CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Test Case for testing numerical dissipation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 16, 2008, 04:40
Default Test Case for testing numerical dissipation
  #1
Flo
Guest
 
Posts: n/a
Hi,

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
  Reply With Quote

Old   January 16, 2008, 04:51
Default Re: Test Case for testing numerical dissipation
  #2
Praveen. C
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   January 16, 2008, 15:04
Default Re: Test Case for testing numerical dissipation
  #3
Flo
Guest
 
Posts: n/a
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
  Reply With Quote

Old   January 16, 2008, 16:37
Default Re: Test Case for testing numerical dissipation
  #4
Ertan Karaismail CFD&AMP
Guest
 
Posts: n/a
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
  Reply With Quote

Old   January 19, 2008, 13:52
Default Re: Test Case for testing numerical dissipation
  #5
Flo
Guest
 
Posts: n/a
Hi Ertan,

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

Flo

  Reply With Quote

Old   January 20, 2008, 17:59
Default Re: Test Case for testing numerical dissipation
  #6
Ertan Karaismail CFD&AMP
Guest
 
Posts: n/a
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)

HTH

Ertan

  Reply With Quote

Old   January 25, 2008, 13:35
Default Re: Test Case for testing numerical dissipation
  #7
Paul Safier
Guest
 
Posts: n/a
Flo,

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
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
3D TRANSITION TEST CASE venkatesh4386@gmail.com FLUENT 0 March 9, 2009 14:04
Flat Plate Transition Test Case Adam CFX 1 June 24, 2005 00:12
Durham test case SAM FLUENT 0 August 16, 2004 06:01
gas combustion test case Tomasx Ochrymiuk Main CFD Forum 2 June 20, 2000 03:42
c1 body test case Eric Lenormand Main CFD Forum 0 March 2, 2000 07:54


All times are GMT -4. The time now is 00:31.