Hi all!

I have problems with the TVR: I have previously searched through the forum and I found very interesting solution approaches: I tried the most of them, but I'm still having problems with it.

I am simulating an air flow past a very simple 3D geometry, a prism with rectangular profile, which is perpendicular to the flow. The rectangle profile is aprox. 1.2m tall and 0.3m thick, and the prism is 2.1m long.

As this prism is oposed to the flow, and the inlet velocity is high (180Km/h) the turbulence behind it is really strong. I have done several meshes, and due to my computational resources, I am limited up to a mesh of 1.2million cells: the mesh is fine at the wake of the rectangle.

I simulate over 160 iterations with 1st order squemes, k-e standard and std. wall functions. All is ok up to here, no TVR limited. But when I switch to 2nd order squemes (QUICK), it shows the message of limited TVR in a few cells. I cannot refine more the grid, I switched to coupled solver (I know that it is not necessary for incopmpressible flows, but it damps a little the generation of TVR) and I switched also to FAS Multigrid solver with VCycle for K and E, and BCGSTAB smooth (also with 2 pre-sweeps)... but TVR continues to increase.

I'm quite desperate, 'cause I have run out of more ideas. Do you know how to rid of this message or this is OK because my type of problem is very turbulent? I have also to simulate this shape with a wind of 320km/h and I'm afraid that in this case TVR will be even more high :S

Please, a little help needed. Thanks to all!

Freeman

In Fluent, go to Solve>Controls>Limits and set the maximum turb. viscosity ratio at whatever is appropriate for your case.

There are many things you can do.

First of all go to control panel and in under relaxation factors, change the urf for turbulent viscosity to something small. I would keep 0.1 or less till k eps are sort of converged.

Further if i read you correctly you do not want to use second order upwind. (using QUICK).

If you wish to use more accurate like CDS , you could use bounded central scheme. (bounded CDS).

This scheme is directly not available, but you can enable it with little effort.

Go to (on command prompt) : solve -> set -> expert

say 'y' to Allow selection of all applicable discretization schemes

Now check the solution control panel and enjoy bounded CDS.

:-D

i dont see the CDS in solution panel

Maybe you can think of keeping the epsilon equation first order. This will make the e field more diffusive and hopefully also your TVR more stable.

/M

Thanks a lot to all; all your advices encourage me not to desperate with this "error", as I see it is not really critical in my case, because the simulation arrives to the convergence after 2500it, with residuals in the order of 1e-5, and TVR limited in 3% of the cells (40.000 out of 1,2million) and the Cd correlates well with the literature; I prefer not to change the parameter of the TVR, but perhaps in order to avoid the message it would be better to use 1st order scheme in k, as mange says.

@Fluent-user: I need to use 2nd order schemes, as I want a precise estimation of the forces, pressures and Cd of the object. By the way, OUTSTANDING your cheat for displaying all the discretizations schemes: I was surprised... Thanks a lot for this tip =)

Again, thanks for your time. Good luck and cheers =)!

Hi FreeMan, I think you could change the tuerbulence model to K-E RNG, it usually works when you have very different reynolds numbers in your domain... Very interesting the bounded central scheme (bounded CDS), did it work to reduce the VTR?

I had no time yet to investigate this about the CDS, but I have read that it may introduce some inestabilities during LES simulation, as it amplificates creation of vorticity...

By the way, really interesting that with the RNG: I didn't know about this model fits better for higher Re. I will investigate when I finish my reports this week; thanks for your notes, Fran

Warmest Regards, Freeman