# UDF for Specific Heat - Problem

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 April 8, 2013, 13:11 UDF for Specific Heat - Problem #1 New Member   Petter Östlund Join Date: Mar 2013 Posts: 3 Rep Power: 6 Hi all! Im doing simulations with High temperature and pressure differences for argon and have specified UFD's for the density, Cp, Therm. cond. and viscosity using Multiple Regression in Excel (with respect to both Temp. and pressure). Loading the UFD's works great. No error messages. But when i try to choose "user - defined" in the drop down menu for Cp (Specific heat) in the Materials setup i get the error message: "No user defiend functions have been loaded". For all the other material properties: density, therm cond etc. the loaded UDF's pops up and and i can choose anyone of them with no problem. Im using Fluent v. 14.5. The code im using looks something like this: #include "udf.h" #include "math.h" DEFINE_PROPERTY(cp_ar, c,t) { real p_operating_Pa; real p_pressure_Pa; real abs_pressure_Pa; real Temp_K; Temp_K = C_T(c,t)+273; p_pressure_Pa = C_P(c,t); p_operating_Pa = RP_Get_Real("operating-pressure"); abs_pressure_Pa = p_operating_Pa + p_pressure_Pa; cp_ar = 0.25 + 0.00060 * abs_pressure_Pa - 0.0099 * Temp_K; return cp_ar; } Any help would be great. thx.

April 9, 2013, 09:25
#2
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 996
Rep Power: 17
Quote:
 Originally Posted by Hamjaj Hi all! Im doing simulations with High temperature and pressure differences for argon and have specified UFD's for the density, Cp, Therm. cond. and viscosity using Multiple Regression in Excel (with respect to both Temp. and pressure). Loading the UFD's works great. No error messages. But when i try to choose "user - defined" in the drop down menu for Cp (Specific heat) in the Materials setup i get the error message: "No user defiend functions have been loaded". For all the other material properties: density, therm cond etc. the loaded UDF's pops up and and i can choose anyone of them with no problem. Im using Fluent v. 14.5. The code im using looks something like this: #include "udf.h" #include "math.h" DEFINE_PROPERTY(cp_ar, c,t) { real p_operating_Pa; real p_pressure_Pa; real abs_pressure_Pa; real Temp_K; Temp_K = C_T(c,t)+273; p_pressure_Pa = C_P(c,t); p_operating_Pa = RP_Get_Real("operating-pressure"); abs_pressure_Pa = p_operating_Pa + p_pressure_Pa; cp_ar = 0.25 + 0.00060 * abs_pressure_Pa - 0.0099 * Temp_K; return cp_ar; } Any help would be great. thx.
Hi!
For specific heat you cannot use define_property but you must use define_specific_heat; however, I think it is not possibile to define specific heat in terms of pressure.
You can define cp function of temperature, see the following example:

Code:
```#include "udf.h"
DEFINE_SPECIFIC_HEAT(my_user_cp, T, Tref, h, yi)
{
real cp=20.*T;  /*This is only an example of linear cp*/
*h = cp*(T-Tref);
return cp;
}```
Code:
```real T: Temperature for the calculation of the specific heat and enthalpy
real Tref: Reference temperature for the enthalpy calculation
real *h: Pointer to real
real *yi: Pointer to array of mass fractions of gas phase species```
In addition:
why this?
Code:
`Temp_K = C_T(c,t)+273`
C_T(c,t) already returns temperature in K.

Daniele

Last edited by ghost82; April 10, 2013 at 02:39.

 April 10, 2013, 11:48 #3 New Member   Petter Östlund Join Date: Mar 2013 Posts: 3 Rep Power: 6 Thx for ze answer! i think i found a way round the problem. Im currently using the DEFINE_SPECIFIC_HEAT marco but with the same code(ish). But since i cant use the C_P(c,t) in my calculations im only using the operating pressure. I think it still might work since the pressure difference in the domain wont change much form the operating pressuer. (around 1700 bars) Dont know why i hace set the Temp_K=C_T(c,t) + 273..

 April 10, 2013, 12:31 #4 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 996 Rep Power: 17 ok, this is right since you can define through fluent udf only specific heat at constant pressure. Remember to add to your code *h enthalpy calculation. Daniele

