CFD Online Discussion Forums

CFD Online Discussion Forums (
-   Main CFD Forum (
-   -   Test Case for testing numerical dissipation (

Flo January 16, 2008 04:40

Test Case for testing numerical dissipation

I am looking for a simple test case, to compare different meshes (tetra, poly, hexa) and difference schemata with respect to numerical dissipation. Later on I would like to do a LES calculation for which I need a very low dissipative combination. Can anyone give me an advice? Thanks! Flo

Praveen. C January 16, 2008 04:51

Re: Test Case for testing numerical dissipation
A linear convection equation can tell you a lot about numerical dissipation. Try computing the advection of a smooth and discontinuous profile and see at what rate they are dissipated. The exact solution maintains the shape of the initial condition. If you give an initial condition like a hill, then look at what rate the maximum height of the hill gets reduced as time progresses.

Flo January 16, 2008 15:04

Re: Test Case for testing numerical dissipation
Hi Praveen,

thanks for your help, but still got some questions... so the easiest setup would be some kind of 2D channel with a constant inlet velocity and a periodic scalar at the inlet. I can then postprocess the scalar values along a line in the channel and can check the amplitude!?

Regards! Flo

Ertan Karaismail CFD&AMP January 16, 2008 16:37

Re: Test Case for testing numerical dissipation
In my opinion, the best and most reliable test case would be a swirling flow without diffusion. You can initially introduce a scalar at a rectangular region within the domain and than observe how the rectangular distribution of scalar changes in time. Physically the rectangular shape has to remain unchanged due to absence of diffusivity. However, you will get a deformed shape (distribution) due to numerical diffusion for sure. I suggest you use strongly monotone schemes. HTH Ertan

Flo January 19, 2008 13:52

Re: Test Case for testing numerical dissipation
Hi Ertan,

thanks, do you know, if I can do it with any of the commercial codes like starcd or fluent?


Ertan Karaismail CFD&AMP January 20, 2008 17:59

Re: Test Case for testing numerical dissipation
Why not.. I haven't done this study in fluent, but the procedure I described below should work out for you. At least it would be my first attempt.

1) Create your mesh (2D or 3D), import it to Fluent.

2) Separate a region (rectangular in 2D or cubic in 3D).

3) Define scalar (UDS) on that region and introduce that scalar only initially, (t=0). You may need a UDF for that. In the UDF also set the diffusivity of scalar to zero or to a very small number.

4) Enable fixed value for u and v velocities for the whole domain including the separated area and hook up a UDF for swirling flow field (u and v velocity components).

5) Set the convergence criterion only for scalar transport.

6) Run unsteady for two periods. (let the core of scalar pass two times its initial location)



Paul Safier January 25, 2008 13:35

Re: Test Case for testing numerical dissipation

As the other post suggested, for a test I would run a simple one dimensional convection equation for a scalar with an initial distribution of a square wave. After you convect it around for several time steps you'll see the square artifically diffuse as your routine adds numerical diffusion so as to remain stable. In my experience, canned over-the-counter routines don't fare well with convectively dominated equations. In my work, I accurately solved transport problems with Peclet numbers on the order of a million (i.e. zero diffusion) by using the Flux-Corrected Transport Method, by Boris and Book. Although it's not very easy to code, this method is excellent for solving convectively dominated PDEs in one and two dimensions.

Good luck, Paul Safier

All times are GMT -4. The time now is 05:35.