CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] Grid refinement ratio for unstructured mesh

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

Like Tree2Likes
  • 1 Post By oj.bulmer
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   February 28, 2013, 12:20
Default Grid refinement ratio for unstructured mesh
  #1
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Hello,

I am trying to streamline the mesh independence practices using Grid Convergence Index and Richardson Extrapolation as they are considered the best in practical CFD. (Ref: Roache, P. J. "Perspective: a method for uniform reporting of grid refinement studies." TRANSACTIONS-AMERICAN SOCIETY OF MECHANICAL ENGINEERS JOURNAL OF FLUIDS ENGINEERING 116 (1994): 405-405.)

Now, element sizes for the consecutive meshes should be known to get the grid refinement ratio used in the calculations in this procedure. But since we use unstructured mesh along with the extruded mesh; I am not sure if the value of element local element size (in the important regions of high gradients) is representative of the size for that particular mesh.

Roache suggests the following formula for grid refinement ratio r for unstructured meshes, using their element-counts N_1 and N_2:

r = \left(\frac{N_1}{N_2}\right)^D

Now, he defines D as Dimensionality. What does it mean and how to calculate it from the fluid domain??

Thanks
OJ
kiddmax likes this.
oj.bulmer is offline   Reply With Quote

Old   February 28, 2013, 13:05
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Although I never followed that method, but what I heard is that you need to refine the successive meshes in such a way that it should be double of the former.

For example : 2k, 4k, 8k.

If the problem is 1D. Then you have to make the refinement by factor of 2 (2 power 1) in x-direction

If the problem is 2d then you have to make the refinement in each direction by factor square root of 2.

If the problem is 3d then you have make the refinement in each direction by factor of cube root of 2.

I dont know how you can achieve that ratio for tetra mesh and specially for patch independent method (may be by playing with surface size).
Far is offline   Reply With Quote

Old   March 1, 2013, 05:28
Default
  #3
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Thanks Far. A bit of search and I realized that dimensionality D is actually the no. of directions in which there is significant variation of results. i.e. 1 for one dimensional, 3 for 3 dimensional etc. The same has been reciprocated in other forums here.

If I may ask, do you personally recommend this method for mesh independence when it comes to unstructured meshes? Or you rely on more general methods of assessing the parameters of interest from results of successive meshes and choose the mesh when you see no significant variation in them? The only problem in this approach is there seems to be no agreed quantification of word "significant".

In this paper, Richardson's extrapolation takes into account the results of meshes that are successively refined and then extrapolates this to predict the value of result at zero grid spacing (i.e. continuum). At the same time, the Grid Convergence Index helps understand if the results generated in the current successive meshes are sufficiently close to the asymptotic range, where any refinement in the mesh won't result in significant change in results. This way we not only ensure the mesh independence but also predict the numerical solution at continuum. Obviously, there will be a difference between actual result and numerical result at continuum, but then, CFD is about getting the best results within its caveats.

Regards
OJ
oj.bulmer is offline   Reply With Quote

Old   March 1, 2013, 05:52
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
If I may ask, do you personally recommend this method for mesh independence when it comes to unstructured meshes? Or you rely on more general methods of assessing the parameters of interest from results of successive meshes and choose the mesh when you see no significant variation in them? The only problem in this approach is there seems to be no agreed quantification of word "significant".
Actually I love this method but find it very demanding for the industrial problems where geometries are complicated and you dont have clear directions for mesh refinement. Moreover you dont know in which direction you have maximum effect.

So I rely on the collective wisdom gained through other people's experience. Which suggest that you must ensure:

1. Quality of gird
2. Y+ requirements for the particular turbulence model (if flow is turbulent)
3. Mesh refinement in high curvature areas.
4. Mesh should be fine enough to capture the geometry features sharply (you need to decide how much enough is enough ).
5. Mesh refinement in normal direction where you have high gradients
6. Finer mesh in wake region.
7. Stream-wise mesh refinement if you have laminar to turbulent transition.
8. Finer mesh in shock region.
9. Finer mesh in mixing area

So after ensuring above criteria and generating acceptable mesh as per my experience (or try to match with the quality research article in no of nodes and Y+ values) I would go for two more meshes. One coarser and other one finer to satisfy the Paper reviewers or professor in your case.

PS: I strongly recommend this method to you if you can bear the frustration due to this method when you will apply it to complex industrial problem and specially with tetra mesh. But if you are successful in this method then your results will be accepted by any one.
kiddmax likes this.
Far is offline   Reply With Quote

Old   March 4, 2013, 06:39
Default
  #5
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Thanks Far for the detailed reply. Typically the actual order of accuracy of the CFD simulation is always smaleler than the local order of accuracy of the stencil used (smaller than 2 for second order etc) and a part of this reduction is due to grid quality. The suggestions you gave will definietely help here but yet we won't for sure know the grid independence.

Quote:
Actually I love this method but find it very demanding for the industrial problems where geometries are complicated and you dont have clear directions for mesh refinement.
Regarding the demanding nature of the method, I can say that if you go by Richardson's extrapolation, then the grid refinement ratio HAS to be integer and the smallest possible value is 2. In unstructured 3D mesh, this means the element size changes by 8 times! Trouble is, if you coarsen by 8 times, the mesh is not likely to remain in the asymptotic range. If you refine by 8 times, the computational cost becomes mammoth.

Roache's Grid Convergence Index addresses the exact issue and suggests a minimum refinement ratio of 1.1 (non-integer). Thus the mesh count increases by just 33% [(1.1/1)^3=1.33, (1.33-1)/1 = 0.33 = 33%]. Now creating three meshes with element count separated by 33% is reasonable effort, if it gives a scientific measure of the grid independence. Hence I am taking the trouble to explore this method

OJ.

Last edited by oj.bulmer; March 4, 2013 at 06:48. Reason: Clarification for mesh count
oj.bulmer 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
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
Weird snapping outside a refinement region jasimpson89 OpenFOAM Meshing & Mesh Conversion 0 July 29, 2012 20:46
Boundary layer in a pipe Clementhuon OpenFOAM Native Meshers: snappyHexMesh and Others 6 March 12, 2012 13:41
pressure eq. "converges" after few time steps maddalena OpenFOAM Running, Solving & CFD 69 July 21, 2011 07:42
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38


All times are GMT -4. The time now is 19:57.