 April 18, 2014, 10:19 #5 New Member     m.akbari Join Date: Apr 2014 Posts: 14 Rep Power: 5 hello dear friends, recently i got that for defining the specific heat, we need to use DEFINE_SPECIFIC_HEAT macro and so i did it but im not sure if my udf code is right? can u give me the honor to have a look at it? the code is below and the formula is attached, and just to mention first of all i'd used this code: real temp=C_T(cell,thread) just like other parts and then i deleted it and used the T variable cause i need it in rho_w line, is it the right way? best regards /************************************************** ******************* Fluent UDF Author: Milan all calculations for al2o3 nanoparticles ************************************************** ********************/ #include "udf.h" #define FI 0.01 #define RHO_np 3600 #define SI_1 0.9830 #define SI_2 12.959 #define KTC_np 36 #define TI 5.E4 #define BETA_1 8.4407 #define BETA_2 -1.07304 #define CP_w 4200 #define KA 1.383E-23 #define SIi_1 2.8217E-2 #define SIi_2 3.917E-3 #define SIi_3 -3.0669E-2 #define SIi_4 -3.91123E-3 #define T_0 298.15 #define D_np 59.E-9 #define CP_np 765 DEFINE_PROPERTY(cell_conductivity,cell,thread) { real ktc,ktc_w,temp,f,beta,rho_w; temp = C_T(cell,thread); f = ((SIi_1*FI+SIi_2*temp)/T_0)+(SIi_3*FI+SIi_4); beta = BETA_1*(pow(100*FI,BETA_2)); rho_w = (-3.570*(pow(10,-3))*(pow(temp,2))+(1.88*temp+753.2)); ktc_w = (-8.354*0.000001*(pow(temp,2)))+((6.53*0.001*temp)-0.5981); ktc = ((KTC_np+(2*ktc_w)-2*(ktc_w-KTC_np)*FI)/(KTC_np+(2*ktc_w)+(ktc_w-KTC_np)*FI))+(TI*beta*FI*rho_w*CP_w*(pow(((KA*temp )/(RHO_np*D_np)),0.5))*f); return ktc; } DEFINE_PROPERTY(cell_density,cell,thread) { real temp,rho_w,rho; temp = C_T(cell,thread); rho_w = (-3.570*(pow(10,-3))*(pow(temp,2))+(1.88*temp+753.2)); rho = (FI*RHO_np)+((1-FI)*rho_w); return rho; } DEFINE_PROPERTY(cell_viscosity,cell,thread) { real mu,mu_w,temp; temp = C_T(cell,thread); mu_w = (2.591*(pow(10,-5))*(pow(10,(238.3/(temp-143.2))))); mu = (SI_1*exp(SI_2*FI)*mu_w); return mu; } DEFINE_SPECIFIC_HEAT(specificheat, T, Tref, h, yi) { real cp,rho_w,rho; rho_w = (-3.570*(pow(10,-3))*(pow(T,2))+(1.88*T+753.2)); rho = (FI*RHO_np)+((1-FI)*rho_w); cp = (FI*RHO_np*CP_np)+(((1-FI)*rho_w*CP_w)/rho); return cp; } Last edited by mdakbari; April 18, 2014 at 13:22.

 April 19, 2014, 07:24 #6 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 996 Rep Power: 17 Hi, I think it's ok, test it. From the cp formula I think there is a mistake: cp = (FI*RHO_np*CP_np)+(((1-FI)*rho_w*CP_w)/rho); should be changed to: cp = ((FI*RHO_np*CP_np)+((1-FI)*rho_w*CP_w))/rho; Are you sure you don't need to add enthalpy calculation in the Cp part of code? mdakbari likes this.

April 19, 2014, 12:00
#7
New Member

m.akbari
Join Date: Apr 2014
Posts: 14
Rep Power: 5
Quote:
 Originally Posted by ghost82 Hi, I think it's ok, test it. From the cp formula I think there is a mistake: cp = (FI*RHO_np*CP_np)+(((1-FI)*rho_w*CP_w)/rho); should be changed to: cp = ((FI*RHO_np*CP_np)+((1-FI)*rho_w*CP_w))/rho; Are you sure you don't need to add enthalpy calculation in the Cp part of code?
hi Mr. Daniele, i really appreciate ur help and that u accepted my request to come here and answer my question.

yessss that was the point,small but really important.i modified it and now i can run the calcs without any error or problem, but is there any necessity to add enthalpy equation in this code, since my goal is to calculate cp?
__________________
Best RegarDs

April 20, 2014, 03:59
#8
Senior Member

Daniele
Join Date: Oct 2010
Location: Italy
Posts: 996
Rep Power: 17
Hi,
it depends on the model you use; in anyway I would define it in udf; all you have to do is to integrate the cp to have enthalpy.
Look at the attached picture for the integrals (you have to sum the blue terms) and implement them in your udf.
You can define an arbitrary Tref (reference temperature) in fluent.

Daniele
Attached Images
 enthalpy.jpg (31.0 KB, 98 views)

Last edited by ghost82; April 20, 2014 at 06:04.

