fluent UDF第四章 DEFINE宏
第四章DEFINE宏
本章介绍了Fluent公司所提供的预定义宏，我们需要用这些预定义宏来定义UDF。在这里这些宏就是指DEFINE宏。
本章由如下几节组成：
? 4.1 概述；4.2 通用解算器DEFINE宏；4.3 模型指定DEFINE宏；4.4 多相DEFINE宏；
? 4.5 离散相模型DEFINE宏
4.1 概述
DEFINE宏一般分为如下四类：通用解算器；模型指定；多相；离散相模型(DPM)
对于本章所列出的每一个DEFINE宏，本章都提供了使用该宏的源代码的例子。很多例子广泛的使用了其它章节讨论的宏，如解算器读取（第五章）和utilities (Chapter 6)。需要注意的是，并不是本章所有的例子都是可以在FLUENT中执行的完整的函数。这些例子只是演示一下如何使用宏。
除了离散相模型DEFINE宏之外的所有宏的定义都包含在udf.h文件中。离散相模型DEFINE宏的定义包含在dpm.h文件中。为了方便大家，所有的定义都列于附录A中。其实udf.h头文件已经包含了dpm.h 文件，所以在你的UDF源代码中就不必包含dpm.h文件了。
注意：在你的源代码中，DEFINE宏的所有参变量必须在同一行，如果将DEFINE声明分为几行就会导致编译错误。
4.2 通用解算器DEFINE宏
本节所介绍的DEFINE宏执行了FLUENT中模型相关的通用解算器函数。表 4.2.1提供了FLUENT 中DEFINE宏，以及这些宏定义的功能和激活这些宏的面板的快速参考向导。每一个DEFINE宏的定义都在udf.h头文件中，具体可以参考附录A。
?DEFINE_ADJUST (4.2.1节)
?DEFINE_INIT (4.2.2节)
?DEFINE_ON_DEMAND (4.2.3节)
?DEFINE_RW_FILE (4.2.4节)
? 4.2.1 DEFINE_ADJUST
? 4.2.2 DEFINE_INIT
? 4.2.3 DEFINE_ON_DEMAND
? 4.2.4 DEFINE_RW_FILE
4.2.1 DEFINE_ADJUST
功能和使用方法的介绍
DEFINE_ADJUST是一个用于调节和修改FLUENT变量的通用宏。例如，你可以用DEFINE_ADJUST 来修改流动变量（如：速度，压力）并计算积分。你可以用它来对某一标量在整个流场上积分，然后在该结果的基础上调节边界条件。在每一步迭代中都可以执行用DEFINE_ADJUST定义的宏，并在解输运方程之前的每一步迭代中调用它。参考图3.3.1 和3.3.2 for可以大致了解一下当DEFINE_ADJUST被调用时FLUENT解的过程
DEFINE_ADJUST有两个参变量：name和d。name是你所指定的UDF的名字。当你的UDF编译并连接时，你的FLUENT图形用户界面就会显示这个名字，此时你就可以选择它了。d是FLUENT解算器传给你的UDF的变量。
D是一个指向区域的指针，调节函数被应用于这个区域上。区域变量提供了存取网格中所有单元和表面的线程。对于多相流，由解算器传给函数的区域指针是混合层区域指针。DEFINE_ADJUST函数不返回任何值给解算器。
例子1
下面的UDF名字是adjust，它使用DEFINE_ADJUST对湍流耗散在整个区域上积分。然后这个值会打印在控制台窗口中。每一步迭代都会调用这个UDF。它可以作为解释程序或者编译后的UDF在FLUENT 中执行。
/*******************************************************************/
/* 积分湍流耗散并将其打印到控制台窗口的UDF */
/********************************************************************/
#include "udf.h"
DEFINE_ADJUST(my_adjust, d)
{
Thread *t;
/* Integrate dissipation. */
real sum_diss=0.;
cell_t c;
thread_loop_c (t,d)
{
begin_c_loop (c,t)
sum_diss += C_D(c,t)*
C_VOLUME(c,t);
end_c_loop (c,t)
}
printf("Volume integral of turbulent dissipation: %g\n", sum_diss);
}
例子：2
下面UDF的名字是adjust_fcn，它用DEFINE_ADJUST指定了某一自定义标量是另一自定义标量的梯度的函数。该函数在每一次迭代中都会被调用。它可以作为编译后的UDF在FLUENT中执行。
/********************************************************************/
/* UDF for defining user-defined scalars and their gradients */
/********************************************************************/
#include "udf.h"
DEFINE_ADJUST(adjust_fcn, d)
{
Thread *t;
cell_t c;
real K_EL = 1.0;
