        ## 9.1.3 Setting Up UDS Equations in ANSYS FLUENT

ANSYS FLUENT allows you to define up to user-defined scalar (UDS) transport equations in your model. The general scalar transport equation, this equation in the separate Theory Guide , is shown below with the four terms (transient, flux, diffusivity, source) that you can customize. (Figure  9.1.1). You will define a UDS transport equation by setting the parameters for these four terms. In addition, you can set boundary conditions for the variables within cells of a fluid or solid zone for a particular scalar equation. This is done by fixing the value of in Figure  9.1.1. When is fixed in a given cell, the UDS scalar transport is not solved and the cell is not included when the residual sum is computed. Additionally, you can also specify custom boundary conditions in the mixture on all wall, inflow, and outflow boundaries on a per-scalar basis.

The procedures for setting up a user-defined scalar (UDS) equation for single-phase and multiphase flows are outlined below. Note that a significant difference between a UDS for a single-phase versus a multiphase application is that you will need to associate each UDS with its corresponding phase domain or mixture domain, depending on your application. If you supply UDFs for transient terms, convective fluxes, and sources, you will need to be aware that they are directly called from the phase or mixture domains, according to the scalar association settings.

See the separate UDF Manual for information on using UDFs to define scalar quantities.

Single Phase Flow

1.   Specify the number of UDS equations you require in the User-Defined Scalars dialog box (Figure  9.1.2).

Define User-Defined Scalars... The maximum number of user-defined scalar transport equations you can define is 50. ANSYS FLUENT assigns numbers to the equations starting with . Note that ANSYS FLUENT assigns a default name for each scalar equation ( User Scalar 0, User Scalar 1, etc.). These labels will appear in graphics dialog boxes in ANSYS FLUENT. You can change them by means of a UDF. See the separate UDF Manual for details. 2.   Enable Inlet Diffusion if you want to include the diffusion term in the UDS transport equation for all inflow and outflow boundaries.

3.   Set the first user-defined scalar equation parameters by making sure that the UDS Index is set to .

(a)   Specify the Solution Zones you want the scalar equation to be solved in as all fluid zones, all solid zones, all zones (fluid and solid) or selected zones. If you choose selected zones, click on the Edit button to view the list of zones you can select.

(b)   Specify the Flux Function to be none, mass flow rate, or a user-defined function (UDF). The Flux Function determines how the convective flux is computed, which determines the equation that ANSYS FLUENT solves for the user-defined scalar. Selecting none, mass flow rate, or a user-defined function results in ANSYS FLUENT solving this equation , this equation , or this equation , respectively (in the separate Theory Guide). See the separate UDF Manual for details on flux UDFs.

(c)   Specify the Unsteady Function to be none, default, or a user-defined function (UDF). Select none for a steady state solution and default if you want the transient term in this equation to be solved (in the separate Theory Guide). See the separate UDF Manual for details on unsteady UDFs.

(d)   Repeat this process for each scalar equation by incrementing the UDS Index.

(e)   Click OK when all user scalar equations have been defined.

4.   To specify source term(s) for each of the UDS equations, enable the Source Terms option in the Fluid or Solid dialog box (Figure  9.1.3) and click on the Source Terms tab. The source parameters will be displayed. Cell Zone Conditions (a)   Specify the number of sources you require for each scalar equation by clicking on the Edit... button next to the scalar name (e.g., User Scalar 0). This will open the User Scalar 0 Sources dialog box (Figure  9.1.4). (b)   Specify the Number of User Scalar Sources for the scalar equation by incrementing the counter. Based on the value you have chosen, the sources will be added to the list in the dialog box. Specify each source to be none, constant, or a user-defined function (UDF). For details on defining a UDF scalar source, see the separate UDF Manual. Click OK when you have specified all scalar sources.

5.   To specify diffusivity for each of the UDS equations, display the Materials task page (Figure  9.1.5) and select either defined-per-uds (the default) or user-defined in the drop-down list for UDS Diffusivity. Materials Create/Edit See Section  8.6 for details on the different options available to you for defining diffusion coefficients.

6.   To specify boundary conditions for the user-defined scalars on wall, inflow, and outflow boundaries, you can define a specific value or a specific flux for each scalar. A coupled boundary condition can be specified on two-sided walls for scalars that are to be solved in regions on both sides of the wall (i.e., scalars solved in both fluid and solid zones). Boundary Conditions

(a)   In the UDS tab under User Defined Scalar Boundary Condition, select either Specified Flux or Specified Value in the drop-down list next to each scalar (e.g., User Scalar 0) for a boundary wall. For interior walls, select Coupled Boundary if the scalars are to be solved on both sides of a two-sided wall. Note that the Coupled Boundary option will only show up in the drop-down list if the scalar is defined in the fluid and solid zones in the User-Defined Scalars dialog box.

(b)   Under User Defined Scalar Boundary Value, enter a constant value or select a user-defined function from the drop-down list for each scalar. If you select Specified Flux, your input will be the value of the flux at the boundary (i.e., the negative of the term in parenthesis on the left hand side of this equation (in the separate Theory Guide) dot [as in the dot product of] [as in the vector, n], where is the normal into the domain). If you select Specified Value, your input will be the value of the scalar itself at the boundary. See the separate UDF Manual for information on using UDFs for UDS boundary conditions.

7.   Set the solution parameters in the Solution Controls task page, specify an initial value for each UDS (as you do for all other scalar transport equations), and calculate a solution.

8.   Examine the results using the usual postprocessing tools. In each postprocessing dialog box, the list of field variables will include the User Defined Scalars... category, which contains the value of each UDS and its diffusion coefficient ( in this equation , this equation , this equation , or this equation (in the separate Theory Guide):

• User Scalar-n

• Diffusion Coef. of Scalar-n

Multiphase Flow

1.   Specify the number of scalars in the User-Defined Scalars dialog box (Figure  9.1.6).

Define User-Defined Scalars...  The maximum number of user-defined scalar transport equations you can define is 50. ANSYS FLUENT assigns numbers to the equations starting with . The default association type is set to mixture for all scalars. Note that ANSYS FLUENT assigns a default name for each scalar equation ( User Scalar 0, User Scalar 1, etc.). These labels will appear in graphics dialog boxes in ANSYS FLUENT. You can change them by means of a UDF. See the separate UDF Manual for details.

2.   Keep the default Inlet Diffusion enabled if you want to include the diffusion term in the UDS transport equation for all inflow and outflow boundaries.

3.   Set the first user-defined scalar equation parameters by making sure that the UDS Index is set to .

(a)   Select the Phase you want the scalar equation solved in as a primary phase, secondary phase, or the mixture.

(b)   Specify the Solution Zones you want the scalar equation to be solved in as all fluid zones, all solid zones, all zones (fluid and solid) or selected zones. If you choose selected zones, click on the Edit button to view the list of zones you can select.

(c)   Specify the Flux Function to Unsteady Function the same way as you would for a single phase flow (see above).

(d)   Repeat this process for each scalar equation by incrementing the UDS Index.

(e)   Click OK when all user scalar equations have been defined.

4.   Specify source term(s) for each of the UDS equations in the Fluid or Solid dialog box as described for a single phase flow(see above).

5.   Specify boundary conditions for the user-defined scalars in the mixture on all wall, inflow, and outflow boundary as described for a single phase flow (see above).

6.   Set the solution parameters, specify an initial value for each UDS (as you do for all other scalar transport equations), and calculate a solution.     Previous: 9.1.2 UDS Theory
Up: 9.1 User-Defined Scalar (UDS)
Next: 9.2 Periodic Flows
Release 12.0 © ANSYS, Inc. 2009-01-29