 April 20, 2014, 06:02 #9 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 996 Rep Power: 17 Try this and remember to define a reference temperature in fluent, under reference values: Code: ```/********************************************************************* Fluent UDF Author: Milan all calculations for al2o3 nanoparticles **********************************************************************/ #include "udf.h" #include "math.h" #define FI 0.01 #define RHO_np 3600.0 #define SI_1 0.9830 #define SI_2 12.959 #define KTC_np 36.0 #define TI 5.E4 #define BETA_1 8.4407 #define BETA_2 -1.07304 #define CP_w 4200.0 #define KA 1.383E-23 #define SIi_1 2.8217E-2 #define SIi_2 3.917E-3 #define SIi_3 -3.0669E-2 #define SIi_4 -3.91123E-3 #define T_0 298.15 #define D_np 59.E-9 #define CP_np 765.0 DEFINE_PROPERTY(cell_conductivity,cell,thread) { real ktc,ktc_w,temp,f,beta,rho_w; temp = C_T(cell,thread); f = ((SIi_1*FI+SIi_2*temp)/T_0)+(SIi_3*FI+SIi_4); beta = BETA_1*(pow(100*FI,BETA_2)); rho_w = (-3.570*(pow(10,-3))*(pow(temp,2))+(1.88*temp+753.2)); ktc_w = (-8.354*0.000001*(pow(temp,2)))+((6.53*0.001*temp)-0.5981); ktc = ((KTC_np+(2*ktc_w)-2*(ktc_w-KTC_np)*FI)/(KTC_np+(2*ktc_w)+(ktc_w-KTC_np)*FI))+(TI*beta*FI*rho_w*CP_w*(pow(((KA*temp )/(RHO_np*D_np)),0.5))*f); return ktc; } DEFINE_PROPERTY(cell_density,cell,thread) { real temp,rho_w,rho; temp = C_T(cell,thread); rho_w = (-3.570*(pow(10,-3))*(pow(temp,2))+(1.88*temp+753.2)); rho = (FI*RHO_np)+((1-FI)*rho_w); return rho; } DEFINE_PROPERTY(cell_viscosity,cell,thread) { real mu,mu_w,temp; temp = C_T(cell,thread); mu_w = (2.591*(pow(10,-5))*(pow(10,(238.3/(temp-143.2))))); mu = (SI_1*exp(SI_2*FI)*mu_w); return mu; } DEFINE_SPECIFIC_HEAT(specificheat, T, Tref, h, yi) { real cp,rho_w,rho; rho_w = (-3.570*(pow(10,-3))*(pow(T,2))+(1.88*T+753.2)); rho = (FI*RHO_np)+((1-FI)*rho_w); cp = ((FI*RHO_np*CP_np)+((1-FI)*rho_w*CP_w))/rho; *h = -1.0/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5))*(1000.0*FI*CP_np*RHO_np*(atan((0.01*(357.0*Tref*FI-94000.0*FI-357.0*Tref+94000.0))/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5)))-1.0*atan((0.01*(357.0*T*FI-94000.0*FI-357.0*T+94000.0))/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5)))))+1.0/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5))*((1000.0*FI*atan((0.01*(357.0*Tref*FI-94000.0*FI-357.0*Tref+94000.0))/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5)))*RHO_np-1000.0*FI*atan((0.01*(357.0*T*FI-94000.0*FI-357.0*T+94000.0))/(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5)))*RHO_np+(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5))*T-1.0*(pow(3570.0*FI*FI*RHO_np-3.572524*pow(10,6)*FI*FI-3570.0*FI*RHO_np+7.145048*pow(10,6)*FI-3.572524*pow(10,6),0.5))*Tref)*CP_w); return cp; }``` mdakbari likes this.

 April 22, 2014, 02:49 A problem #10 New Member     m.akbari Join Date: Apr 2014 Posts: 14 Rep Power: 5 hello dear daniele thank u for ur help that is really kind of u. but i have some problems: 1- first of all i used my last code(post #7) that needed a correction about parenthesis, without the enthalpy line( u wrote for me), but after running the calcs for a simple tube, and extracted the h diagram in excel, there was an odd diagram about h, it had to be like pic1((attached) for water) but it was very unusual like pic2(attached). 2.when i used the code with ur enthalpy line and interpret it, an error occured about : math.h: No such file or directory any help would be appreciated PIC1-WATER PIC2-NANOFLUID __________________ Best RegarDs

 April 22, 2014, 06:00 #11 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 996 Rep Power: 17 math.h is header necessary for atan (arctan); macro DEFINE_SPECIFIC_HEAT has to be compiled, not interpreted. Daniele

April 22, 2014, 07:51
pordon
#12
New Member

m.akbari
Join Date: Apr 2014
Posts: 14
Rep Power: 5
Quote:
 Originally Posted by ghost82 math.h is header necessary for atan (arctan); macro DEFINE_SPECIFIC_HEAT has to be compiled, not interpreted. Daniele
with interpret i meant the interpret in fluent.but pordon me what do u mean about complie?with what program?
__________________
Best RegarDs

