CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   How to define roughness height in a fluid domain (http://www.cfd-online.com/Forums/cfx/23149-how-define-roughness-height-fluid-domain.html)

Afzal October 6, 2006 12:41

How to define roughness height in a fluid domain
 
Hi friends, I m a new user to CFX, I am solving laminar flow problem for a channel. How can I assign roughness height to any of the walls of the channel which is a fluid domain, if it is possible. If not this way can you please suggest any other way to do laminar flow in a rough channel using CFX.

your responses will be highly appreciated and acknowledged.

Thanks

johnny October 6, 2006 13:07

Re: How to define roughness height in a fluid doma
 
Simply select "rough wall" instead of "smooth wall" for Wall Roughness on your wall boundary under the Boundary Details panel. Then enter the roughness height.

Michael October 6, 2006 18:11

Re: How to define roughness height in a fluid doma
 
Contact Ansys-CFX and ask for the following paper.

Treatment of rough walls in CFX-10 by R. Lechner and F.R. Menter July 2005

Discusses the theory behind the rough wall calculation and most importantly you need to know the equivalent sand-grain roughness. The paper provides a reference.

Afzal October 6, 2006 22:43

Re: How to define roughness height in a fluid doma
 
Mr. Johnny, Thanks for your quick response,

Actually this option is not visible to me when I define my domain as "Fluid". only two options are in the boundary detail; free-slip and no-slip. I saw rough wall and smooth wall option under the solid face of solid-fluid interface, there is an option for roughness height. But as I have only fluid domain (laminar flow in a channel) I am not seeing the way to assign roughness height to any of the walls on the channel.

Your responses will be appreciated

johnny October 7, 2006 07:27

Re: How to define roughness height in a fluid doma
 
You need to change the wall boundary to "no slip" before the wall roughness option appears. And you must have a turbulence model defined (ie. the case cannot be laminar if you want to specify a roughness).

And in addition to Michael's point, you can check Schlichting's book for equivalent sand grain roughnesses as well.

Afzal October 7, 2006 10:50

Re: How to define roughness height in a fluid doma
 
Thanks again,

I think problem will be solved using turbulence model with roughness defined in terms of equivalent sand grain roughness.

Afzal October 7, 2006 10:55

Re: How to define roughness height in a fluid doma
 
Thanks for your useful suggestion,

I got the point to incorporate roughness height in terms of equivalent sand grain roughness under simulation with turbulence model.

Bart Prast October 9, 2006 03:56

Re: How to define roughness height in a fluid doma
 
When using a omega based turbulence model, the roughness option is not visible in pre (at least not in cfx10). You have to manually add it in ccl. Using the SST model (which is omega based at the wall) will hence also not show the roughness option.

If you switch to a k-epsilon model, this option should come up in the wall boundary treatment when switching from smooth to rough wall

Bart


All times are GMT -4. The time now is 01:12.