CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Divergence using UDF for specific Heat(Fluent)

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

Like Tree1Likes
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 3, 2020, 13:28
Default Divergence using UDF for specific Heat(Fluent)
  #1
New Member
 
John Antony Misquith
Join Date: Feb 2020
Posts: 4
Rep Power: 2
johnam29 is on a distinguished road
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
johnam29 is offline   Reply With Quote

Old   June 3, 2020, 14:26
Default Specific Heat
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
You don't need a UDF for this. This is just piecewise polynomial, which can be entered directly in GUI.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   June 3, 2020, 15:28
Default
  #3
New Member
 
John Antony Misquith
Join Date: Feb 2020
Posts: 4
Rep Power: 2
johnam29 is on a distinguished road
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
johnam29 is offline   Reply With Quote

Old   June 3, 2020, 15:44
Default Udf
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
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.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   June 4, 2020, 02:15
Default
  #5
New Member
 
John Antony Misquith
Join Date: Feb 2020
Posts: 4
Rep Power: 2
johnam29 is on a distinguished road
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
johnam29 is offline   Reply With Quote

Old   June 4, 2020, 03:28
Default Specific Heat and Enthalpy
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,948
Blog Entries: 1
Rep Power: 31
vinerm will become famous soon enough
That''s because you have got the Thermodynamics wrong in the UDF. Enthalpy is equal to C_p(T-T_{ref}) only for constant C_p. 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 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   June 11, 2020, 19:19
Default
  #7
New Member
 
John Antony Misquith
Join Date: Feb 2020
Posts: 4
Rep Power: 2
johnam29 is on a distinguished road
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
johnam29 is offline   Reply With Quote

Old   July 8, 2020, 11:10
Default
  #8
New Member
 
Join Date: Jul 2020
Posts: 1
Rep Power: 0
Danwei is on a distinguished road
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
Danwei is offline   Reply With Quote

Reply

Tags
fluent - udf - parallel, specific heat, supercritical water

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PEMFC model with FLUENT brahimchoice FLUENT 22 April 19, 2020 15:44
Two Phase Flow In Vertical Pipe stonepreston FLUENT 2 October 31, 2017 08:35
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
UDF for heat convection coefficient with fixed surface temperature Boo85 Fluent UDF and Scheme Programming 2 July 10, 2012 18:43
heat flow UDF on coupled surface (wall-shadow wall) Friedmann Fluent UDF and Scheme Programming 0 August 5, 2010 10:25


All times are GMT -4. The time now is 10:33.