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

How to treat BC at center of O mesh???

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 26, 2005, 14:12
Default How to treat BC at center of O mesh???
  #1
DISC
Guest
 
Posts: n/a
Use an O mesh (polar system) to calculate an incompressible flow. How to set BC at the center of the O mesh, to where all mesh lines in the radius direction sink?

How about interpolation, or, average?

Thanks for comments and sharing your experinece.

DISC

  Reply With Quote

Old   May 26, 2005, 14:32
Default Re: How to treat BC at center of O mesh???
  #2
ag
Guest
 
Posts: n/a
For a polar axis I have seen both used. An average is usually more robust, in the sense that it doesn't screw up the flow solver as much. However, polar axes don't always play nice and sometimes there is no good way to treat them short of trying a different grid strategy.
  Reply With Quote

Old   May 26, 2005, 17:28
Default Re: How to treat BC at center of O mesh???
  #3
Jim_Park
Guest
 
Posts: n/a
If your code has the flexibility, mesh it with quadralateral cells (rectangles as the most simple) and solve the equations in Cartesian coordinates instead of cylindrical.

If you wish, you can convert your solution (x, y) to cylindrical coordinates (r, theta).
  Reply With Quote

Old   May 26, 2005, 18:41
Default Since a circular pipe needs to be taken care of
  #4
DISC
Guest
 
Posts: n/a
Since the the discharge is from a circular pipe and thus O mesh is used.

Interestingly, when 2st-order scheme is used, the solution has problem at the axis. Whereas, when a 1st, upwind scheme is used, it looks much better.

D
  Reply With Quote

Old   May 26, 2005, 20:54
Default Re: How to treat BC at center of O mesh???
  #5
Jim_Park
Guest
 
Posts: n/a
I wasn't very clear - and I WAS incomplete. Sorry.

You can use boundary-fitted coordinates (deformable quadralaterals) and a block-structured scheme. This is definitely doable in Fluent and CFX. Using the Cartesian equations removes the 1/r singularity at the origin.

I think there's a diagram for this in the CFX manual.
  Reply With Quote

Old   May 26, 2005, 22:12
Default Jim: ou you mean Cartesian grid at the center?
  #6
DISC
Guest
 
Posts: n/a
Thanks Jim. In your reply you said Cartesian equations. You meant Cartesian grids?

Where can I find the CFX manual or similar things?

D
  Reply With Quote

Old   May 27, 2005, 08:34
Default Re: Jim: ou you mean Cartesian grid at the center?
  #7
Jim_Park
Guest
 
Posts: n/a
Actually I meant Cartesian equations. Calculate velocities as u, v, or u_x, u_y. The mesh (grid) would be made up of quadralateral cells. These are skewed to fit your circular boundary. After you have the solution, you can convert these to radial-angular components if you wish.

The only way I'm sure you can get the CFX manual is to buy a license for the code. If you're at a university that has a license, the license would (I think) give access to online documentation. This will really help, because the grid structure will be obvious when you see the diagram.

Perhaps some other reader can suggest a web site where a circular domain is meshed with a block of quadralaterals?
  Reply With Quote

Old   May 27, 2005, 12:42
Default Re: How to treat BC at center of O mesh???
  #8
Mani
Guest
 
Posts: n/a
Is there no solution to this problem besides using the Cartesian description? How do you calculate axisymmetric flow on a 2D grid (axial and radial directions), using the equations in cylindrical form? As far as I know this has been done before, so there must be some other way to deal with the singularity. The motivation for using a cylindrical description in the first place is given by its simplicity, at least in the axisymmetric case, where the problem is reduced to 2D. If the problem is not axisymmetric, then it makes less sense to use the cylindrical equations.
  Reply With Quote

Old   May 27, 2005, 13:04
Default Jim:reference for Cartesan eq on cylindrical grid?
  #9
DISC
Guest
 
Posts: n/a
Jim: are you saying use Cartesian eqs on a cylindrical grid? If yes, this will be interesting. But, where to find ref?

Thanks a lot

D
  Reply With Quote

Old   May 27, 2005, 21:48
Default Re: How to treat BC at center of O mesh???
  #10
Jim_Park
Guest
 
Posts: n/a
In the axisymmetric case, the velocity radial and tangential velocities are zero, and these conditions replace the radial and tangential momentum equations, so the terms with 1/r -> oo do not appear. Something similar happens in the axial momentum equation.

But you're right that, as soon as the flow becomes non-axisymmetric, the problem on the r = 0 axis reappears.

Other methods? Probably, but I'm not aware of those. I think averaging was mentioned earlier, and I'm aware of one application of that idea (about 1980). That was I believe NASA-VOF/3D, which was developed at Los Alamos for NASA to calculate sloshing of fuel in tumbling tanks in a low-gravity environment. They used the cylindrical coordinate system in 3 dimensions.
  Reply With Quote

Old   May 28, 2005, 04:29
Default Re: How to treat BC at center of O mesh???
  #11
tmp
Guest
 
Posts: n/a
A different possibility is to use a spectral method based on Gauss-Radau quadrature points in the radial coordinate in order to avoid the singularity.
  Reply With Quote

Old   June 2, 2005, 15:01
Default Re: How to treat BC at center of O mesh???
  #12
khairy
Guest
 
Posts: n/a
dear DISC i can help u but,the boundary condition is but at the boundaries, what is the thing at center(cylinder -airfoil or what)
  Reply With Quote

Old   June 3, 2005, 13:18
Default The problem is solved using DDM.
  #13
DISC
Guest
 
Posts: n/a
The problem is solved using a H-grid to cover the cylinder region (domain decomposition methd, or, zonal method).

Thanks all for your response.

I once posted a message telling this and conclusion. But it was gone now. Some people deleted the post?

DISC
  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
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Converting Starccm+ mesh Ladnam OpenFOAM 0 September 14, 2011 06:30
engrid -> save as .stl with boundarie codes Zymon enGrid 31 August 29, 2011 13:40
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 17:03.