/* Do nothing if gradient isn't allocated yet. */
if (! Data_Valid_P())
return;
thread_loop_c (t, d)
{
if (FLUID_THREAD_P(t))
{
begin_c_loop_all (c,t)
{
C_UDSI(c,t,1) += K_EL*NV_MAG2(C_UDSI_G(c,t,0))*C_VOLUME(c,t);
}
end_c_loop_all (c, t)
}
}
}
Activating an Adjust UDF in FLUENT
在为adjust UDF的源代码进行编译和连接之后，你可以在FLUENT中的User-Defined Function Hooks面板激活这个函数。更详细的内容请参阅8.1.1节。
4.2.2 DEFINE_INIT
功能和使用方法的介绍
你可以用DEFINE_INIT宏来定义一组解的初始值。DEFINE_INIT 完成和修补一样的功能，只是它以另一种方式——UDF来完成。每一次初始化时DEFINE_INIT函数都会被执行一次，并在解算器完成默认的初始化之后立即被调用。因为它是在流场初始化之后被调用的，所以它最常用于设定流动变量的初值。参考图3.3.1和3.3.2关于FLUENT解过程的介绍可以看出什么时候调用DEFINE_INIT函数。
DEFINE_INIT有两个参变量：name和d。name是你所指定的UDF的名字。当你的UDF编译并连接时，你的FLUENT图形用户界面就会显示这个名字，此时你就可以选择它了。d是FLUENT解算器传给你的UDF的变量。
d is a pointer to th
e domain over which the initialization function is to be applied. The domain argument provides access to all cell and face threads in the mesh. For multiphase flows, the domain pointer that is passed to the function by the solver is the mixture-level domain pointer. A DEFINE_INIT function does not return a value to the solver.
例子
下面的UDF名字是my_init_func，它在某一个解中初始化了流动变量。在解过程开始时它被执行了一次。它可以作为解释程序或者编译后的UDF在FLUENT中执行。
/*******************************************************************/
/* UDF for initializing flow field variables */
/***********************************************************************/
#include "udf.h"
DEFINE_INIT(my_init_function, domain)
{
cell_t c;
Thread *t;
real xc[ND_ND];
/* loop over all cell threads in the domain */
thread_loop_c (t,domain)
{
/* loop over all cells */
begin_c_loop_all (c,t)
{
C_CENTROID(xc,c,t);
if (sqrt(ND_SUM(pow(xc[0] - 0.5,2.),
pow(xc[1] - 0.5,2.),
pow(xc[2] - 0.5,2.))) < 0.25)
C_T(c,t) = 400.;
else
C_T(c,t) = 300.;
}
end_c_loop_all (c,t)
}
}
The macro ND_SUM(a, b, c) that is used in the UDF computes the sum of the first two arguments (2D) or all three arguments (3D). It is useful for writing functions involving vector operations so that the same function can be used for 2D and 3D. For a 2D case, the third argument is ignored. See Chapter 5 for a description of predefined solver access macros (e.g., C_CENTROID) and Chapter 6 for utility macros (e.g., ND_SUM).
Activating an Initialization UDF in FLUENT
编译并连接UDF源代码之后。you can activate the function in the User-Defined Function Hooks panel in FLUENT. See Section 8.1.2 for more details.
