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

numerical diffusion in tetrahedral grids

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2011, 09:49
Default numerical diffusion in tetrahedral grids
  #1
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
Hello everybody,

I made some cfd-simulations to get the mass fraction of a species passing a tube inside another type of species. Afterwards I was calculating kind of the ”spread” that the species experienced during this pass. Unfortunately the results differ a lot when I am using different grid types. When I am using a tetrahedral grid the spread is pretty low, when I am using a structured hexahedral grid the spread is about two orders of magnitude higher.
Could this effect arise due to the numerical diffusion within the tetrahedral grid?
We also found out that the larger the diffusion coefficient we are using, the smaller the spread of the species. But within a normal range of variation the difference in the spread of the species is not two orders of magnitude.
Can the effect of the numerical diffusion have such a huge impact on the results of my simulations?
It would be really nice, if somebody could help me!


Thanks a million in advance,
Lilly
Lilly is offline   Reply With Quote

Old   May 6, 2011, 12:31
Default
  #2
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 7
sail is on a distinguished road
thet are intrinsically more diffusive than exa, and in addition thet grid are ususlly relatively coarser than exa given a fixed number of cells, becuase you need 8 thet to resolve a hexa.
sail is offline   Reply With Quote

Old   May 27, 2011, 10:13
Default minimise/avoid numerical diffusion in tetrahedral mesh
  #3
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
Thank you for your help, sail!

Does anybody know how I can minimise or (in best case) avoid this numerical diffusion?
I am using the QUICK Scheme know which leads to a much better result, but is there a way to improve the results even more? I thought of maybe reducing the time step size to get a CFL number of about one? Does anybody has experience with this?
Thank you in advance for your help!
Lilly
Lilly is offline   Reply With Quote

Old   May 27, 2011, 11:08
Default
  #4
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 7
sail is on a distinguished road
from my experience:

cfl between 1 and 12
y+ no less than 30 and no bigger than 100, higher or lower values increase the diffusion
timestep as small as possible.
grid must be aligned with the flow, and possibly refined as much as possible where you have the "phase change"
at least second order in space, settle for first order in time, otherwise there might be some instabilities.

take notice that i have never done pipes simulations so the parameters might vary.

good luck
sail is offline   Reply With Quote

Old   May 29, 2011, 17:57
Default
  #5
New Member
 
A.R. Baserinia
Join Date: Jan 2010
Location: Canada
Posts: 24
Rep Power: 7
baserinia is on a distinguished road
Quote:
Originally Posted by Lilly View Post
Does anybody know how I can minimise or (in best case) avoid this numerical diffusion?
As Sail mentioned, the grid must be aligned with the flow velocity. In my experience, a tetrahedral grid introduces an enormous amount of numerical diffusion. What is the geometry that you are modelling? If it is a simple tube, you should use an extruded grid along the length of the tube.
baserinia is offline   Reply With Quote

Old   May 30, 2011, 07:40
Default
  #6
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
Thank you sail and baserinia for your help!

I will try to improve the cfl-number timestep size and y+.

Unfortunately, my geometry has a bifurcation which makes it really hard to create a structured hexahedral grid aligned with the flow (I tried different mrthods in the bifurcation area, but failed). Do you have any idea how to circumvent this problem?

Thanks a million for your advice!
Lilly
Lilly is offline   Reply With Quote

Old   May 30, 2011, 10:23
Default
  #7
New Member
 
A.R. Baserinia
Join Date: Jan 2010
Location: Canada
Posts: 24
Rep Power: 7
baserinia is on a distinguished road
Quote:
Originally Posted by Lilly View Post
Unfortunately, my geometry has a bifurcation which makes it really hard to create a structured hexahedral grid aligned with the flow (I tried different mrthods in the bifurcation area, but failed). Do you have any idea how to circumvent this problem?
Lilly
Lilly, for a 2D bifurcation, your meshing strategy should look like the one in the picture. You need to define 3 blocks and then mesh each block with quads. In 3D, the general idea is the same. However, at the sections of each tube you need to use a butterfly-grid. It's fairly straightforward but you have to do the blocking manually.

I'm not sure what program you're using for generating your mesh. I usually use ICEM for these sort of things.
Attached Images
File Type: png bifur.png (14.4 KB, 16 views)

Last edited by baserinia; May 30, 2011 at 10:49.
baserinia is offline   Reply With Quote

Old   May 31, 2011, 03:59
Default
  #8
Senior Member
 
Join Date: Feb 2011
Posts: 128
Rep Power: 6
Lilly is on a distinguished road
Thank you for your help Baserinia!

I don't have access to ICEM, but to Gambit and Tgrid. Did you work with them or do you know, whether I can build such a butterfly-grid using them?
Lilly
Lilly is offline   Reply With Quote

Old   May 31, 2011, 10:08
Default
  #9
New Member
 
A.R. Baserinia
Join Date: Jan 2010
Location: Canada
Posts: 24
Rep Power: 7
baserinia is on a distinguished road
Quote:
Originally Posted by Lilly View Post
I don't have access to ICEM, but to Gambit and Tgrid. Did you work with them or do you know, whether I can build such a butterfly-grid using them?
Lilly
You're welcome! I don't have much experience with Gambit or Tgrid, but any package which alloys you defining and editing blocks should work. As for the butterfly grid, you can find some info here.
baserinia is offline   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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Numerical error in tetrahedral cells Sam Main CFD Forum 1 February 17, 2009 18:18
Numerical error in tetrahedral cells Sam Main CFD Forum 1 February 14, 2009 15:51
Numerical Diffusion in CFX John S. CFX 4 August 17, 2008 19:47
Estimation of numerical diffusion varghese FLUENT 0 March 24, 2003 06:02


All times are GMT -4. The time now is 11:41.