When you select the Discrete Transfer model and click OK in the Radiation Model dialog box, the DTRM Rays dialog box (Figure 16.18: The DTRM Rays Dialog Box) will open automatically. If you need to modify the current settings later in the problem setup or solution procedure, you can open this dialog box by clicking DTRM Rays... in the Physics ribbon tab (Model Specific group box).

Figure 16.18: The DTRM Rays Dialog Box

In this dialog box you will set parameters for and create the rays and clusters discussed in The DTRM Equations in the Theory Guide.

The procedure is as follows:

Your inputs for Cells Per Volume Cluster and Faces Per Surface Cluster will control the number of radiating surfaces and absorbing cells. By default, each is set to 1, so the number of surface clusters (radiating surfaces) will be the number of boundary faces, and the number of volume clusters (absorbing cells) will be the number of cells in the domain. For small 2D problems, these are acceptable numbers, but for larger problems you will want to reduce the number of surface and/or volume clusters in order to reduce the ray-tracing expense. See Clustering in the Theory Guide for details about clustering.

Your inputs for Theta Divisions and Phi Divisions will control the number of rays being traced from each surface cluster (radiating surface).

Theta Divisions defines the number of discrete divisions in the angle used to define the solid angle about a point on a surface. The solid angle is defined as varies from 0 to 90 degrees (in the Theory Guide), and the default setting of 1 for the number of discrete settings implies that there will be one ray traced from the surface.

Phi Divisions defines the number of discrete divisions in the angle used to define the solid angle about a point on a surface. The solid angle is defined as varies from 0 to 360 degrees (Figure 5.2: Angles θ and φ Defining the Hemispherical Solid Angle About a Point P in the Theory Guide). The default setting of 4 implies that each ray traced from the surface will be located at a 90^° angle, and in combination with the default setting for Theta Divisions, above, implies that 4 rays will be traced from each surface control volume. In many cases, it is recommended that you at least double the number of divisions in and .

After you have activated the DTRM and defined all of the parameters controlling the ray tracing, you must create a ray file, which will be read back in and used during the radiation calculation. The ray file contains a description of the ray traces (for example, path lengths, cells traversed by each ray). This information is stored in the ray file, instead of being recomputed, in order to speed up the calculation process.

By default, a binary ray file will be written. You can also create text (formatted) ray files by turning off the Write Binary Files option in The Select File Dialog Box.

The ray filename must be specified to Ansys Fluent only once. Thereafter, the filename is stored in your case file and the ray file will be automatically read into Ansys Fluent whenever the case file is read. Ansys Fluent will remind you that it is reading the ray file after it finishes reading the rest of the case file by reporting its progress in the console.

Note that the ray filename stored in your case file may not contain the full name of the directory in which the ray file exists. The full directory name will be stored in the case file only if you initially read the ray file through the GUI (or if you typed in the directory name along with the filename when using the text interface). In the event that the full directory name is absent, the automatic reading of the ray file may fail (since Ansys Fluent does not know in which directory to look for the file), and you will need to manually specify the ray file, using the File/Read/DTRM Rays... ribbon tab item. The safest approaches are to use the GUI when you first read the ray file or to supply the full directory name when using the text interface.

Once a ray file has been created or read in manually, you can click the Display Clusters button in the DTRM Rays dialog box to graphically display the clusters in the domain. See Displaying Rays and Clusters for the DTRM for additional information about displaying rays and clusters.

You can use the View Factors and Clustering dialog box (Figure 16.20: The View Factors and Clustering Dialog Box) to define how the surface clusters are formed and how the view factors are calculated for the S2S model. To open this dialog box, click Settings... in the View Factors and Clustering group box in the Radiation Model Dialog Box (Figure 16.19: The Radiation Model Dialog Box (S2S Model)).