4.2.3 DEFINE_ON_DEMAND
功能和使用方法的介绍
你可以使用DEFINE_ON_DEMAND macro to define a UDF to execute on demand in FLUENT, rather than having FLUENT call it automatically during the calculation. Your UDF will be executed immediately, once it is activated, but it is not accessible while the solver is iterating. Note that the domain pointer d is not explicitly passed as an argument to DEFINE_ON_DEMAND. Therefore, if you want to use the domain variable in your on-demand function, you will need to first retrieve it using the Get_Domain utility provided by Fluent (shown in 例子：below). See Section 6.5.1 for details on Get_Domain.
There is only one argument to DEFINE_ON_DEMAND: name. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可被选择。 A DEFINE_ON_DEMAND function does not return a value to the solver.
例子：
下面的UDF名字为demand_calc，计算并打印出当前数据场的最小、最大和平均温度。It then computes a temperature function
and stores it in user-defined memory location 0 (which is allocated as described in Section 6.7). Once you execute the UDF (as described in Section 8.1.3), the field values for f( T) will be available in the drop-down lists in postprocessing panels in FLUENT. You can select this field by choosing udm-0 in the User Defined Memory... category. If you write a data file after executing the UDF, the user-defined memory field will be saved to the data file. The UDF can be executed as an interpreted or compiled UDF in FLUENT.
/**********************************************************************/
/* UDF to calculate temperature field function and store in */
/* user-defined memory. Also print min, max, avg temperatures. */
/**********************************************************************/
#include "udf.h"
DEFINE_ON_DEMAND(on_demand_calc)
Domain *d; /* declare domain pointer since it is not passed a */
/* argument to DEFINE macro */
{
real tavg = 0.;
real tmax = 0.;
real tmin = 0.;
real temp,volume,vol_tot;
Thread *t;
cell_t c;
d = Get_Domain(1); /* Get th
e domain using Fluent utility */
/* Loop over all cell threads in the domain */
thread_loop_c(t,d)
{
/* Compute max, min, volume-averaged temperature */
/* Loop over all cells */
begin_c_loop(c,t)
{
volume = C_VOLUME(c,t); /* get cell volume */
temp = C_T(c,t); /* get cell temperature */
if (temp < tmin || tmin == 0.) tmin = temp;
if (temp > tmax || tmax == 0.) tmax = temp;
vol_tot += volume;
tavg += temp*volume;
}
end_c_loop(c,t)
tavg /= vol_tot;
printf("\n Tmin = %g Tmax = %g Tavg = %g\n",tmin,tmax,tavg);
/* Compute temperature function and store in user-defined memory*/
/*(location index 0) */
begin_c_loop(c,t)
{
temp = C_T(c,t);
C_UDMI(c,t,0) = (temp-tmin)/(tmax-tmin);
}
end_c_loop(c,t)
}
}
Get_Domain is a macro that retrieves the pointer to a domain. It is necessary to get the domain pointer using this macro since it is not explicitly passed as an argument to DEFINE_ON_DEMAND. The function, named on_demand_calc, does not take any explicit arguments. Within the function body, the variables that are to be used by the function are defined and initialized first. Following the variable declarations, a looping macro is used to loop over each cell thread in the domain. Within that loop another loop is used to loop over all the cells. Within the inner loop, the total volume and the minimum, maximum, and volume-averaged temperature are computed. These computed values are printed to the FLUENT console. Then a second loop over each cell is used to compute the function f( T) and store it in user-defined memory location 0. Refer to Chapter 5 for a description of predefined solver access macros (e.g., C_T) and Chapter 6 for utility macros (e.g., begin_c_loop).
Activating an On-Demand UDF in FLUENT
After you have compiled and linked the source code for your on-demand UDF, you can activate the function in the Execute On Demand panel in FLUENT. See Section 8.1.3 for more details.
4.2.4 DEFINE_RW_FILE
功能和使用方法的介绍
你可以使用DEFINE_RW_FILE macro to define customized information that you want to be written to a case or data file, or read from a case or data file. You can save and restore custom variables of any data types (e.g., integer, real, Boolean, structure) using DEFINE_RW_FILE. It is often useful to save dynamic information (e.g., number of occurrences in conditional sampling) while your solution is being calculated, which is another use of this function. Note that the read order and the write order must be the same when you use this function.
