I wrote a letter to you but ur mailbox rejected it.
Remote host said: 552 Message size exceeds maximum permitted,I'm afraid the attachment i mention at the following paragraph can be downloaded from my ftp
I am using your code calculating turbulent flow over a circular cylinder.For the unsteady periodic flow i use the t-ts physical time subiteration method and set dt=0.2 sub iterations=4(i think it is enough),and the grid is 201*100。All the grid files,init files,and the results are involved in the attachment.
Now i have got the periodic results(Re=500&1000),it seems linear turbulence models can't get periodic result for the separate flow so i add some nonlinear models to the code such as CLS(Craft,Launder & Suga),LL(LIEN & LESCHZINER),SZL(Shih,Zhu,Lumley).Consider the strong adverse pressure gradient I use the two-layer method(at inner layer I use Norrison-Reynolds one equation model and at outer layer I use these two-equation nonlinear models).
The results seemed not bad but when i compared it to experiment and numerical computations by X.-Y.LU AND C.DALTON(Journal of Fluids and Structures (1996) 10 ,527-541)，I found it in correct. The comparison is also in the attachment:e.g.In the experiment the St=0.21(Re=500) St=0.22(Re=1000) but my
I also checked the distribution of the streamwise mean velocity along the wake center-line(Re=1550,2150),and I find it much worse compared to the experiment. And the dissipation in the flow field seems quite strong cos I can only get three vortices at most so there is no vortex street.
I guess these incorrect results are due to B.C.s,cos I really don't know how to set the boundary conditions precisely.I usually set the left half 'farfield' BC and the right half 'subsonic outflow' BC(the back pressure is set to default),and I find this the best.If I set the right half 'EXTRAPOLATE' the CL/CD would damp with time,and the freestream velocity is 0.088 if I set Mach=0.1 in the INIT.DAT,how could this happen?Would you please explain more about B.C.s?so confused.
OK.My last question is the 'VISCOUS' value in the INIT.DAT.When I set
in the INIT.DAT the results are worse than the situation when i set
The amplitude of CL/CD is much smaller in the previous situation when Re=1000,and in the situation Re=500 the amplitude of CL is 0.01nearly zero. The wake seems not reasonable,either.For this blunt body the viscous effect is obvious in the both direction unlike the airfoil!How could this happen that viscous 2 is worse than viscous 1?
Your comments will be most appreciated!
I was able to download your files and look at the results. You have clearly been busy to have added the models that you list. I am very interested in how the rest of your work goes.
I think that the first problem to evaluate is the grid and the second is the time step. You have generated an O-type grid for calculating the shedding flow from the circular cylinder. An O-type grid has a fundamental problem that it loses resolution in the wake of the body. It is more appropriate for an inviscid calculation than for this viscous calculation. You, at least, need to cluster the grid points in the wake region if you continue to use an O-grid. A C-grid would work better. Or a C-grid on the upstream portion of the cylinder and a Cartesian grid on the back half; this would have the benefit that the implicit operator would not be broken across the current CUT line and would give you more freedom in generating a grid with the resolution where you need it.
If you plot contours of the velocity for your calculations, you will see the eddies shedding from the cylinder in the near wake of the cylinder. However, further downstream (by about 3-4 body diameters) these eddies have been dissipated and are not identifiable. At this location you have no unsteady flow structure at all but only a very diffused turbulent wake. If you overplot the grid onto these contours, you can see that youhave only two or three cells covering a very diffuse eddy; once it is this poorly resolved, it dissipates completely. The velocity contours are then almost constant to the outflow boundary.
I agree that a linear eddy viscosity model will generate too much eddy viscosity for this case; a non-linear model will do a better job by reducing the dissipation and allowing the flow to establish itself as unsteady. However, I would not draw any conclusions on the suitability of any model for this case based on the results on this grid. This grid is too coarse and will dissipate the eddies for any model. I think that this is part of the problem with the VISCOS 2 issue also; turning on the viscous terms in the I direction adds more dissipation and you already have too much. So everything dissipates out even quicker. This should really be run with full Navier-Stokes terms in both the I and J direction on a much finer grid. Then I don't believe that the additional viscous terms will cause the problems you are seeing now.
I am also concerned that the inner iterations on the iterative implicit operator are not sufficient. You need to do a study - on a sufficiently refined grid - on the effect of the inner iterations. You also need to monitor the convergence of the inner iterations. If the overall time step is small enough, then a small number of inner iterations may be sufficient. You can only know by doing a convergence study.
And this comes back to the grid issue. You cannot make a calculation on a single grid and then assume that your answers are correct. You need to do a grid convergence study being careful that your coarsest grid is sufficient to capture the physics. Otherwise the grid convergence study is meaningless.
How did you verify your coding of the new turbulence models?
I think that your boundary conditions are probably ok. The boundary conditions will be a little less of a problem once you have the grid refined.
I do not know how refining the grid will make your calculations compare to the experiment. But refining the grid and time step are necessary first steps before you can make a comparison with data. Please keep me informed on your progress and good luck.
Another note, the paper that you referenced for the numerical results, Lu and Dalton, is for laminar results. Did you run the Re = 500 and 1000 laminar to match there case? If you ran it turbulent, I would expect a more diffused vortex street. I could not tell from their paper what the location of the outer boundary domain was. This would affect the grid distribution dramatically. Also, a turbulent grid would have a smaller wall normal spacing than laminar which would further reduce the grid resolution in the vortex region.
I have generated a C-grid and I encountered the orthogonality problem,it had the following output:
MAIN : FIXQ : ERROR-> Density < 1.00E-08 at 4 locations
Pressure < 1.00E-08 at 3 locations
RUN ABORTING! Attempting to write output and restart files.
can you give me some advice?I have sent the grid file to you
The errors indicate that the solution failed when the density and/or pressure became zero or negative. The pressure and density are positive quantities, and cannot be negative. If they get too small, it is an indicator that the solution will not run as is. There are several reasons why this can occur in the iterative process. Different time steps and/or multigrid strategy will often fix this problem. Some turbulence models have much more problem than others due.
However, this is quite likely due to the grid that you are using. You have created a C-grid which should alleviate some of your issues with the O-grid. But the grid needs to smoothly vary rather than have a discontinuity in spacing. ISAAC (and many other CFD codes) is designed for a smoothly varying grid. The grid spacing should increase by no more than 1.15 times its neighbor in the viscous region (i.e., if dy_j is the spacing at the j-th point/cell in the wall "normal" direction and dy_j+1 is the spacing in the same direction at the next outer point/cell, then dy_j+1 <= 1.15 dy_j. I actually prefer closer to 1.1, but up to 1.25 should work. 1.1 should give better answers. 1.25 is too high. There are papers in the literature that talk about the truncation error as a function of the stretching.
You have a large jump in the spacing in the wall normal direction. This will not give an accurate solution, and is probably causing the code to get negative pressures and densities.
Log in to post a comment.
Sign up for the SourceForge newsletter:
You seem to have CSS turned off.
Please don't fill out this field.