CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Modeling of boundary layer wind profile in CFX 5 (http://www.cfd-online.com/Forums/cfx/21538-modeling-boundary-layer-wind-profile-cfx-5-a.html)

Cuong NK August 22, 2005 09:41

Modeling of boundary layer wind profile in CFX 5
 
I am doing a modeling of a virtual wind tunnel using CFX5 and I try to model the boundary wind layer profile, which follow the either power law or log law. I set a box 2x2m cross section and 3m long and used expression to set the wind speed at inlet as a function of height (let say z coordinate). The result shows the velocity if still uniformly over the cross section.

If any one of you knows how to generate the boundary layer wind profile, please show me some instructions for that.

I am highly appreciating your help.

Regards,

Cuong NK


Carlos August 22, 2005 11:34

Re: Modeling of boundary layer wind profile in CFX
 
Maybe You can create an inlet zone (extra tunnel in front of your tunnel). Then the boundary layer comes from alone. If You use a rough wall, you may control your boundary layer, but Im not an expert its just an idea.

Cuong NK August 22, 2005 21:09

Re: Modeling of boundary layer wind profile in CFX
 
Thank you for your response Carlos! It's a good idea to create another inlet in front of the tunnel. In actual wind tunnel we use Spires and floor roughness to model the wind profile and turbulence profile but it is not so convenient to do the same in CFX since the size of problem becomes too big.

I still thing that we can generate wind profile and turbulence profile by declaring velocity and turbulence as a function of height at the inlet. If anybody has done that in CFX, please share!!!

Best regards,

Cuong NK


test August 23, 2005 05:25

Re: Modeling of boundary layer wind profile in CFX
 
Hi,

You can check if the profile boundary condition you have specified is correct in Pre itself. in the boundary condition tab, you can create contour plot/vector plots to check you profile.

There may be a small error in your profile specification. Check the profile in pre first before you go to the solver. A good practice would be to save the result backup before the iterations start (using expert parameter in the I/O section, backup file at zero= t). You can then post process this file to see if the intial conditions look fine.

Regards, test

Cuong NK August 23, 2005 08:05

Re: Modeling of boundary layer wind profile in CFX
 
Thank you very much for your recommendation! That was my error when I define the equation in Pre. It's a very good idea to check the profile in Pre as you recommended.

Regards,

Cuong NK


funster August 30, 2005 09:31

Re: Modeling of boundary layer wind profile in CFX
 
You can specify a log law profile for the velocity components at the inlet, also incorporating K and e for the turbulence and specify a roughness height on the wall defining the floor of the tunnel.

Run multiple tests to try and compare profiles, it will be a compromise between maintaining the profile through the empty model and also matching the profile at the cross section where the final test case (ie centre of the working section) model is to sit with the desired boundary layer profile.

Maintaining a constant profile can be tricky and a constant problem. Some codes allow a feedback mechanism to perpetuate the flow through the model. What happends is that you specify an inlet condition - your profile, amd then at the out let you feed back the outlet flow profile back into the inlet. This constant loop ensures that the result reaches a stable profile for a given inlet condition. This can then be input into the final model for a gived roughness and there should be no change in profile conditions throughth the model.

Hope this helps a little ?

Stuart

MuhammadK April 26, 2012 06:19

Hi everyone!

I searched this post as it has something related to what I am trying to do now.

I am also trying to build an expression for boundary layer wind profile.

What I did was setting the inlet velocity along the z direction, w as an expression, named BLZ

I had tried to insert a new expression, which is
(0.2047/0.4)[m/s] * loge (y + 0.00054[mm]/0.00054[mm])

My thesis supervisor did this with me just now and it works.
However, when I tried it myself, it does not work
Error:
Quote:

"Bad expression value 'BLZ' detected in parameter 'W' in object '/FLOW:Flow Analysis 1/DOMAIN:Default Domain/BOUNDARY:Inlet/BOUNDARY CONDITIONS/MASS AND MOMENTUM'.
CEL error:
Inconsistent dimensions on each side of '+' operator at position 29.
Dimensions on left: 'm'
Dimensions on right: '<dimensionless>'."
http://img577.imageshack.us/img577/7...ssionerror.jpg
Shot at 2012-04-26

Any thoughts? :)

Lance April 26, 2012 08:23

Quote:

Originally Posted by MuhammadK (Post 357155)

I had tried to insert a new expression, which is
(0.2047/0.4)[m/s] * loge (y + 0.00054[mm]/0.00054[mm])

The error is obvious, in loge you add y which has dimensions [mm] with something that is dimensionless (0.00054[mm]/0.00054[mm]).

My guess is that you forgot a parenthesis:
loge ((y + 0.00054[mm])/0.00054[mm])


All times are GMT -4. The time now is 06:28.