There are two arguments to DEFINE_RW_FILE: name and fp. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可被选择。fp is a variable that is passed by the FLUENT solver to your UDF.
fp is a pointer to the file to or from which you are writing or reading. A DEFINE_RW_FILE function does not return a value to the solver.
!! Do not use the fwrite macro in DEFINE_RW_FILE functions that are running on Windows platforms. Use fprintf instead.
例子：
The following C source code contains 例子：s of functions that write information to a data file and read it back. These functions are concatenated into a single file that can be executed as interpreted or compiled in FLUENT. /***********************************************************************/
/* UDFs that increment a variable, write it to a data file */
/* and read it back in */
/***********************************************************************/
#include "udf.h"
int kount = 0; /* define global variable kount */
DEFINE_ADJUST(demo_calc, domain)
{
kount++;
printf("kount = %d\n",kount);
}
DEFINE_RW_FILE(writer, fp)
{
printf("Writing UDF data to data file...\n");
fprintf(fp, "%d",kount); /* write out kount to data file */
}
DEFINE_RW_FILE(reader, fp)
{
printf("Reading UDF data from data file...\n");
fscanf(fp, "%d",&kount); /* read kount from data file */
}
At the top of the listing, the integer kount is defined and initialized to zero. The first function ( demo_calc)ltindexdemo_calc is an ADJUST function that increments the value of kount at each iteration, since the ADJUST function is called once per iteration. (See Section 4.2.1 for more information about ADJUST functions.) The second function ( writer) instructs FLUENT to write the current value of kount to the
data file, when the data file is saved. The third function ( reader) instructs FLUENT to read the value of kount from the data file, when the data file is read.
The functions work together as follows. If you run your calculation for, say, 10 iterations ( kount has been incremented to a value of 10) and save the data file, then the current value of kount (10) will be written to your data file. If you read the data back into FLUENT and continue the calculation, kount will start at a value of 10 and will be incremented at each iteration. Note that you can save as many static variables as you want, but you must be sure to read them in the same order in which they are written.
Activating a Read/Write Case or Data File UDF in FLUENT
After you have compiled and linked the source code for your read/write UDF, you can activate the function in the User-Defined Function Hooks panel in FLUENT. See Section 8.1.4 for more details.
4.3 模型指定DEFINE宏
本节所介绍的DEFINE宏用于set parameters for a particular model in FLUENT. Table 4.3.1 provides a quick reference guide to the DEFINE macros, the functions they are used to define, and the panel where they are activated in FLUENT. Definitions of each DEFINE macro are listed in the udf.h header file. For your convenience, the definitions are also provided in Appendix A.
?DEFINE_DELTAT (Section 4.3.1)
?DEFINE_DIFFUSIVITY (Section 4.3.2)
?DEFINE_HEAT_FLUX (Section 4.3.3)
?DEFINE_NOX_RATE (Section 4.3.4)
?DEFINE_PROFILE (Section 4.3.5)
?DEFINE_PROPERTY(Section 4.3.6)
?DEFINE_SCAT_PHASE_FUNC (Section 4.3.7)
?DEFINE_SOURCE (Section 4.3.8)
?DEFINE_SR_RATE (Section 4.3.9)
?DEFINE_TURB_PREMIX_SOURCE (Section 4.3.10)
?DEFINE_TURBULENT_VISCOSITY (Section 4.3.11)
?DEFINE_UDS_FLUX (Section 4.3.12)
?DEFINE_UDS_UNSTEADY (Section 4.3.13)
?DEFINE_VR_RATE (Section 4.3.14)
? 4.3.1 DEFINE_DELTAT
? 4.3.2 DEFINE_DIFFUSIVITY
? 4.3.3 DEFINE_HEAT_FLUX
? 4.3.4 DEFINE_NOX_RATE
? 4.3.5 DEFINE_PROFILE
? 4.3.6 DEFINE_PROPERTY
? 4.3.7 DEFINE_SCAT_PHASE_FUNC
? 4.3.8 DEFINE_SOURCE
? 4.3.9 DEFINE_SR_RATE
? 4.3.10 DEFINE_TURB_PREMIX_SOURCE
? 4.3.11 DEFINE_TURBULENT_VISCOSITY
? 4.3.12 DEFINE_UDS_FLUX
? 4.3.13 DEFINE_UDS_UNSTEADY
? 4.3.14 DEFINE_VR_RATE
4.3.1 DEFINE_DELTAT
功能和使用方法的介绍
你可以使用DEFINE_DELTAT宏来控制时间相关问题解的时间步长。This macro can only be used if the adaptive time-stepping method option has been activated in the Iterate panel in FLUENT.