Figure 16.20: The View Factors and Clustering Dialog Box

 

16.3.4.1.1. Forming Surface Clusters

You can set the number of faces per surface cluster (FPSC) for each flow boundary (that is, exhaust fan, inlet vent, intake fan, outlet vent, mass-flow inlet, mass-flow outlet, pressure far-field, pressure inlet, pressure outlet, outflow, and velocity inlet boundary) and wall that is adjacent to a fluid zone; in this way, you can control the number of radiating surfaces and (if you select Cluster to Cluster for Basis) view factor surfaces. By default, the FPSC value is set to everywhere, so the number of surface clusters (radiating/view factor surfaces) will be equal to the number of boundary faces. For small 2D problems, this is an acceptable number. For larger problems, you may want to reduce the number of surface clusters (that is, increase the FPSC) to reduce both the size of the view factor file and the memory requirement. Such a reduction in the number of clusters, however, comes at the cost of some accuracy. Note that for a thermally coupled mesh interface (that is, a fluid-fluid interface with Coupled Wall enabled, or an interface involving a solid zone), the FPSC is always set to 1. See Clustering in the Theory Guide for details about clustering.

---

Important:  If you plan to use the cluster to cluster basis for the view factor calculation, be sure that the FPSC values are appropriate for both the radiosity calculation and the view factors.

---

Note that during the creation of a cluster on a non-conformal interface, its parent thread is taken into the consideration; it may happen that the cluster is somewhat larger than its child face, which may lead some inaccuracy in the flux calculation.

The Clustering group box in the View Factors and Clustering dialog box (Figure 16.20: The View Factors and Clustering Dialog Box) provides two methods for revising the default FPSC values:

• manual

• automatic

If you select Manual in the Options group box, you can specify an FPSC value for all flow boundaries in the Faces per Surface Cluster for Flow Boundary Zones number-entry box in the Manual group box. If you then click Apply to All Walls, you will apply this value to all wall zones that are adjacent to fluid zones as well. For a wall that requires a different FPSC value (that is, you may want a lower value for walls in critical areas, and higher values in non-critical areas), you will need to open the boundary condition dialog box (Figure 16.21: The Wall Dialog Box) for that particular wall and modify the Faces Per Surface Cluster in the S2S Parameters group box of the Radiation tab. Note that the Radiation tab also allows you to specify whether the wall participates in the view factor calculation, as described in Specifying Boundary Zone Participation.

---

Note:

• Only zones attached to fluid cell zones are used for creating surface clusters.

• Faces Per Surface Cluster (FPSC) is indicative of the actual reduction factor except when the surfaces are planar. The surface clustering algorithm uses other criteria (angle between faces, and so on) to ensure the clusters are nearly planar, so it is possible that there will be no further reduction in the total number of clusters beyond a certain value of FPSC.

---

Figure 16.21: The Wall Dialog Box

---

Important:  The Faces Per Surface Cluster number-entry box will not be visible in the GUI on wall boundary zones that are attached to a solid.

---

Using the manual method to specify the FPSC values for walls can become very cumbersome if the model involves a large number of radiating faces, which is typically the case in underhood models. In such circumstances, it is recommended that you use the automatic clustering method instead. In this method, different FPSC values are assigned to the walls automatically, based on the distance of the walls from and the FPSC values of the walls that are defined as critical. The steps you will need to take are as follows:

1. Select Automatic from the Options list in the View Factors and Clustering dialog box.

2. For each wall that you deem critical, perform the following actions in the Wall dialog box (Figure 16.21: The Wall Dialog Box):

   1. Click the Radiation tab.

   2. Enter an appropriate value for Faces Per Surface Cluster in the S2S Parameters group box.

   3. Enable the Critical Zone option.

   4. Click OK to close the Wall dialog box.

3. Enter the Maximum Faces per Surface Cluster value in the View Factors and Clustering dialog box and click the Compute button. Ansys Fluent will automatically calculate and update the Faces Per Surface Cluster values for all Wall dialog boxes adjacent to fluid zones that do not have Critical Zone enabled, without computing the clusters.

4. You can check the automatically assigned FPSC values by opening the boundary condition dialog box of any non-critical wall of interest and examining the value for Faces Per Surface Cluster in the S2S Parameters group box of Radiation tab. You can manually modify the value for Faces Per Surface Cluster as necessary.

