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

Mesh inflation / Wall condition doubts

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 21, 2007, 12:38
Default Mesh inflation / Wall condition doubts
  #1
Kushagra Mittal
Guest
 
Posts: n/a
Hi there,

As a beignner, I again need your kind help.

1) I create my geometry and mesh in Gambit and then run simulations in CFX-11. CFX tutorails talk about 'inflation layers'. Is its objective same as that of size function/boundary layer in Gambit? Or CFXmesh-ICEM are the only option for mesh creation in order to get better results in CFX?

2) When I create fine mesh using tetra T-grid scheme, I have nodes in the range of 5*10^5 and elements 35*10^5. Meaning less calculating points than number of computing cells !

Is it fine with solver to have less computing points ? Any issues expected with the solution?

3) In my simulations, wall condition is 'No SLIP', still the plot(CHART) in CFX post doesn't give ZERO velocity at the wall? Is it because of interpolation ? I have tried to verify the same in tutorials and find the same. Any Comments from your valuable experience is highly welcome.

Your reply will help me a lot in clarifying my doubts and have a better understanding of this software package !

Many Thanks in advance !!!!!

Regards, Kushagra Mittal.
  Reply With Quote

Old   September 21, 2007, 13:35
Default Re: Mesh inflation / Wall condition doubts
  #2
CycLone
Guest
 
Posts: n/a
Hi Kushagra,

1) Inflation refers to the generation of prism layers next to the wall to increase the resolution of gradients normal to the wall. This is accomplished with the boundary layer function in Gambit.

2) CFX assembles control volumes around the element vertices, resulting in polyhedral control volumes and hence there are fewer nodes than cells with a tet mesh. While this results in fewer control volumes, there are far more integration points so the resolution of gradients is more accurate per control volume. If you compare FLUENT and CFX solutions, you may find the FLUENT solution is slightly more accurate for the same mesh, but much more costly to run (since you are solving 5x the number of equations), so you can afford to run a finer mesh in CFX.

The polyhedral control volumes are also much less sensitive to poor mesh quality. If your physics allows for it, you can see similar benefits in FLUENT by converting your tet mesh to polyhedra.

3. The No Slip condition is still applied. Because of the vertex centered formulation, the node for the near wall control volume lies on the boundary. To allow users to view both the conservative control volume value at these locations, as well as the boundary value, CFX Post differentiates these as "Conservative" and "Hybrid" fields. The Hybrid term originates from the fact that the solution field plotted is a hybrid of the conservative fields (for the interior nodes) and the boundary only fields. There are many threads on this topic on the forum, just search for "Hybrid Values" to see them. It is also explained in the documentation.

-CycLone
  Reply With Quote

Old   September 21, 2007, 15:34
Default Re: Mesh inflation / Wall condition doubts
  #3
Kushagra Mittal
Guest
 
Posts: n/a
Hi,

Thank you very very much...!!!!!!! []

I am amazed how well you explain these things....As you suggested, I have read the CFX documents and Now I am TOTALLY comfortable with it. It works !!!!!

Thanks a ton !!!! I will need guidance again and again...

Best Regards, Kushagra Mittal.
  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
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
UDF for wall slipping HFLUENT Fluent UDF and Scheme Programming 0 April 27, 2011 12:03
External Radiation Boundary Condition (Two sided wall), Grid Interface CFD XUE FLUENT 0 July 8, 2010 06:49
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 15:08.