There are two arguments to DEFINE_DELTAT: name and domain. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可
被选择。domain is passed by the FLUENT solver to your UDF. Your UDF will need to return the real value of the physical time step to the solver.
例子：
下面的UDF名字为mydeltat, is a simple function that shows how you can use DEFINE_DELTAT to change the value of the time step in a simulation. First, RP_Get_Real is used to get the value of the current simulation time ( flow_time). Then, for the first 0.5 seconds of the calculation, a time step of 0.1 is set. A time step of 0.2 is set for the remainder of the simulation. The time step variable is then returned to the solver. See Section 6.9 for details on RP_Get_Real.
/***********************************************************************/
/* UDF that changes the time step value for a time-dependent solution */
/***********************************************************************/
#include "udf.h"
DEFINE_DELTAT(mydeltat, domain)
{
real time_step;
real flow_time = RP_Get_Real("flow-time");
if (flow_time < 0.5)
time_step = 0.1;
else
time_step = 0.2;
return time_step;
}
Activating an Adaptive Time Step UDF in FLUENT
Once you have compiled and linked the source code for an adaptive time step UDF, you can activate it in the Iterate panel in FLUENT. See Section 8.2.8 for more details.
4.3.2 DEFINE_DIFFUSIVITY
功能和使用方法的介绍
你可以使用DEFINE_DIFFUSIVITY macro to specify the diffusivity for the species transport equations or user-defined scalar (UDS) transport equations.
There are four arguments to DEFINE_DIFFUSIVITY: name, c, and t, and i. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可被选择。c, t, and i are variables that are passed by the FLUENT solver to your UDF.
c is an index that identifies a cell within the given thread. t is a pointer to the threa
d on which th
e diffusivity function is to be applied. i is an index that identifies the species or user-defined scalar. Your UDF will need to return the real value o
f diffusivity to the solver.
Note that diffusivity UDFs (defined using DEFINE_DIFFUSIVITY) are called by FLUENT from within a loop on cell threads. Consequently, your UDF will not need to loop over cells in a thread since FLUENT is doing it outside of the function call. Your UDF will be required to compute the diffusivity only for a single cell and return the real value to the solver.
例子：
下面的UDF名字为mean_age_diff, computes the diffusivity for the mean age of air using a user-defined scalar. Note that the mean age of air calculations do not require that energy, radiation, or species transport calculations have been performed. You will need to set uds-0 = 0.0 at all inlets and outlets in your model. This function can be executed as an interpreted or compiled UDF.
/**********************************************************************/
/* UDF that computes diffusivity for mean age using a user-defined */
/* scalar. */
/**********************************************************************/
#include "udf.h"
DEFINE_DIFFUSIVITY(mean_age_diff, c, t, i)
{
return C_R(c,t) * 2.88e-05 + C_MU_EFF(c,t) / 0.7;
}
Activating a Diffusivity UDF in FLUENT
Once you have compiled and linked your diffusivity UDF, you can activate it by selecting it as the mass or UDS diffusivity in the Materials panel in FLUENT. See Section 8.2.4 for more details.