 

16.3.4.1.1.1. Setting the Split Angle for Clusters

Whether you set the FPSC value manually or automatically, you have the option of modifying the cutoff or “split” angle between adjacent face normals for the purpose of controlling surface clustering. The split angle sets the limit for which adjacent faces are clustered. A smaller split angle allows for a better representation of the view factor. By default, no surface cluster will contain any face that has a face normal greater than 20^°. To modify the value of this parameter, you can use the split-angle text command:

define → models → radiation → s2s-parameters → split-angle

 

16.3.4.1.2. Setting Up the View Factor Calculation

You can control many aspects of how the view factors are calculated for your S2S model: how surfaces are defined; the computational method and related parameters; whether surface blocking will be accounted for; and which boundary zones will participate in the calculation. All of these controls are available in the View Factors group box in the View Factors and Clustering dialog box (Figure 16.20: The View Factors and Clustering Dialog Box), and are described in the sections that follow.

 

16.3.4.1.2.1. Selecting the Basis for Computing View Factors

Ansys Fluent allows two ways to define the surfaces used for the view factor calculation, as described in Clustering and View Factors in the Theory Guide. If you want the surfaces to be the boundary faces of the mesh, select Face to Face for Basis in the View Factor group box of the View Factors and Clustering dialog box. This is the default selection.

Alternatively, you can select Cluster to Cluster for Basis, in order to reduce the computational expense and storage requirements. In this case, the surfaces used to calculate the view factors are the clusters defined by the settings in the Cluster group box of the View Factors and Clustering dialog box. The reduction in computational time will be proportional to the number of surface clusters used in the view factor calculation. The trade-offs of using the cluster to cluster basis for the calculation are that the accuracy may decrease, and the following limitations apply:

• The mesh must be 3D.

• You cannot subdivide the faces as part of the hemicube method parameters, which can cause the view factors to be overestimated.

• Polyhedral meshes are restricted to 1 face per surface cluster.

• When using Cluster to Cluster, surface clusters will form on non-conformal interfaces by default only with the Ray Tracing method enabled. If you do not want clusters to form on non-conformal interfaces, you can use the following command and answer no.

  define/models/radiation/s2s-parameters/enable-mesh-interface-clustering?

 

16.3.4.1.2.2. Selecting the Method for Computing View Factors

Ansys Fluent provides two methods for computing view factors: the ray tracing method (which is selected by default) and the hemicube method. The following limitations apply:

• The hemicube method is available only for 3D and axisymmetric cases.

• The hemicube method should not be used when any of the zones are defined as periodic or symmetry boundaries, as these types are not currently supported.

• For the ray tracing method, when running in distributed parallel mode (including with Microsoft Job Scheduler), the working directory must be shared across all machines.

The hemicube method uses a differential area-to-area method and calculates the view factors on a row-by-row basis. The view factors calculated from the differential areas are summed to provide the view factor for the whole surface. This method originated from the use of the radiosity approach in the field of computer graphics  [33].

To use the hemicube method to compute the view factors, select Hemicube from the Method list in the View Factors and Clustering dialog box. It is recommended that you use the hemicube method for large, complex models with few obstructing surfaces between the radiating surfaces.

The hemicube method is based upon three assumptions about the geometry of the surfaces: aliasing, visibility, and proximity. To validate these assumptions, you can specify three different hemicube parameters, which can help you obtain better accuracy in calculating view factors. In most cases, however, the default settings will be sufficient.

• Aliasing—The true projection of each visible face onto the hemicube can be accurately accounted for by using a finite-resolution hemicube. As described previously, the faces are projected onto a hemicube. Because of the finite resolution of the hemicube, the projected areas and resulting view factors may be overestimated or underestimated. Aliasing effects can be reduced by increasing the value of the Resolution of the hemicube in the Parameters group box.

• Visibility—The visibility between any two faces does not change. In some cases, face has a complete view of face from its centroid, but some other face occludes much of face from face . In such a case, the hemicube method will overestimate the view factor between face and face calculated from the centroid of face . This error can be reduced by subdividing face into smaller subfaces. You can specify the number of subfaces by entering a value for Subdivisions in the Parameters group box. Note that you cannot subdivide the faces when Cluster to Cluster is selected for Basis.