 April 22, 2014, 10:46 #13 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 996 Rep Power: 17 Yes, in fluent you can interpret or compile a udf. To compile a udf you need visual studio installed. Read here for more information: http://www.cfd-online.com/Forums/flu...iled-udfs.html From the wiki, for win 7 64 bit: Code: `How can I manage to compile my UDF with Windows 7 64bit?` Code: ``` Install Visual Studio. Most of the time the Visual C++ 2008 Express Edition [3] is recommended. On my system it even works with the new Visual Studio 2010 Professional Release Candidate [4]. Set the correct environment variables. Browse your way through the Windows system control to 'System'. There you will find a section 'Advanced system settings'. In the following dialog go to the 'Advanced' tabulator and click on 'Environment variables' (lower right corner). Go through the 'System variables' list and search for the 'Path' entry. Add the following to the variable: C:\Program Files (x86)\Microsoft Visual Studio 10.0\Common7\Tools;C:\Program Files (x86)\Microsoft Visual Studio 10.0\VC\bin;C:\Program Files\ANSYS Inc\v120\fluent\ntbin\win64. Adjust this entry to your system concerning the installation directories! The Visual Studio entry should point to the location where 'nmake' is located. Install a Software Development Kit (SKD) for 64bit systems. This may be the difference between 32bit and 64bit systems. I have used the .NET Framework 2.0 Software Development Kit (SDK) (x64) from 2006 [5] because it is explicitly for 64bit systems and I was not sure if more recent versions are for 64bit systems as well. Start FLUENT from the SDK command prompt. Do not use the Visual Studio command prompt, use the SDK command prompt! Go to the directory your case is in and type 'fluent'. ``` mdakbari likes this.

 April 23, 2014, 11:23 ok #14 New Member     m.akbari Join Date: Apr 2014 Posts: 14 Rep Power: 5 Ok dear daniele I'll do that. tnx so much __________________ Best RegarDs

 April 24, 2014, 07:05 #15 Senior Member   François Grégoire Join Date: Jan 2010 Location: Laval University, Canada Posts: 389 Rep Power: 10 Hi, I have Windows 8.1 64 bit and Fluent 14.5.7 64 bit. I installed Microsoft Visual Studio 10 Ultimate and it worked like a charm, didn't even need to modify the environment variable, I just had to start Fluent from one of the 64 bit Visual Studio 10 command prompt and it compiled/loaded (I almost cried).

 February 26, 2016, 06:25 UDF for specific heat of water #16 New Member   Ram Kumar Pal Join Date: Apr 2015 Posts: 22 Rep Power: 4 Dear friends, I have to write udf for specific heat of water as function of temperature. I have written according to DEFINE_PROPERTY macro, but it is not working. Specific heat of water as a function of temperature (in deg Celsius) is as follows: cp = 4.2174356 - 0.0056181625*temp + 0.0012992528*pow(temp,1.5) - 0.00011535353*pow(temp,2.0) + 4.14964*pow(10.0,-6.0)*pow(temp,2.5) I have seen in UDF manual DEFINE_SPECIFIC_HEAT, but don't understand how can I write for above defined function. Please help me. Thanks in advance

 April 4, 2016, 05:01 #17 New Member   Andrew Vella Join Date: Feb 2015 Posts: 12 Rep Power: 4 Hi Daniele, Dear All, I have just compiled the above UDF for the specific heat of Al2O3 nanofluids in FLUENT. The UDF was compiled and the CASE file was initialised with no errors. However, as soon as I initiated the calculations, I was prompted with a solver error due to a diverging temperature. This was not the case with a constant Cp and with the UDFs for density, conductivity and viscosity. Hence, my suspicion is that the cause of this error is Tref. Hence do we need to specify a reference temperature? Thanks in advance!

June 17, 2017, 01:28
#18
Member

NGP
Join Date: Mar 2016
Posts: 31
Rep Power: 3
Quote:
 Originally Posted by ghost82 Hi, it depends on the model you use; in anyway I would define it in udf; all you have to do is to integrate the cp to have enthalpy. Look at the attached picture for the integrals (you have to sum the blue terms) and implement them in your udf. You can define an arbitrary Tref (reference temperature) in fluent. Daniele

Dear Daniele
How this equation for "h" come?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post prince_pahariaa FLUENT 4 July 11, 2011 02:58 h.daniyel FLUENT 5 June 12, 2008 05:06 fea user CFX 0 November 28, 2006 18:39 Carl FLUENT 1 August 5, 2006 19:01 kerem FLUENT 2 June 20, 2006 06:56

All times are GMT -4. The time now is 00:52.

 Contact Us - CFD Online - Top