4.3.3 DEFINE_HEAT_FLUX
功能和使用方法的介绍
In spite of its name, the DEFINE_HEAT_FLUX macro is not to be used to explicitly set the heat flux along a wall. FLUENT computes the heat flux along a wall based on currently selected models to account for the diffusive and radiative energy fluxes (if any). You must only use a DEFINE_HEAT_FLUX UDF when you want to employ some other heat transfer mechanism that is not currently being modeled. The total heat flux at the wall will be the sum of the currently computed heat flux (based on the activated models) and the heat flux defined by the UDF.
There are seven arguments to DEFINE_HEAT_FLUX: name, f, t, c0, t0, cid, and cir. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可被选择。f, t, c0, t0, cir[], and cid[] are variables that are passed by the FLUENT solver to your UDF.
f is an index that identifies a wall face within the given thread. t is a pointer to the thread on which the heat flux function is to be applied. c0 is an index that identifies the cell next to the wall, and t0 is a pointer to the adjacent cell's thread.
cid[] and cir[] are real arrays that need to be computed by your UDF. Array cid[] stores the fluid-side diffusive heat transfer coefficients, while array cir[] stores radiative heat transfer coefficients. With these inputs provided to the function, the diffusive heat flux ( qid) and radiative heat flux ( qir) are computed by FLUENT according to the following equations:
qid = cid[0] + cid[1]*C_T(c0,t0) - cid[2]*F_T(f,t) - cid[3]*pow(F_T(f,t),4)
qir = cir[0] + cir[1]*C_T(c0,t0) - cir[2]*F_T(f,t) - cir[3]*pow(F_T(f,t),4)
The sum of qid and qir defines the total heat flux from the fluid to the wall (this direction being positive flux), and, from an energy balance at the wall, equals the heat flux of the surroundings (exterior to the domain). Note that heat flux UDFs (defined using DEFINE_HEAT_FLUX) are called by FLUENT from within a loop over wall faces.
!! In order for the solver to compute C_T and F_T, the values you supply to cid[1] and cid[2] should never be zero.
例子：
Section 10.5.2 provides an 例子：of the P-1 radiation model implementation through a user-defined scalar. An 例子：of the usage of the DEFINE_HEAT_FLUX macro is included in that implementation.
Activating a Heat Flux UDF in FLUENT
Once you have compiled and linked your heat flux UDF, you can activate it by selecting it in the User-Defined Function Hooks panel in FLUENT. See Section 8.2.2 for more details.
4.3.4 DEFINE_NOX_RATE
功能和使用方法的介绍
你可以使用DEFINE_NOX_RATE macro to calculate NOx production and reduction rates in FLUENT . The UDF rate that you specify is independent of the standard NOx model options. You can deselect the standard NOx options in your simulation, and choose the UDF rate instead.
There are four arguments to DEFINE_NOX_RATE: name, c, t, and NOx. name is the name of the UDF, specified by you. 当你的UDF 编译和连接时，你为函数所选择的名字会在FLUENT 图形用户界面中变得可见，且可被选择。 c, t, and NOx are variables that are passed by the FLUENT solver to your UDF. c is an index that identifies a cell within the given thread. t is a pointer to the thread on which the NOx rate is to be applied. NOx is a pointer to the NOx structure. A DEFINE_NOX_RATE function does not return a value. The calculated NOx rates are returned through the NOx structure.
Note that, although the data structure is called NOx, the DEFINE_NOX_RATE macro can be used to calculate the rates of any of the pollutant species (i.e., NO, HCN, and NH 3), depending on which of the pollutant species equations is being solved. 例子：
下面编译的UDF 名字为user_nox, computes NOx production and reduction rates based on the forward and reverse rates of NO defined as
(4.3.1)
and
(4.3.2)
where the rate coefficients, which have units of m 3/mol-s, are defined as k 1
=
(4.3.3)
k-1
= (4.3.4) k2
= (4.3.5) k-2
= (4.3.6)
O concentration is given by
= (4.3.7)
All concentrations in the rate expressions have units of mol/mol 3.