• Proximity—The distance between faces is great compared to the effective diameter of the faces. The proximity assumption is violated whenever faces are close together in comparison to their effective diameter or are adjacent to one another. In such cases, the distances between the centroid of one face and all points on the other face vary greatly. Since the view factor dependence on distance is nonlinear, the result is a poor estimate of the view factor.

  In the Parameters group box, you can set a limit for the Normalized Separation Distance, which is the ratio of the minimum face separation to the effective diameter of the face. If the computed normalized separation distance is less than the specified value, the face will then be divided into a number of subfaces until the normalized distances of the subfaces are greater than the specified value. Alternatively, you can specify the number of subfaces to create for such faces by entering a value for Subdivisions.

While the hemicube method projects radiating surfaces onto a hemicube, the ray tracing method instead traces rays through the centers of every hemicube face to determine which surfaces are visible through that face. Note that the ray tracing method does not subdivide the faces (as can be done when using the hemicube method by setting the Subdivisions or Normalized Separation Distance parameters), and so the view factors may be less accurate than those calculated using the hemicube method for surfaces that have a normalized separation distance less than 5.

To use the ray tracing method to compute the view factors, select Ray Tracing from the Method list in the View Factors and Clustering dialog box. You can adjust the value of the Resolution in the Parameters group box in order to reduce the impact of aliasing effects, as described previously.

 

16.3.4.1.2.3. Accounting for Blocking Surfaces

View factor calculations depend on the geometric orientations of surface pairs with respect to each other. Two situations may be encountered when examining surface pairs:

• If there is no obstruction between the surface pairs under consideration, then they are referred to as “nonblocking” surfaces.

• If there is another surface blocking the views between the surfaces under consideration, then they are referred to as “blocking” surfaces. Blocking will change the view factors between the surface pairs and require additional checks to compute the correct value of the view factors.

For cases with blocking surfaces, select Blocking from the Surfaces list in the View Factors and Clustering dialog box. For cases with nonblocking surfaces, you can choose either Blocking or Nonblocking without affecting the accuracy. However, it is better to choose Nonblocking for such cases, as it takes less time to compute.

 

16.3.4.1.2.4. Specifying Boundary Zone Participation

You can choose to exclude walls and inlet and exit boundaries from participating in the view factor calculation. If you are unsure whether it is necessary to calculate view factors for a particular boundary zone ahead of time, it is recommended that you allow it to participate; you can always reverse this decision as part of a future calculation run.

There are two ways in which you can enable/disable the participation of walls and inlet and exit boundaries in the view factor calculation. One of those ways is to use the Participates in View Factor Calculation option in the Radiation tab of the boundary condition dialog box. The other method is to use the Participating Boundary Zones dialog box (Figure 16.22: The Participating Boundary Zones Dialog Box), which is accessed by clicking the Select... button next to the Zones Participating in View Factor Calculation label in the View Factors and Clustering dialog box. For cases that are made up of a very large number of zones, such as underhood applications, the latter method is recommended.

---

Important:  If you compute the view factors and then later alter which boundary zones participate in the view factor calculation, you must recompute the view factors so that the data is up to date.

---

Figure 16.22: The Participating Boundary Zones Dialog Box

The Participating Boundary Zones dialog box allows you to easily specify those zones that are participating or non-participating without having to visit the boundary conditions dialog box of each zone. For cases that have a small number of boundary zones, you can simply select the zones that you do not want to participate in the view factor calculation from the Participating Boundary Zones list and click the arrow button that points to the right, so that the zones are moved to the Non-Participating Boundary Zones list; if you make an error, you can always reverse this process (that is, select a zone in the Non-Participating Boundary Zones list and click the arrow button that points to the left). This can be cumbersome for cases that have a large number of boundary zones, and so the following procedure is recommended instead:

1. Make sure that your clustering options (see Forming Surface Clusters) are appropriate for your view factor settings:

   1. Select Automatic from the Options list in the Clustering group box of the View Factors and Clustering dialog box, as this enables some GUI items in the Participating Boundary Zones dialog box.

