CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   How can I make an interpolated function? (http://www.cfd-online.com/Forums/cfx/23313-how-can-i-make-interpolated-function.html)

 Se-Hee November 18, 2006 05:38

How can I make an interpolated function?

Dear All,

I am trying to make the heat transfer coefficient function, h(T), with respect to T. I have some sampled data sets as follows:

T:: 280 290 300 350 400

h(T):: 2 7 8 12 14

Here, I'd like to make an interpolated function of which name is 'myH.' Where can I setup this kind of function and how can I use it?

Many Thanks, Se-Hee

 Glenn Horrocks November 19, 2006 18:19

Re: How can I make an interpolated function?

Hi,

This is a CEL 1-d interpolation expression. It is described in the documentation.

Glenn Horrocks

 Se-Hee November 20, 2006 04:23

Re: How can I make an interpolated function?

Dear Mr. Glenn,

Thanks for your comments. I have built my own interpolated function followed by your guide as follows:

1) In CFX-Pre, Create/User function

2) My function name is 'myHCoeff'

3) Interpolation, One dimensional

4) Input data set: Temperature .vs. heat transfer coefficient

5) OK

And when I use this function as boundary condition, how can I express the function? There were some errors to express my defined function when I try to use it. My expression was 'myHCoeff(T).' Is it incorrect?

Many thanks,

Se-Hee

 Robin November 20, 2006 12:52

Re: How can I make an interpolated function?

What were the errors?

 Se-Hee November 22, 2006 20:08

Re: Error Message

The error message is as follows:

The variable 'T' referenced in parameter 'Heat Transfer Coefficient' in object '/Flow/Domain:Tank/Boundary:TankH/Boundary Conditions/Heat Transfer' does not have one of the required prefixes: phase or particle.

Se-Hee

 Se-Hee November 24, 2006 01:44

what is the prefixes: phase or particle?

As I mentioned in the above message, the error message was as follows:

The variable 'T' referenced in parameter 'Heat Transfer Coefficient' in object '/FLOW/DOMAIN:Tank/BOUNDARY:TankH/BOUNDARY CONDITIONS/HEAT TRANSFER' does not have one of the required prefixes: phase or particle.

Here, could anyone please explain 'phase or particle'? I've tried many ways for resolving my problem, but I am still stuck at this stage.

Se-Hee

 Johnny November 24, 2006 07:32

Re: what is the prefixes: phase or particle?

If you have a multiphase flow, you need to add the phase/particle name before variables. Example:

Air Ideal Gas.Temperature

Maybe this is what the error message is referring to?

 Se-Hee November 25, 2006 08:30

Re: solved this problem with input profile.

Considering your comments, I have solved this problem at last as follows:

1. making profile instead of table

2. retype the function -> myHCoeff.hval(WireAl.T)

where myHCoeff represents the function name of which I defined, hval represents the value of my function with reapect to temperature, and WireAl represents the material name of which I used in my simulation setup.