# numerical scheme without artificial diffusion artifact

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 October 25, 2011, 05:22 numerical scheme without artificial diffusion artifact #1 New Member   Peter Maday Join Date: Aug 2011 Posts: 14 Rep Power: 6 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

October 26, 2011, 05:03
#2
Senior Member

Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 921
Rep Power: 17
Quote:
 Originally Posted by mpeti 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.

 October 26, 2011, 11:36 #3 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,894 Rep Power: 26 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 live DVD/USB, hard drive image and virtual image. OpenQBMM - An open-source implementation of quadrature-based moment methods

 Tags artifact numerical sheme

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 PCFD CFX 4 July 12, 2010 13:49 varghese FLUENT 0 March 24, 2003 06:02 ado Main CFD Forum 3 October 12, 2000 08:20 Valdemir G. Ferreira Main CFD Forum 8 February 3, 2000 14:31

All times are GMT -4. The time now is 07:54.

 Contact Us - CFD Online - Top