/************************************************************/
/* UDF 例子：of User-Defined NOx Rate */
/************************************************************/
#include "udf.h"
#define SMALL_S 1.e-29
DEFINE_NOX_RATE(user_nox, c, t, NOx)
{
real kf1, kr1, kf2, kr2;
real o_eq;
real s1, s2, s3, rf, rr;
Rate_Const K_F[2] = {{1.80e8, 0.0, 38370.0},
{1.80e4, 1.0, 4680.0}};
Rate_Const K_R[2] = {{3.80e7, 0.0, 425.0},
{3.80e3, 1.0, 20820.0}};
Rate_Const K_O = {3.664e1, 0.5, 27123.0};
if (NOX_EQN(NOx) != EQ_NO) return;
kf1 = ARRH(NOx, K_F[0]);
kr1 = ARRH(NOx, K_R[0]);
kf2 = ARRH(NOx, K_F[1]);
kr2 = ARRH(NOx, K_R[1]);
s1 = kf2*MOLECON(NOx, O2);
s3 = s1 + kr1*MOLECON(NOx, NO);
/* determine O concentration (partial equilibrium)*/
o_eq = ARRH(NOx, K_O)*sqrt(MOLECON(NOx, O2));
/* calculate NO rate */
s2 = 2.*o_eq;
/* forward rate... */
rf = s2*(kf1*MOLECON(NOx, N2))*s1/s3;
/* reverse rate... */
rr = -s2*kr1*kr2*pow(MOLECON(NOx, NO), 2.0)/s3;
/* rates have units mole/m^3/s */
NOX_FRATE(NOx) = rf;
NOX_RRATE(NOx) = rr;
}
A number of Fluent-provided macros can be used in the calculation of pollutant rate using user-defined functions. The macros listed below are defined in the header file sg_nox.h which is included in the udf.h file. The variable NOx indicates a pointer to the NOx_Parameter structure.
?NOX_EQN(NOx) returns the index of the pollutant equation currently being solved. The indices are EQ_NO for NO, EQ_HCN for HCN, and EQ_NH3 for NH 3.
?MOLECON(NOx, SPE) returns the molar concentration of a species specified by SPE, which must be replaced by one of the following identifiers: FUEL, O 2, O, OH, H 2O, N 2, N, CH, CH 2, CH 3, NO, HCN, NH 3. Identifier FUEL represents the fuel species as specified in the Fuel Species drop-down list under Prompt NO Parameters in the NOx Model panel.
?NULLIDX(NOx, SPE) returns TRUE if the species specified by SPE does not exist in the FLUENT case (i.e., in the Species panel).
?ARRH(NOx, K) returns the Arrhenius rate calculated from the constants specified by K. K is defined using the Rate_Const data type and has three elements - A, B, and C. The Arrhenius rate is given in the form of
where T is the temperature.
?NOX_FRATE(NOx) is used to return the production rate of the pollutant species being solved.
?NOX_RRATE(NOx) is used to return the reduction rate of the pollutant species being solved. Activating a NOx Rate UDF in FLUENT
Once you have compiled and linked your NOx rate UDF, you can activate it by selecting it in the NOx Model panel in FLUENT. See Section 8.2.3 for more details.
4.3.5 DEFINE_PROFILE
功能和使用方法的介绍
你可以使用DEFINE_PROFILE macro to define a custom boundary profile that varies as a function of spatial coordinates or time. Some of the variables you can customize at a boundary are
?velocity, pressure, temperature, turbulent kinetic energy, turbulent dissipation rate
?volume fraction (multiphase)
?species mass fraction (species transport)
?wall thermal conditions
?wall stress conditions
There are three arguments to DEFINE_PROFILE: name, t, and i. name is the name of the UDF, specified by you. 当你的UDF编译和连接时，你为函数所选择的名字会在FLUENT图形用户界面中变得可见，且可被选择。t and i are variables that are passed by the FLUENT solver to your UDF.
t is a pointer to the thread on which the boundary condition is to be applied. i is an index that identifies the variable that is to be defined. i is set when you associate (hook) the UDF with a variable in a boundary condition panel through the graphical user interface. This index is subsequently passed to your UDF by the FLUENT solver, so that your function knows which variable to operate on.