      ---

      Important:  Note that if you do not want to use the Automatic option for the clustering, you can revert to the Manual option after you are done using the Participating Boundary Zones dialog box.

      ---

   2. Verify that the walls you specified as critical (by enabling the Critical Zone option in the Radiation tab of the boundary condition dialog box) also correspond to those that are critical for the view factor calculation. You must have specified at least one critical zone for the steps that follow.

2. Click the Compute button in the Maximum Distance from Critical Zone dialog box, to update the value displayed for To All Other Zones. This value represents the maximum distance between the centroids of a critical zone and a non-critical zone in the mesh; it is for information purposes only, and cannot be edited in this dialog box.

3. Based on the value displayed for To All Other Zones, enter a threshold value for To Participating Zones. The value you enter will specify the maximum distance allowed between the centroids of a critical zone and a zone that participates in the view factor calculation. Then click the Apply button to move all zones beyond this distance into the Non-Participating Boundary Zones list.

4. Review the zones displayed in the Participating Boundary Zones and Non-Participating Boundary Zones lists. If necessary, select zones in these lists and use the arrow buttons to move them to the appropriate list, as described previously.

If at any point you want to visually identify zones displayed in the Participating Boundary Zones and Non-Participating Boundary Zones lists, select the zones and click the Display Zones button. Only the selected zones will be displayed in the graphics window.

If any zones are displayed in the Non-Participating Boundary Zones list, ensure to enter an appropriate temperature for Non-Participating Boundary Zones Temperature. In most cases the appropriate value is the ambient temperature, which by default is assumed to be 300 K.

After you have specified which zones do not participate in view factor calculation and set their temperature, click OK to store the settings and close the Participating Boundary Zones dialog box. You can then proceed to computing the view factors, as described in the section that follows.

Ansys Fluent can compute the view factors for your problem in the current session and save them to a file for use in the current session and future sessions.

To compute view factors in your current Ansys Fluent session, you must first set the parameters for the view factor calculation in the View Factors and Clustering dialog box (see View Factors and Clustering Settings for details) and click OK to save them. When you have set the view factor and surface cluster parameters, click the Compute/Write/Read... button in the View Factors and Clustering group box of the Radiation Model dialog box. A Select File dialog box will open, prompting you for the name of the file to which you would like to save the surface cluster information and view factors.

View factor files can be created in any of the following formats:

Note that when using the TUI, you must directly specify the extension in the file name you provide.

The option to Write Binary Files is enabled by default, which reduces the time needed to write and read view factor files. When you click OK in the Select File dialog box, Ansys Fluent  writes the surface cluster information to the file. Ansys Fluent uses the surface cluster information to compute the view factors, save the view factors to the same file, and then automatically read the view factors. The Ansys Fluent console will report the status of the view factor calculation. For example:

 Completed 25% calculation of view factors
 
 Completed 50% calculation of view factors
 
 Completed 75% calculation of view factors
 
 Completed 100 % calculation of view factors

Intersection zones for non-conformal interfaces are not created.
View factors will be computed during solution initialization.

If the view factors for your problem have already been computed and saved to a file, you can read them into Ansys Fluent. To read in the view factors, click Read Existing File... button in the View Factors and Clustering group box of the Radiation Model dialog box. A Select File dialog box will open where you can specify the name of the file containing the view factors. For Files of type, select CFF S2S Files to read .h5 files or select S2S Files to read other formats. Alternatively, you can read the view factors file using the File/Read/View Factors... ribbon tab item.

When you select the Discrete Ordinates model, the Radiation Model dialog box will expand to show inputs for Angular Discretization (see Figure 16.16: The Radiation Model Dialog Box (DO Model)). In this section, you will set parameters for the angular discretization and pixelation described in Angular Discretization and Pixelation in the Theory Guide.

