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

Deciding the mesh element size in CFD

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 2, 2012, 18:24
Default Deciding the mesh element size in CFD
  #1
Senior Member
 
---------
Join Date: Oct 2010
Posts: 295
Rep Power: 7
saisanthoshm88 is on a distinguished road
Could some one please let me know how to choose / decide on the element size for meshing in a CFD analysis.
__________________
Best regards,
Santhosh.
saisanthoshm88 is offline   Reply With Quote

Old   August 3, 2012, 03:10
Default
  #2
Senior Member
 
cfdnewbie
Join Date: Mar 2010
Posts: 550
Rep Power: 10
cfdnewbie is on a distinguished road
Depends on your method (FV, FD, FE...), your flow situation, boundary conditions, time step considerations, RAM size, CPU time available, governing equations.... impossible to give a general answer here...
cfdnewbie is offline   Reply With Quote

Old   August 3, 2012, 05:44
Default
  #3
Senior Member
 
Join Date: Aug 2011
Posts: 251
Rep Power: 6
leflix is on a distinguished road
There is at least one global rule.
If you perform 3D DNS, then the whole number of grid points should be N=Re(power 9/4)
where Re is the Reynolds number.
So if for instance you have Re=1000 then it would require 178 grid points in each direction NX=178, NY=178, NZ=178.
If you are below this grid resolution it does not mean thecomputation will faill.It is just the requirement to capture the smallest eddies at the Kolmogorov scale.

So the grid size is first a question of the level of accuracy you expect.
Apart of this accuracy requirement,you have some requirements due to the stability of your temporal scheme.
It links the grid size and the time step.
for explicit schemes the CFL condition is the rule. roughly speaking it indicates that between a time step period, the information which travels at velocity U, must not cover a distance greater that a grid size.

so start to decide what should be the grid size following your accuracy requirement.Then you apply the CFL condition and it will give you the time step.

Implicit time schemes are theoretically unconditionnaly stable. which means that whatever the grid size, any time step will work. In practice it is not completely true. And even if the constraint is less than for explicit schemes you can choose greater time step than those for explicit schemes.

For the same accuracy, high order spatial schemes will require less grid points than low order schemes.
It means that with a low order scheme (upwind scheme) you can obtain the same accuracy with a high order scheme,but it would cost much more towards grid points and thus computational time.

To verifiy that you have used the correct grid size, and to validate your results you should perform griz size independancy tests. You compute your solution with a given grid size. Then you refine the grid and compute again. You do this several time with finer and finer grids. Then your monitored solution at one given location and at the same time step of course, should tend assymptotically to one value.
The grid size for which the monitored solution does not evolve anymore, will be the right size.
leflix is offline   Reply With Quote

Old   August 3, 2012, 09:14
Default
  #4
Senior Member
 
cfdnewbie
Join Date: Mar 2010
Posts: 550
Rep Power: 10
cfdnewbie is on a distinguished road
Quote:
Originally Posted by leflix View Post
There is at least one global rule.
If you perform 3D DNS, then the whole number of grid points should be N=Re(power 9/4)
where Re is the Reynolds number.
So if for instance you have Re=1000 then it would require 178 grid points in each direction NX=178, NY=178, NZ=178.
If you are below this grid resolution it does not mean thecomputation will faill.It is just the requirement to capture the smallest eddies at the Kolmogorov scale.
Am I mistaken, or is the Kolmogorov scale estimate just a measure of proportionality? I.e the relationship I remember goes like nu = K * Re(power 9/4), where K is the unknown proportionality constant..... that would mean that you cannot fix your minimum N the way you described, the only thing you could do is to do a full DNS of a flow at a given Reynolds number, ensure you do indeed have a DNS and then use this relationship to compute N for a different Re....

Are you sure that's an exact equation, not a proportionality relation?
cfdnewbie is offline   Reply With Quote

Old   August 3, 2012, 09:27
Default
  #5
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,002
Rep Power: 17
flotus1 will become famous soon enough
You are right, it is actually just a proportionality relation.
flotus1 is offline   Reply With Quote

Old   August 3, 2012, 10:48
Default
  #6
Senior Member
 
Join Date: Aug 2011
Posts: 251
Rep Power: 6
leflix is on a distinguished road
Quote:
Originally Posted by cfdnewbie View Post
Are you sure that's an exact equation, not a proportionality relation?
yes indeed you are right cfdnewbie and Flotus1, N has to be proportional to Re(power 9/4).
leflix 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
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 2 November 25, 2012 08:54
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 02:48.