[johnam29]

Hello Everyone!

Background: Running water in co-axial channels into a 2-D domain with temperatures varying from sub- to super-critical using Fluent

Since water has a Cp spike for Super critical water ( as attached in the file).
Cp_NIST_data.JPG

I was looking at trying to model the spike using a UDF with temperature range from 300K to 1000K .I Took data points from the NIST website and generated piece-wise functions for multiple temperature ranges ( as depicted in the code).
Cp_temp_contour.JPG


While I believe the UDF gets loaded properly into fluent( using interpreted , it loads without showing any error), the residuals of continuity tend to blow up ( --> 1e+10 etc) while the energy residual (1e+0) and i get all sorts of temperature spots in the domain(As depicted in the picture).

CODE:

#include "udf.h"

DEFINE_SPECIFIC_HEAT(john_cp, T, Tref, h, yi)

{

real cp;



if (T >= 523 && T <=600)

cp = 6.84697E+04 + -2.41062E+02*T + 2.28273E-01*T*T;



else if (T>600 && T <= 630)

cp = 6.05982E+05 -2.00334E+03*T +1.67297E+00*T*T;



else if (T>630 && T<= 650)

cp =8.91902E+06 -2.81935E+04*T+ 2.23004E+01*T*T;



else if (T>650 && T <= 658)

cp = 3.34752E+08 -1.02965E+06*T+ 7.91808E+02*T*T;



else if (T>658 && T <= 660)

cp = -1.01330E+08+ 3.22934E+05*T-2.56559E+02*T*T;



else if (T>660 && T <= 668)

cp =2.60837E+08 + -7.81911E+05*T+ 5.86025E+02*T*T;



else if (T>668 && T <= 700)

cp = 4.94026E+06 -1.41350E+04*T+ 1.01250E+01*T*T;



else if (T>700 && T <= 850)

cp = 1.18004E+06 -4.36540E+03*T+ 5.40459E+00*T*T -2.23261E-03*T*T*T;

else

cp = 3000;



*h = cp*(T-Tref);

return cp;

}


I was wondering if anyone has faced such an issue.

p.s: I tried to recreate the Cp plot using the functions in MATLab and it seems to recreate them pretty well.

I have also tried with coarse and fine mesh and it still gives me such plots.

Any help or suggestion would be greatly appreciated.



John Misquith

[vinerm]

You don't need a UDF for this. This is just piecewise polynomial, which can be entered directly in GUI.

[johnam29]

Thank you for your reply.

I am currently using piecewise polynomials to capture the curve but since ansys fluent does not allow more than 3 temperature ranges and puts a restriction on the number of significant digits after the decimal point (for the coefficients entered), I cant seem to accurately capture the peak without deviating a lot from the curve.

Hence I decided to move to UDFs. Would love any other suggestions.
Thank you

[vinerm]

If you want to use UDF, you have to compile it. Specific Heat UDF or any UDF that uses references or structures need to be compiled. Interpreter cannot handle this.

[johnam29]

Thanks for your reply again!

Yeah so i tried compiling the code and running it instead of the interpreter. It gave me an 'nmake' error , which i rectified by running fluent through the VS prompt (version 2019).

Even after i was able to compile the code correctly , Im still facing this issue of random temperature spots all over the domain.

Regards
John

[vinerm]

That''s because you have got the Thermodynamics wrong in the UDF. Enthalpy is equal to only for constant . Enthalpy is integral of the specific heat over the temperature range. Therefore, you have to calculate different value of enthalpy for each range and this has to be calculated by integrating the specific heat polynomials over respective ranges. The constants of integration have to be such that the enthalpy values maintain continuity across the entire range.

[johnam29]

Thank you for your reply!

You are absolutely right! Thanks for pointing that out. I made the changes to the code to calculate the enthalpy(h) using the integral from Tref to T and it worked!

Thanks for your help again!

John M

[Danwei]

Hi Johnam,
I meet a problem similar to yours. However, I'm not quite familiar with C language. Could you please specify how to write a code for the integral to calculate enthalpy?
Regards,
Danwei