# Modeling of boundary layer wind profile in CFX 5

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

 August 22, 2005, 09:41 Modeling of boundary layer wind profile in CFX 5 #1 Cuong NK Guest   Posts: n/a Sponsored Links 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

 August 22, 2005, 11:34 Re: Modeling of boundary layer wind profile in CFX #2 Carlos Guest   Posts: n/a 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 I´m not an expert it´s just an idea.

 August 22, 2005, 21:09 Re: Modeling of boundary layer wind profile in CFX #3 Cuong NK Guest   Posts: n/a 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

 August 23, 2005, 05:25 Re: Modeling of boundary layer wind profile in CFX #4 test Guest   Posts: n/a 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

 August 23, 2005, 08:05 Re: Modeling of boundary layer wind profile in CFX #5 Cuong NK Guest   Posts: n/a 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

 August 30, 2005, 09:31 Re: Modeling of boundary layer wind profile in CFX #6 funster Guest   Posts: n/a 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

April 26, 2012, 06:19
#7
New Member

Join Date: Apr 2012
Location: Sydney, Australia
Posts: 10
Rep Power: 7
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/DOMAINefault 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: ''."

Shot at 2012-04-26

Any thoughts?

April 26, 2012, 08:23
#8
Senior Member

Lance
Join Date: Mar 2009
Posts: 606
Rep Power: 14
Quote:
 Originally Posted by MuhammadK 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])

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post HMR CFX 5 October 10, 2016 05:57 Luk CFX 3 February 27, 2009 04:22 Marco CFX 1 December 1, 2008 21:46 Erdem FLUENT 0 June 20, 2006 13:00 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15