
[Sponsors] 
December 28, 2010, 17:33 
udf for heat generation rate

#1 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
hi every body
I am supposed to write a udf for heat generation rate which is a cosine function #include"udf.h" DEFINE_SOURCE(energy_source,c,t,ds,eqn) { real x; ds[eqn]=0.3*cos(0.3*x); return sin(0.3*x) ; } but there are some errors! any one can help me to modidfy it. thanks 

December 28, 2010, 19:23 

#2 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
Is "x" in your function the xcoordinate of the cell? If so, try the following unchecked code. Code:
#include "udf.h" #include "math.h" DEFINE_SOURCE(energy_source,c,t,dS,eqn) { real x[ND_ND]; real source; C_CENTROID(x,c,t); source = sin(0.3*x[0]); dS[eqn] = 0.3*cos(0.3*x[0]); return source; } Code:
#include "udf.h" #include "math.h" DEFINE_SOURCE(energy_source,c,t,dS,eqn) { real x[ND_ND]; real source; C_CENTROID(x,c,t); source = 0.3*cos(0.3*x[0]); dS[eqn] = 0.09*sin(0.3*x[0]); return source; } Last edited by ComputerGuy; December 28, 2010 at 19:27. Reason: added additional code 

December 29, 2010, 12:08 

#3 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
ComputerGuy
I am really thankful of you for your response , but X is the height of my geometry (of course its better to use y instead of x , I did mistake to type x!) my geometry its here: Heat generation rate is a cosine function of y (height) : source =5.958*sin(pi *y/11)+1.866 So ds= 5.958*pi /11*cos(pi* y/11) I am grateful if you help me to write a udf for it . Best regards 

December 29, 2010, 12:14 

#4 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
I have given you the code you need to make your function work. Instead of x[0], which returns the "x" component of the geometry, you'll need to use x[1], which returns the "y" component. The only other thing is changing the source=.... and dS[eqn]=.... to the heat generation function and its derivative. ComputerGuy 

December 29, 2010, 13:11 

#5 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear ComputerGuy
I am new in udf so there is some thing that I don't know about them , such as ND could you explain me about ND , why you define x[ND_ND] ? thanks Sarah 

December 29, 2010, 14:25 

#6 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
You should read through the Fluent UDF manual. However, from the Fluent 6.3 UDF manual (Fluent, Inc., September 11, 2006), page 326: "The constant ND_ND is dened as 2 for RP 2D (FLUENT 2D) and RP 3D (FLUENT 3D). It can be used when you want to build a 2 x2 matrix in 2D and a 3 x3 matrix in 3D. When you use ND_ND, your UDF will work for both 2D and 3D cases, without requiring any modications." Thus, when I defined "real x[ND_ND]," I was making x a position vector with dimension ND, where n is the number of dimensions in your simulation. x[0] would be the x component x[1] would be the y component x[2] would be the z component The manual has extremely thorough examples  go through it. ComputerGuy 

December 30, 2010, 11:36 
Hello Computer Guy

#7 
New Member
masters
Join Date: Sep 2010
Posts: 5
Rep Power: 6 
My problem is also related to heat generation in the energy eqn..
In my model Qg(heat generation) is proportional to exponential function of temperature and time gradient of new variable (dC/dt) Initial condition of C is specified i.e t=0,C=0 My aim is to calculate a C at different times.. Is this possible in fluent to include the new variable in the fluent UDF... I have written the UDF for the exponential function of temperature but how to include dc/dt is still a question for me.. 

December 30, 2010, 14:14 

#8 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear ComputerGuy
Yes , you are right , I have read this manual and its so good but there is not any theme about porosity , really in my project I have to define porosity as a function of x and I don’t know how to write a udf for it , everybody who I asked them , say: its impossible or very hard by fluent 6.3.26! Could you help me about this issue ?of course I am really thankful of you for your great help about heat generation rate . Best regards Sarah 

December 30, 2010, 23:49 

#9  
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Manohar,
Is C a scalar? Is it a property of the fluid which travels with the fluid (like species mass fraction, for example)? Or, is it something about the cell which simply changes with time? For example, if you wanted to track the change in temperature in a cell such that you approximate dT/dt (or dC/dt in your case), there are macros which allow you to access the previous time step of a given cell. The previous temperature in a cell may be accessed by: Code:
C_T_M1(c,t); If you can't find your answer there, or if Fluent doesn't automatically track what you're looking for, you could always create a few UserDefined Memory Locations to track values from a previous time step. That is, assume C_UDMI(cell,thread,2) is the current value of C and C_UDMI(cell,thread,1) is the previous value: If you're looking for a "value" or "property" of the fluid which will move with a fluid parcel (advect, diffuse, etc.), look into UserDefined Scalars. If you provide a little more information, especially the functional form of your equation and what you're trying to track (i.e., what is C), perhaps you'll be able to get more help. ComputerGuy Quote:


