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

Understanding usual mesh constraints

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 18, 2013, 13:40
Default Understanding usual mesh constraints
  #1
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 4
malaboss is on a distinguished road
Hi everyone,
I am currently dealing with meshing issues on a cylinder case.
In fact, I saw that in my mesh I have to maintain a cell aspect ratio close to 1, and to make sure that the size a cell over the size of another cell in the vicinity of the first one, should not exceed 1.2.

However, I do not understand why we have to respect these ratios, numerically I mean. I need to know the quantification of the numerical error induced by a poor mesh, and this is why I need to know exactly from where does an error come from.

If you have any title of books, article or website pages I could read for that, I would be very delighted.
Thank you for your help
malaboss is offline   Reply With Quote

Old   March 19, 2013, 07:27
Default
  #2
Senior Member
 
andy
Join Date: May 2009
Posts: 129
Rep Power: 8
andy_ is on a distinguished road
Quote:
Originally Posted by malaboss View Post
In fact, I saw that in my mesh I have to maintain a cell aspect ratio close to 1, and to make sure that the size a cell over the size of another cell in the vicinity of the first one, should not exceed 1.2.

However, I do not understand why we have to respect these ratios, numerically I mean. I need to know the quantification of the numerical error induced by a poor mesh, and this is why I need to know exactly from where does an error come from.
The restriction comes from the particular discretization adopted by your software. What are you using?

A strong requirement for a constant spacing in all directions can follow from some triangular/tetrahedral based discretizations although not all. Grid generators can be made to automatically enforce it making it a minor practical problem although one can end up using a lot of elements. If the number of elements is becoming a problem then using some hexahedral elements aligned with the flow gradients should bring the element count down a lot.
andy_ is offline   Reply With Quote

Old   March 19, 2013, 08:41
Default
  #3
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 4
malaboss is on a distinguished road
Thanks for replying.
Actually I am using Open FOAM for a cylinder case in 2D. i made the mesh without using a mesh generator. I use the blockMesh utility.
The cells are hexahedron.

I don't see why the way derivation are discretized has an influence on the solution. What matters is the density of points where we make calculation and not the homogeneity of the space between those points, isn't it ?

I know I am wrong because I saw with some experiences that the density of mesh is not the only thing important (skewness, aspect ratio and sudden changes in size of cells are very important). But I would like to understand clearly what is going on numerically.

Thank you in advance !
malaboss is offline   Reply With Quote

Old   March 19, 2013, 10:08
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,099
Rep Power: 16
RodriguezFatz will become famous soon enough
Hi Malaboss,

This is what you need
http://powerlab.fsb.hr/ped/kturbo/Op...JureticPhD.pdf

Also this one is nice:
http://www.sciencedirect.com/science...45793012000667

Some of the questions you have are pretty basic, look in some good cfd book:
http://www.cfd-online.com/Books/show_book.php?book_id=4
or
http://www.cfd-online.com/Books/show...php?book_id=37

Cheers!
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   March 19, 2013, 10:50
Default
  #5
Senior Member
 
Join Date: Dec 2011
Location: Madrid, Spain
Posts: 133
Rep Power: 6
michujo is on a distinguished road
Hi, the effect of size ratio between adjacent cells on the accuracy of the numerical method is clearly seen when performing a finite difference discretization on a non-uniform grid.

You can show with pen and paper that if the cell size ratio is large, the order of the discretization will be lower than that with a uniform grid.

The same principle holds for different discretization approaches (i.e. finite volumes).

You can check the references you were given above. I can also suggest having a look at C. Hirsch "Numerical computation of internal and external flows".

Cheers,
Michujo.
michujo is offline   Reply With Quote

Old   March 27, 2013, 07:12
Default
  #6
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 4
malaboss is on a distinguished road
Hi everyone,
I come back to you to give you a feedback about what I just read.
The thesis of Franjo Juretic gives clear understanding of the numerical issues.
It explains well the effect of skewness and non orhtogonality.
There isn't much detail about aspect ratio, but we can deduce it from the expression of the truncation errors.
In the paper "High aspect ratio grid effects on the accuracy of Navier–Stokes solutions
on unstructured meshes" I did not find much numerical explanations about the effect of aspect ratio. It rather shows numerical experiments of different aspect ratios. It still is very interesting, but less for my problem.

Just to be sure, here is what I understood from the links about cell aspect ratio
For a first order accuracy, you have something like
TruncationError ~ delta(x)*dU/dx + delta(y)*dU/dy + delta(z)*dU/dz
For a second order accuracy you have :
TruncationError ~ delta(x)*dU/dx + delta(y)*dU/dy + delta(z)*dU/dz

With delta(x) delta(y) delta(z), the size of the cell in each direction.

Then, to know the what extent I can use cells with a high aspect ratio, I have to know if I have a first or second order accuracy and then compare the first or second order derivative terms of U in each direction.

Thanks for your answers, and thank you again for the links !
malaboss 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
Number of cells in mesh don't match with size of cellLevel colinB OpenFOAM Native Meshers: snappyHexMesh and Others 11 January 13, 2015 12:47
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52
Converting Starccm+ mesh Ladnam OpenFOAM 0 September 14, 2011 06:30
basic of mesh refinement arya CFX 4 June 19, 2007 12:21


All times are GMT -4. The time now is 03:15.