Error reading profile data in expression in cfx post
 

Hello,

I need to incorporate different turbulent intensity values changing with height at inlet. In order to do so i created user defined function in the form of interpolation(data input) with ti as function name.

I then created an expression as ti(z) and checked this by plotting and evaluating it. I am getting the required plot.

For turbulence option at inlet I chose intensity and auto compute length and in fractional intensity column gave the expression name which includes my created function.

However in CFX post when i checked the turbulence intensity values by creating turbulence intensity expression and creating new variable for this expression, the values are not matching those which i had inserted in function. For example my highest value inserted was 0.15 at 0[z] but the contour with turbulence intensity variable is showing max value of 0.12 at 0[z]

Also the expression with the user function is showing error in cfx post as
ERROR
The following unrecognised name was referenced: ti.

why cfx post is not recognizing user defined function? Also why there is possible difference in turbulence intensity values?

Thanks and regards
banu

Here are some possible reasons why there is a difference:
* Hybrid vs conservative variables
* The turbulence quickly dissipates and your visualisation is after some dissipation

You cannot access user variables in the post processor. They are not in the output file. To put them in the output file you should define a user variable equal to the function and put the user variable in the results file.

Hi sir ghorrocks,

I created the additional variable in pre hence forth able to view my CEL function.

Regarding my Turbulence intensity query, if The visualization is after some dissipation, is there any possibility to obtain the contour before the dissipation starts?

Also with this dissipated turbulence intensity values, will my result be valid? As in I expected my results based on my input ed values, but obviously there is some dissipation. Will my result still hold good?

Thanks and regards
banu:)

If you view the boundary surface you should see the conditions applied to the boundary.

High levels of turbulence usually exist with high levels of dissipation - which means the turbulence dissipates very quickly. This is normal and correct. Unless you provide energy to the flow to keep the turbulence levels high then it will dissipate quickly. So if you want high levels of turbulence to flow in and not dissipate you will have to reduce your dissipation at the boundary condition.

So you will have to redefine your inlet conditions to have less dissipation. If you do not know what this is or how to define it then get a turbulence modelling textbook like "Turbulence modelling for CFD" by Wilcox.

ok, got it. Thanks a ton:)