CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

numerical scheme without artificial diffusion artifact

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 25, 2011, 05:22
Question numerical scheme without artificial diffusion artifact
  #1
New Member
 
Peter Maday
Join Date: Aug 2011
Posts: 14
Rep Power: 7
mpeti is on a distinguished road
Dear Forum members,

I am using a modified version of icoFoam to keep track of the concentration of an agent in a pipe flow setup. The scalar field representing the concentration is "carried along" by solving a convection diffusion equation for each timestep using the computed flow velocities. What I experience is that even though there are relatively large gradients in the concentration values around the inlet (resulting from time varying BCs) the gradients quickly diminish (e.g. there seems to be a strong diffusion effect) even if the diffusivity constant is set to zero (!)).

I thought it might be an effect of the numerical schemes used to introduce such artifacts, however I am not quite sure which ones to use instead.

The numerical schemes currently used:
div:
velocity: Gauss limitedLinearV 1;
agent concentration: Gauss limitedLinear 1;

laplacian:
velocity: Gauss linear corrected;
pressure:Gauss linear corrected;
agent concentration: Gauss linear corrected;

P.S. if a non limited numerical scheme is used for the div of the agent concentration the simulation blows up

Thanks for your replies,
Peter
mpeti is offline   Reply With Quote

Old   October 26, 2011, 05:03
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,137
Rep Power: 20
akidess will become famous soon enough
Quote:
Originally Posted by mpeti View Post
What I experience is that even though there are relatively large gradients in the concentration values around the inlet (resulting from time varying BCs) the gradients quickly diminish (e.g. there seems to be a strong diffusion effect) even if the diffusivity constant is set to zero (!)).
Setting the diffusivity to zero will lead to a very stiff equation system, which is very hard to solve numerically without introducing artificial diffusion. There are numerical schemes designed to minimize numerical diffusion such as SuperBee or MUSCL (have a try if that improves your results for a realistic value of the diffusion coefficient). If I remember correctly the implementation of MUSCL in OpenFoam has the advantage that there is a bounded version (MUSCL01), but it's slightly more diffusive than SuperBee.

If you really need to solve a pure advection equation (e.g. for volume fraction in multiphase flows), even that will not be good enough. You'll need a special algorithm such as MULES + interface compression to handle such problems.
akidess is offline   Reply With Quote

Old   October 26, 2011, 11:36
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,907
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
The best results in terms of reducing diffusion is obtained with central schemes (their diffusive error is zero, since only dispersive errors are present, but they put limitations on the grid size).

If you really need zero diffusion, one possible way is to solve the tracer in a Lagrangian sense.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Reply

Tags
artifact numerical sheme

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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Expert-param:: Cht diffusion scheme PCFD CFX 4 July 12, 2010 13:49
Estimation of numerical diffusion varghese FLUENT 0 March 24, 2003 06:02
numerical scheme ado Main CFD Forum 3 October 12, 2000 08:20
Artificial numerical diffusion Valdemir G. Ferreira Main CFD Forum 8 February 3, 2000 14:31


All times are GMT -4. The time now is 21:11.