[mujahidbadshah]

Hi all,
I want to specify a non uniform turbulence intensity at the inlet boundary conditions. I have a two columns csv file. The first column represent the depth and the second the turbulence intensity.
"Can I use this csv file of depth versus Turbulence intensity directly? Please tell me the procedure in the CFX? and what is the variable name to be used in the CFX user expression for turbulence intensity?

[ghorrocks]

You can set turbulence intensity at inlets. It does not have a native CFX variable, it is a derived variable - so when you define turbuelnce intensity at the inlet it is converted to k and e/w.

To apply you data put your data into a 1D interpolation function, and use that function as the turbulence intensity input variable at your inlet.

[ghorrocks]

I have just seen this post is essentially the same as this post: http://www.cfd-online.com/Forums/cfx...ndary-cfx.html

Please do not post duplicate posts. It wastes everybody's time.

[mujahidbadshah]

Thanks for the reply. I will avoid duplicating threads in the future. Can you please tell me what should be the variable name that I should use for the turbulence intensity in the csv file. I have tried the variable name fractional intensity but it gives me error.
Thanking in anticipation.

[ghorrocks]

You do not use CSV files to set up 1D interpolation functions. Have a look at the CFX documentation or tutorials for a description of how to set them up.

[mujahidbadshah]

Thanks a lot. I will read the documentation and then discuss.

[mujahidbadshah]

I have created a user function using 1D interpolation and data points available. Now the problem is that when I input this function at the inlet boundary it gives me an error. I think I am missing a step in between. Kindly, explain a bit more if not inconvenient to you.

[ghorrocks]

What error message are you getting?

[mujahidbadshah]

I followed the following procedure:
1. In CFX Pre inserted a new expression named" TurbInt"
2. On the basic setting Tab of the function,selected the:
i. Option--- interpolation(Data)
ii. Argument Units--- m
iii. Result Units--- percent(Because Turbulence Intensity is dimensionless)
iv. Interpolation data
option--- One Dimensional
v. in the window for coordinate and value--- Right click and imported the coordinate points and values and click ok
-----------------------------------------------------------
3. Edit inlet boundary
a. On the boundary detail tab
i. Turbulence Option---Intensity and autocompute length
ii. Fractional Intensity---TurbInt()(This is the name of interpolation function created)
------------------------------------------------------------
4. I got the following error message:
Bad expression value 'TurbInt()' detected in parameter 'Fractional Intensity' in object '/FLOW:Flow Analysis 1/DOMAIN:fluid domain/BOUNDARY:inlet/BOUNDARY CONDITIONS/TURBULENCE'.
CEL error:
In the expression assigned to 'Fractional Intensity', the function 'TurbInt' is called with the wrong number of arguments (0 - expected 1).

[Lance]

Originally Posted by mujahidbadshah

ii. Argument Units--- m
[...]
option--- One Dimensional
[...]
ii. Fractional Intensity---TurbInt()(This is the name of interpolation function created)
[...]
In the expression assigned to 'Fractional Intensity', the function 'TurbInt' is called with the wrong number of arguments (0 - expected 1).

You need to call your function with a coordinate. If your turbulence values are varying on your inlet along the x-direction, use TurbInt(x) instead of TurbInt().

[mujahidbadshah]

Thanks a lot to all of you for giving me your time. You have solved my problem. The issue of specifying non uniform turbulence intensity has resolved.

Best Regards