CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] A mesh generation for aero acoustic computation (http://www.cfd-online.com/Forums/ansys-meshing/73739-mesh-generation-aero-acoustic-computation.html)

ringtail March 15, 2010 23:27

A mesh generation for aero acoustic computation
 
2 Attachment(s)
Hi everyone,
The following picture shows a mesh of a 2D cylinder. This mesh is mentioned in the document "Tutorial: Modeling Flow-Induced (Aeroacoustic) Noise Problems Using FLUENT".


Attachment 2595

Attachment 2596

Who can tell me how to generate a similar one or where to download the mesh file cylinder2d.msh

Wish your repies.

thanks very much.

mbell10 April 15, 2010 06:54

The mesh has been formed by creating a cell density region behind the cylinder. Here the cells are clumped together and allowed to expand at a particular rate. Its relatively straight forward in Icem

ringtail April 15, 2010 11:27

Quote:

Originally Posted by mbell10 (Post 254749)
The mesh has been formed by creating a cell density region behind the cylinder. Here the cells are clumped together and allowed to expand at a particular rate. Its relatively straight forward in Icem

dear Mark Bell

thanks for your reply. But, I do not quite catch your meaning, what does " Its relatively straight forward in Icem" mean?
Is there direct command for cell density in ICEM? what is it?

thanks again.

mbell10 April 16, 2010 05:45

Under the Mesh tab, there is a button, "Create Mesh Density".

It will allow you to create your regions of mesh density and control how dense the mesh is. It will take a little playing about with, but otherwise it's quite straight forward.

PSYMN April 16, 2010 12:13

ICEM CFD's create mesh density doesn't apply to Patch dependent 2D meshes, so make sure you have your surface mesh method set to "Patch Independent".

Simon

ringtail April 17, 2010 03:24

hi, Mark Bell and simon
i have read ICEM CFD help manual carefully. And now I know density box
"affects only Tetra, Cartesian, and Patch Independent surface mesh methods."

I tried to generate the mesh by HEXA MESHER, and then created a mesh density, and it did not work.

Is hexa mesh a cartesian mesh?

PSYMN April 17, 2010 13:18

Nope, these are all different methods... What matters is how the mesh is generated. The methods that work with the Density boxes all rely on top down meshing with a back ground grid... On the other hand, Hexa relies on a blocking structure that lets you mesh it any way you like... You can refine blocks in hexa or use blocking strategies (such as Ogrid) to refine the mesh...

The method closest to what you had seen in Gambit is the Patch Independent surface meshing with "quad" or "quad dominant". This method will accept density zones or sizing function in the same way (and for the same reasons) as they worked in Gambit...

Other methods, such as ICEM CFD Hexa, may be able to give a much higher quality mesh, but require a bit more practice and effort due to the higher level of user interaction. Have you tried the ICEM CFD Hexa tutorials?

Simon

ringtail April 19, 2010 02:27

3 Attachment(s)
Quote:

Originally Posted by PSYMN (Post 255072)
Nope, these are all different methods... What matters is how the mesh is generated. The methods that work with the Density boxes all rely on top down meshing with a back ground grid... On the other hand, Hexa relies on a blocking structure that lets you mesh it any way you like... You can refine blocks in hexa or use blocking strategies (such as Ogrid) to refine the mesh...

The method closest to what you had seen in Gambit is the Patch Independent surface meshing with "quad" or "quad dominant". This method will accept density zones or sizing function in the same way (and for the same reasons) as they worked in Gambit...

Other methods, such as ICEM CFD Hexa, may be able to give a much higher quality mesh, but require a bit more practice and effort due to the higher level of user interaction. Have you tried the ICEM CFD Hexa tutorials?

Simon

hi, Simon
yes ,i have.
as the below images show, I have generated the by using O-grid. The mesh quality seems good.
Attachment 3010

Attachment 3011

Attachment 3012

In fact, my real trouble is how to refine or coarsen the mesh. In order to make suer the y plus is approximate to 1, I have to make the first layer grid be close to cylinder wall enough. So the density of radial grid should be big. And for making sure aspect ratio do not exceed limitation of FLUENT, I have refined the density of circumferential grid too. as a result, the mesh became very very dense.( up to 3 million nodes.)

how could I coarsen the mesh ?

thanks.

PSYMN June 8, 2010 19:49

This is a bit late (I don't always have time to get back to CFD online threads), but hopefully you figured out how to adjust the edge params to have fewer parameters but the same intial distribution. You could even split that Ogrid so you could have two separate ratios.

I would probably have blocked it a bit differently, with HGrid thru the entire domain and then splits ahead and behind the hole, and above and below the circle. This would give 9 Hgrid blocks, the middle one would be centered on the circle. Then I would create an Ogrid in that center block, delete its center o grid and associate its center square with the circle... This will give higher quality than this current example and the mesh density would be easier to control.


All times are GMT -4. The time now is 10:45.