence problem on this shock/boundary layer interaction when using the mixing length model of BaldwinLomax. The residuals drop down with six order of magnitude with respect to the initial residual (provided that the CFL number is reduced with respect to the inviscid case). As far as the discretisation of viscous flux is concerned, I use the Gauss theorem for the calculation of gradients. The integration path (IP) you must consider however, is not unique. I have implemented a standard cellcentred IP (averaging the right and left discrete gradients at the interface) as well as a socalled 'diamond' path connecting the left and right cell centroids to the interface (theoretically less sensitive to grid streching) and an hexahedral IP centred on the interface. A correction has been also introduced in the first case (cellcentred IP) for preventing from the evenodd coupling issue, by using the directional derivative along the direction connecting the left and right cellcentroids. Last: I also use the Venkatakrishnan's limiter in the MUSCL extrapolation for the mean flow system. I tried all of these IP for laminar computations but I didn't see any clear differences on both solution accuracy and convergence rate to steady state. My point is then the following (sorry that I forgot to mention it in my first post). Problems arise in my case when dealing with the oneequation SpalartAlmaras model for the eddyviscosity calculation. The discretisation of the SpalartAlmaras equation is performed separately from the RANS equations, and regarding the convective flux, by using the Roe scheme (without MUSCL extrapolation) but still considering the Harten entropy correction for the linear wave approaching zero. I have experienced that introducing a proper scaling function (based on cell aspectratio considerations) for the entropy fix parameter improved significantly the convergence rate in some subsonic or transonic cases (without shock wave). Going back to the RAE2822 airfoil in transonic regime, I tried to lower the CFL number, unsuccessfully, my residuals fall down of about 4 order of magnitude and afterwards, in the worse case, I get a clear divergence of the solution and in the better case, by enforcing some dissipation parameters (the unscaled entropy fix parameter and the Venkatakrishnan's limiter coefficient), let say that I got something like a stable solution with oscillating residuals around 3.5, 4 order of magnitude. I could check the convergence on the history of the drag/thrust coefficients but what I am trying to obrain is a stable calculation. According to the original paper of SpalartAllmaras, there is no need to a very fine grid near the walls for this turbulence model, which can by applied on the same grids as the ones considered for mixing length models, with a first cell size of about 10^5 chord. I found Y+ values less than unity accross and downstream the shock wave in my (unstable) computations. The conclusion may be that this test case is a critical one for CFD computations. This is maybe a consequence of physical instabilities due to the presence of a recirculation area in the boundary layer downstream of the shock wave, which is not properly convected and dampted out by the solver. When using mixing length models, there is no recirculation predicted and this explains why these models give a fast convergence to a steady state. In other words, the less the physic is captured, the more are stable the algorithms. I will let you know about my future investigations regarding this issue. Thanks again Ganesh for advices and suggestions. 

October 4, 2005, 16:14 
Re: Scaling of the Adaptive Dissipation for NS

#4 
Guest
Posts: n/a

>the less the physic is captured, the more are stable the algorithms
I think this is the key, considering that the flow in your case really should be unsteady. There are certainly a lot of numerical issues at play, everything that ganesh mentioned, plus additional problems caused by the turbulence model, and the coupling between model and NS equations. I would agree with ganesh that the primary cause of your problems is probably not with the inviscid fluxes (alone). Nevertheless, I am sure that you can find a numerical procedure to suppress the physical instability (introduce more numerical diffusion using different "entropy fixes") and get some steady solution, but you may not want to even go that way. To see if the turbulence model is acting up, you could also try to freeze the eddy viscosity after some iterations (turning off the SA model after several orders of convergence), and see if you get it to converge or at least stay stable. However, to gain better understanding of this problem you should spend some time to try and prove that this conjecture of yours is actually true: Why don't you solve the unsteady equations and see if you can get convergence? I wouldn't be surprised to see that it works far better than your attempted steady state solution. At least that's my experience in such situations. If that works, you gain some sense of closure to what's causing this instability, and then you can work something out for the steady state. 

October 4, 2005, 23:33 
Re: Scaling of the Adaptive Dissipation for NS

#5 
Guest
Posts: n/a

I have recently solved flow past RAE2822 at M=0.729, alpha=2.31 deg and Re=6.5 million using a vertexcentered finite volume scheme, Roe flux without entropy fix and SpalartAllmaras model. The convective term in SA model is treated with first order upwind and the dissipative terms are treated with a Galerkin approximation. I had problem with positivity of turbulent viscosity. This was mainly due to the wall destruction term in the SA model, ie., the term
C<sub>w1</sub> f<sub>w</sub>(ν/d)<sup>2</sup> It is recommended to use an implicit scheme for integrating the SA model since it is rather stiff and can lead to negativity if you use the same timestep as used for the NS equations. Presently I am using an implicittype treatment only for the destruction term (all other terms in the SA model can be treated in a way that positivity is not violated by them) C<sub>w1</sub> f<sub>w</sub>(ν/d)<sup>n</sup>(ν/d)<sup>n+1</sup> where the superscript indicates the time level. If turbulent viscosity is becoming nonpositive then you can try to identify the problem by removing the destruction term and checking if the blowup goes away. 

October 5, 2005, 09:35 
Re: Scaling of the Adaptive Dissipation for NS

#6 
Guest
Posts: n/a

Another possibility to consider (if you haven't already) is the variable precision you're using. I've had CFD problem which converged to 104 or so using real*4 variables. Changing to real*8 allowed the convergence parameter to fall to reach ~ 107.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
CFX12 rif errors  romance  CFX  4  October 26, 2009 14:41 
adaptive grids for compressible flow  Shuo  Main CFD Forum  2  May 9, 2008 19:23 
Can 'shock waves' occur in viscous fluid flows?  diaw  Main CFD Forum  104  February 16, 2006 06:44 
Dissipation rate access  K. Kevala  FLUENT  0  July 14, 2004 11:11 
TKE SPECTRUM & DISSIPATION  Christian Paukert  Main CFD Forum  2  March 14, 2001 20:34 