While DEFINE_PROFILE is usually used to specify a profile condition on a boundary face zone, it can also be used to specify, or fix, flow variables that are held constant during computation in a cell zone. See Section 6.26 of the User's Guide for more information on fixing values in a cell zone boundary condition. The arguments of the macro will change accordingly. There are three arguments to DEFINE_PROFILE for a cell zone: name, thread, and np. name is the name of the UDF, specified by you. thread and np are variables that are passed by the FLUENT solver to your UDF.
Note that unlike source term and property UDFs, profile UDFs (defined using DEFINE_PROFILE) are not called by FLUENT from within a loop on threads in the boundary zone. The solver only passes the DEFINE_PROFILE macro the pointer to the thread associated with the boundary zone. Your UDF will need to do the work of looping over all of the faces in the thread, compute the face value for the boundary variable, and then store the value in memory. Fluent has provided you with a face looping macro to loop over all faces in a thread ( begin_f_loop...). See Chapter 6 for details about face looping macro utilities.
F_PROFILE is typically used along with DEFINE_PROFILE, and is a predefined macro provided by Fluent. F_PROFILE stores a boundary condition in memory for a given face and index and is nested within the face loop in the 例子：s below. It is important to note that the index i that is an argument to DEFINE_PROFILE is the same argument to F_PROFILE. F_PROFILE uses the thread pointer t, face identifier f, and index i to set the appropriate boundary face value in memory. See Section 6.4 for a description of F_PROFILE.
例子：1
下面的UDF名字为pressure_profile, generates a parabolic pressure profile according to the equation
Note that this UDF assumes that the grid is generated such that the origin is at the geometric center of the
boundary zone to which the UDF is to be applied. y is 0.0 at the center of the inlet and extends to at the top and bottom of the inlet. This function can be executed as an interpreted or compiled UDF in FLUENT.
/***********************************************************************/
/* UDF for specifying steady-state parabolic pressure profile boundary */
/* profile for a turbine vane */
/***********************************************************************/
#include "udf.h"
DEFINE_PROFILE(pressure_profile, t, i)
{
real x[ND_ND]; /* this will hold the position vector */
real y;
face_t f;
begin_f_loop(f, t)
{
F_CENTROID(x,f,t);
y = x[1];
F_PROFILE(f, t, i) = 1.1e5 - y*y/(.0745*.0745)*0.1e5;
}
end_f_loop(f, t)
}
The function named pressure_profile has two arguments: t and i. t is a pointer to the face's thread, and i is an integer that is a numerical label for the variable being set within each loop.
Within the function body, variable f is declared as a face. A one-dimensional array x and variable y are declared as real data types. Following the variable declarations, a looping macro is used to loop over each face in the zone to create a profile, or an array of data. Within each loop, F_CENTROID returns the value of the face centroid (array x) for the face with index f that is on the thread pointed to by t. The y coordinate stored in x[1] is assigned to variable y, and is then used to calculate the pressure. This value is then assigned to F_PROFILE, which uses the integer i (passed to it by the solver, based on your selection of the UDF as the boundary condition for pressure in the Pressure Inlet panel) to set the pressure face value in memory.
例子：2
在下面的例子中，：, DEFINE_PROFILE is used to generate profiles for the x velocity, turbulent kinetic energy, and dissipation rate, respectively, for a 2D fully-developed duct flow. Three separate UDFs named x_velocity, k_profile, and dissip_profile are defined. These functions are concatenated in a single C source file which can be executed as interpreted or compiled in FLUENT.
The 1/7th power law is used to specify the x velocity component:
A fully-developed profile occurs when is one-half the duct height. In this 例子：, the mean x velocity is prescribed and the peak (free-stream) velocity is determined by averaging across the channel.
The turbulent kinetic energy is assumed to vary linearly from a near-wall value of
to a free-stream value of
The dissipation rate is given by
where the mixing length is the minimum of and 0.085 . ( is the von Karman constant = 0.41.)
The friction velocity and wall shear take the forms
The friction factor is estimated from the Blasius equation: