
[Sponsors] 
May 26, 2005, 14:12 
How to treat BC at center of O mesh???

#1 
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 

May 26, 2005, 14:32 
Re: How to treat BC at center of O mesh???

#2 
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.


May 26, 2005, 17:28 
Re: How to treat BC at center of O mesh???

#3 
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). 

May 26, 2005, 18:41 
Since a circular pipe needs to be taken care of

#4 
Guest
Posts: n/a

Since the the discharge is from a circular pipe and thus O mesh is used.
Interestingly, when 2storder scheme is used, the solution has problem at the axis. Whereas, when a 1st, upwind scheme is used, it looks much better. D 

May 26, 2005, 20:54 
Re: How to treat BC at center of O mesh???

#5 
Guest
Posts: n/a

I wasn't very clear  and I WAS incomplete. Sorry.
You can use boundaryfitted coordinates (deformable quadralaterals) and a blockstructured 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. 

May 26, 2005, 22:12 
Jim: ou you mean Cartesian grid at the center?

#6 
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 

May 27, 2005, 08:34 
Re: Jim: ou you mean Cartesian grid at the center?

#7 
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 radialangular 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? 

May 27, 2005, 12:42 
Re: How to treat BC at center of O mesh???

#8 
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.


May 27, 2005, 13:04 
Jim:reference for Cartesan eq on cylindrical grid?

#9 
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 

May 27, 2005, 21:48 
Re: How to treat BC at center of O mesh???

#10 
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 nonaxisymmetric, 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 NASAVOF/3D, which was developed at Los Alamos for NASA to calculate sloshing of fuel in tumbling tanks in a lowgravity environment. They used the cylindrical coordinate system in 3 dimensions. 

May 28, 2005, 04:29 
Re: How to treat BC at center of O mesh???

#11 
Guest
Posts: n/a

A different possibility is to use a spectral method based on GaussRadau quadrature points in the radial coordinate in order to avoid the singularity.


June 2, 2005, 15:01 
Re: How to treat BC at center of O mesh???

#12 
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)


June 3, 2005, 13:18 
The problem is solved using DDM.

#13 
Guest
Posts: n/a

The problem is solved using a Hgrid 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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[ICEM] surface mesh merging problem  everest  ANSYS Meshing & Geometry  44  April 14, 2016 06:41 
[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 