December 30, 2010, 23:57 

#10  
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
If you can write an equation (or an algorithm) for porosity as a function of geometric position, you can write a UDF for it. It's not that hard. The trick is that as opposed to DEFINE_SOURCE for energy, you must use a DEFINE_PROFILE UDF. Set the region you're interested in to a porous zone, code the DEFINE_PROFILE UDF, compile or interpret the UDF, then load the UDF into the porosity dropdown menu. Let me know if you need further assistance! ComputerGuy Quote:


December 31, 2010, 11:56 
Hello Computer Guy

#11 
New Member
masters
Join Date: Sep 2010
Posts: 5
Rep Power: 6 
My model is related due to absorption(Where gas is getting absorbed by solid).
I am solving energy equation(Unsteady) for the cylindrical model In my model Qg = exp(const/T)*dc/dt (1) where dc/dt = (pg  Peq)/peq*(some constant) (2) where pg =constant= 3 bar peq is a function of Temperature(T). C is concentration of gas in the solid My aim is to find to find T and C for different time. I can substitute (2) eqn in (1) eqn and total heat source will be in function of temperature but finding C by means of temperature will be a long procedure. Is there any way to find both C and T parallel by writing UDF?? 

December 31, 2010, 12:38 

#12 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear ComputerGuy
Thank you It is very kind of you . well I have written an equation for porosity , Its here : Porosity= 0.39*(1+1.05*exp(100*(y1)/0.06)) 1 < y<1.425 Porosity= 0.39*(1+1.05*exp(100*(1.85y)/0.06)) 1.425<y<1.85 y=1 , y=1.85 porosity =0.39 And I have written a udf for it : #include "udf.h" DEFINE_PROFILE(porosity_profile,t,i) { real x[ND_ND]; real y; cell_t c; begin_c_loop(c,t) { y=x[1]; if(1<y<1.425) F_PROFILE(c,t,i)=0.39*(1+1.05*exp(100*(y1)/0.06)); else if(1.425<y<1.85) F_PROFILE(c,t,i)=0.39*(1+1.05*exp(100*(1.85y)/0.06)); } end_c_loop(c,t) } is it corresponding to the equation of porosity? And when we use udf for porosity so we have to write a udf for viscous resistance and inertial resistance as well , so should we interpereted and hook udfs respectively ?, It means we should first hook porosity_udf then viscous resistance_udf and inertial resistance_udf , isn’t it ? I should also thank you since your advices help me in my project so far . Best regards Sarah 

December 31, 2010, 12:41 

#13 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Manohar,
If I understand correctly:
ComputerGuy Last edited by ComputerGuy; January 1, 2011 at 03:03. 

December 31, 2010, 13:05 

#14  
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
Your UDF was basically correct, although didn't address the case where y=1 or y=1.85. You also need to assign a vector to x, which I did with the C_CENTROID command. I've changed it below: Code:
DEFINE_PROFILE(porosity_profile,t,i) { real x[ND_ND]; real y; cell_t c; begin_c_loop(c,t) { C_CENTROID(x,c,t); y=x[1]; if((y==1.)  (y==1.85)) { F_PROFILE(c,t,i)=0.39; } if ((y>1.) && (y<=1.425)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(y1.)/0.06)); } if ((y>1.425) && (y<1.85)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(1.85y)/0.06)); } } end_c_loop(c,t) } Examples 5 and 6 show the usage of both F_PROFILE and C_PROFILE for defining porosity. You can do the same for viscous and inertial resistances, using basically the same code as above, but modified with the appropriate values. ComputerGuy Quote:


December 31, 2010, 14:36 

#15 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear ComputerGuy
Thank you for modification of my code , but now I have faced a funny problem! While I interpreting a udf , previous udf would be removed , for example , in my case ,first I interpreted and hooked udf of energy _source and then udf of porosity but I saw energy_source udf has been removed , what should I do till fluent accepts many udfs not only one . thanks Best regards Sarah 

