To begin the process, you’ll need to define the problem you want to solve using a UDF (Step 1). For example, suppose you want to use a UDF to define a custom boundary profile for your model. You will first need to define the set of mathematical equations that describes the profile.

Next you will need to translate the mathematical equation (conceptual design) into a function written in the C programming language (Step 2). You can do this using any text editor. Save the file with a .c suffix (for example, udfexample.c) in your working folder. (See Appendix A: C Programming Basics for some basic information on C programming.)

After you have written the C function, you are ready to start Ansys Fluent and read in (or set up) your case file (Step 3). You will then need to interpret or compile the source code, debug it (Step 4), and then hook the function to Ansys Fluent (Step 5). Finally you’ll run the calculation (Step 6), analyze the results from your simulation, and compare them to expected results (Step 7). You may loop through this entire process more than once, depending on the results of your analysis. Follow the step-by-step process in the sections below to see how this is done.

The first step in creating a UDF and using it in your Ansys Fluent model involves defining your model equation(s).

Consider the elbow duct illustrated in Figure 8.1: The Mesh for the Elbow Duct Example. The domain has a velocity inlet on the left side, and a pressure outlet at the top of the right side.

Figure 8.1: The Mesh for the Elbow Duct Example

A flow field in which a constant x velocity is applied at the inlet will be compared with one where a parabolic x velocity profile is applied. The results of a constant velocity (of 0.1 m/s) at the inlet are shown in Figure 8.2: Velocity Magnitude Contours for a Constant Inlet x Velocity and Figure 8.3: Velocity Vectors for a Constant Inlet x Velocity.

Figure 8.2: Velocity Magnitude Contours for a Constant Inlet x Velocity

Figure 8.3: Velocity Vectors for a Constant Inlet x Velocity

Now suppose that you want to impose a non-uniform x velocity to the duct inlet, which has a parabolic shape. The velocity is 0 m/s at the walls of the inlet and 0.1 m/s at the center.

To solve this type of problem, you can write a custom profile UDF and apply it to your Ansys Fluent model.

Now that you have determined the shape of the velocity profile that defines the UDF, you can use any text editor to create a file containing C code that implements the function. Save the source code file with a .c extension (for example, udfexample.c) in your working folder. The following UDF source code listing contains only a single function. Your source file can contain multiple concatenated functions. (Refer to Appendix A: C Programming Basics for basic information on C programming.)

Below is an example of how the profile described in Step 1 can be implemented in a UDF. The functionality of the UDF is designated by the leading DEFINE macro. Here, the DEFINE_PROFILE macro is used to indicate to the solver that the code that follows will provide profile information at boundaries. Other DEFINE macros will be discussed later in this manual. (See DEFINE Macros for details about DEFINE macro usage.)

/***********************************************************************
   udfexample.c 
  UDF for specifying steady-state velocity profile boundary condition
 ************************************************************************/
 
 #include "udf.h"
 
 DEFINE_PROFILE(inlet_x_velocity, thread, position)
 {
    real x[ND_ND]; /* this will hold the position vector */
    real y, h;
    face_t f;
    h = 0.016; /* inlet height in m */
    begin_f_loop(f,thread)
    {
      F_CENTROID(x, f, thread);
      y = 2.*(x[1]-0.5*h)/h; /* non-dimensional y coordinate */
      F_PROFILE(f, thread, position) = 0.1*(1.0-y*y);
    }
    end_f_loop(f, thread)
 
 }

The first argument of the DEFINE_PROFILE macro, inlet_x_velocity, is the name of the UDF that you supply. The name will appear in the boundary condition dialog box after the function is interpreted or compiled, enabling you to hook the function to your model. Note that the UDF name you supply cannot contain a number as the first character. The equation that is defined by the function will be applied to all cell faces (identified by f in the face loop) on a given boundary zone (identified by thread). The thread is defined automatically when you hook the UDF to a particular boundary in the Ansys Fluent GUI. The index is defined automatically through the begin_f_loop utility. In this UDF, the begin_f_loop macro (Looping Macros) is used to loop through all cell faces in the boundary zone. For each face, the coordinates of the face centroid are accessed by F_CENTROID (Face Centroid (F_CENTROID)). The coordinate y is used in the parabolic profile equation and the returned velocity is assigned to the face through F_PROFILE. begin_f_loop and F_PROFILE (Set Boundary Condition Value (F_PROFILE)) are Ansys Fluent-supplied macros. Refer to Additional Macros for Writing UDFs for details on how to utilize predefined macros and functions supplied by Ansys Fluent to access Ansys Fluent solver data and perform other tasks.

After you have created the source code for your UDF, you are ready to begin the problem setup in Ansys Fluent.

You are now ready to interpret or compile the profile UDF (named inlet_x_velocity) that you created in Step 2 and that is contained within the source file named udfexample.c. In general, you must compile your function as a compiled UDF if the source code contains structured reference calls or other elements of C that are not handled by the Ansys Fluent interpreter. To determine whether you should compile or interpret your UDF, see Differences Between Interpreted and Compiled UDFs.

Now that you have interpreted or compiled your UDF following the methods outlined in Step 4, you are ready to hook the profile UDF in this sample problem to the Velocity Inlet boundary condition dialog box (see Hooking UDFs to Ansys Fluent for details on how to hook UDFs). First, click the Momentum tab in the Velocity Inlet dialog box (Figure 8.8: The Velocity Inlet Dialog Box) and then choose the name of the UDF that was given in our sample problem with udf preceding it (udf inlet_x_velocity) from the X-Velocity drop-down list. Click OK to accept the new boundary condition and close the dialog box. Your user profile will be used in the subsequent solution calculation.

 Setup →   Boundary Conditions →   cold-inlet → Edit...

Figure 8.8: The Velocity Inlet Dialog Box

After initializing the solution, run the calculation.

 Solution → Run Calculation  Calculate

After the solution is run to convergence, obtain a revised velocity field. The velocity magnitude contours for the parabolic inlet x velocity are shown in Figure 8.9: Velocity Magnitude Contours for a Parabolic Inlet Velocity Profile, and can be compared to the results of a constant velocity of 0.1 m/s (Figure 8.2: Velocity Magnitude Contours for a Constant Inlet x Velocity). For the constant velocity condition, the velocity profile is seen to develop as the flow passes through the duct. The velocity field for the imposed parabolic profile, however, shows a maximum at the center of the inlet, which drops to zero at the walls.

Figure 8.9: Velocity Magnitude Contours for a Parabolic Inlet Velocity Profile