December 31, 2010, 14:55 

#16 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
Put all the UDF's in the same .c file. For instance: #include "udf.h" DEFINE_SOURCE() {} DEFINE_PROFILE() {} etc.. All of the appropriate functions will be available in the dropdown lists. ComputerGuy 

December 31, 2010, 18:36 

#17 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear ComputerGuy
Thank you so much! , however there is still a question for me , you declared that I use the same code which written for porosity for viscous and inertial resistances , but It is too hard since in my project these are defined as: C1= (Dp^2 *porosity^3)/(150(1porosity)^3) C2=(3.5*(1porosity))/(Dp*porosity^3)) So can I write a udf for them like this: #include "udf.h" DEFINE_PROFILE(inertial_res,t,i) { cell_t c; begin_c_loop(c,t) { F_PROFILE(c,t,i) = 3.5*(1  C_POR(c,t)) /(d_p*pow(C_POR(c,t),3)); } end_c_loop(c,t) } C_POR(c,t) is porosity , so I have to modify porosity code of course I don’t know how do it! Could you help me? Thanks Sarah 

December 31, 2010, 19:52 

#18 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
You need to use a similar format to the porosity function I wrote, not the same one. Short of writing all the UDF's for you, here's what I'd suggest:
Regards, ComputerGuy 

January 1, 2011, 00:03 

#19 
Member
sarah
Join Date: Aug 2010
Posts: 40
Rep Power: 6 
Dear computerGuy
Yes , I am supposed to simulate a packed bed and I’ve read Fluent manual which related to porous media modeling , I ‘ve taken your advices and wrote this code: #define C_UDMI(c,t,0) F_PROFILE(c,t,i) DEFINE_PROFILE(porosity_profile,t,i) { real x[ND_ND]; real y; cell_t c; begin_c_loop(c,t) { C_CENTROID(x,c,t); y=x[1]; if((y==1.)  (y==1.85)) { F_PROFILE(c,t,i)=0.39; } if ((y>1.) && (y<=1.425)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(y1.)/0.06)); } if ((y>1.425) && (y<1.85)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(1.85y)/0.06)); } } end_c_loop(c,t) } // inertial resistance udf . DEFINE_PROFILE(inertial_res,t,i) { cell_t c; begin_c_loop(c,t) { F_PROFILE(c,t,i) = 3.5*(1  C_UDMI(c,t,0)) /(0.06*pow(C_UDMI(c,t,0),3)); } end_c_loop(c,t) } //viscous resistance udf . DEFINE_PROFILE(viscous_res,t,i) { cell_t c; begin_c_loop(c,t) { F_PROFILE(c,t,i) = 150*pow((1  C_UDMI(c,t,0)),2) /(0.0036*pow(C_UDMI(c,t,0),3)); } end_c_loop(c,t) } Is it correct? Of course I could hook it to fluent like porosity code which I had written my self but you modified it , really you suggested to enable a userdefined memory location, why? Best regards Sarah 

January 1, 2011, 00:23 

#20 
Senior Member
Real Name :)
Join Date: Jan 2010
Location: United States
Posts: 180
Rep Power: 7 
Sarah,
I think everything looks right, except for the first line. Try this: Code:
DEFINE_PROFILE(porosity_profile,t,i) { real x[ND_ND]; real y; cell_t c; begin_c_loop(c,t) { C_CENTROID(x,c,t); y=x[1]; if((y==1.)  (y==1.85)) { F_PROFILE(c,t,i)=0.39; } if ((y>1.) && (y<=1.425)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(y1.)/0.06)); } if ((y>1.425) && (y<1.85)) { F_PROFILE(c,t,i)=0.39*(1.+1.05*exp(100.*(1.85y)/0.06)); } C_UDMI(c,t,0)=F_PROFILE(c,t,i); } Let us know if this works for you! ComputerGuy 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
strain rate in UDF  Paulina  FLUENT  11  November 20, 2014 04:06 
UDF to measure Mass Flow Rate  a.lynchy  Fluent UDF and Scheme Programming  21  February 15, 2014 03:18 
UDF for critical strain rate to extinction  Birute Bunkute  FLUENT  1  March 25, 2010 16:40 
surface reaction rate with udf  yellowstuff  FLUENT  4  January 29, 2010 13:53 
heat generation rate w/m3 in 2D  Laszlo  FLUENT  1  May 6, 2004 11:58 