Theta Divisions () and Phi Divisions () will define the number of control angles used to discretize each octant of the angular space (see Figure 5.3: Angular Coordinate System in the Theory Guide). Note that higher levels of discretization are recommended for problems where specular exchange of radiation is important to increase the likelihood of the correct beam direction being captured. For a 2D model, Ansys Fluent will solve only 4 octants (due to symmetry); therefore, a total of directions will be solved. For a 3D model, 8 octants are solved, resulting in directions . By default, the number of Theta Divisions and the number of Phi Divisions are both set to 2. For most practical problems, these settings are acceptable, however, a setting of 2 is considered to be a coarse estimate. Increasing the discretization of Theta Divisions and Phi Divisions to a minimum of 3, or up to 5, will achieve more reliable results. A finer angular discretization can be specified to better resolve the influence of small geometric features or strong spatial variations in temperature, but larger numbers of Theta Divisions and Phi Divisions will add to the cost of the computation.

Theta Pixels and Phi Pixels are used to control the pixelation that accounts for any control volume overhang (see Figure 5.7: Pixelation of Control Angle in the Theory Guide and the figures and discussion preceding it). For problems involving gray-diffuse radiation, the default pixelation of is usually sufficient. For problems involving symmetry, periodic, specular, or semi-transparent boundaries, a pixelation of is recommended and will achieve acceptable results. The computational effort, as a result of increasing the pixelation, is less than the computational effort caused by increasing the divisions. You should be aware, however, that increasing the pixelation adds to the cost of computation.

If you want to model non-gray radiation using the DO model, you can specify the Number of Bands () under Non-Gray Model in the expanded Radiation Model dialog box (Figure 16.24: The Radiation Model Dialog Box (Non-Gray DO Model)). For a 2D model, Ansys Fluent will solve directions. For a 3D model, directions will be solved. By default, the Number of Bands is set to zero, indicating that only gray radiation will be modeled. Because the cost of computation increases directly with the number of bands, you should try to minimize the number of bands used. In many cases, the absorption coefficient or the wall emissivity is effectively constant for the wavelengths of importance in the temperature range of the problem. For such cases, the gray DO model can be used with little loss of accuracy. For other cases, non-gray behavior is important, but relatively few bands are necessary. For typical glasses, for example, two or three bands will frequently suffice.

When a nonzero Number of Bands is specified, the Radiation Model dialog box will expand once again to show the Wavelength Intervals (Figure 16.24: The Radiation Model Dialog Box (Non-Gray DO Model)). You can specify a Name for each wavelength band, as well as the Start and End wavelength of the band in m. Note that the wavelength bands are specified for vacuum (). Ansys Fluent will automatically account for the refractive index in setting band limits for media with different from unity.

Figure 16.24: The Radiation Model Dialog Box (Non-Gray DO Model)

The frequency of radiation remains constant as radiation travels across a semi-transparent interface. The wavelength, however, changes such that is constant. Therefore, when radiation passes from a medium with refractive index to one with refractive index , the following relationship holds:

(16–3)

Here and are the wavelengths associated with the two media. It is conventional to specify the wavelength rather than frequency. Ansys Fluent requires you to specify wavelength bands (in m) for an equivalent medium with .

For example, consider a typical glass with a step jump in the absorption coefficient at a cut-off wavelength of . The absorption coefficient is for and for . The refractive index of the glass is . Since is constant across a semi-transparent interface, the equivalent cut-off wavelength for a medium with is using Equation 16–3. You should choose two bands in this case, with the limits 0 to and to 100. Here, the upper wavelength limit has been chosen to be a large number, 100, in order to ensure that the entire spectrum is covered by the bands. When multiple materials exist, you should convert all the cut-off wavelengths to equivalent cut-off wavelengths for an medium, and choose the band boundaries accordingly.

The bands can have different widths and need not be contiguous. You can ensure that the entire spectrum is covered by your bands by choosing and . Here and are the minimum and maximum wavelength bounds of your wavelength bands, and is the minimum expected temperature in the domain.

Ansys Fluent allows you to use a user-defined function (UDF) to modify the emissivity weighting factor (which otherwise defaults to the black body emission factor obtained from a standard Planck distribution). The emissivity weighting factor appears in the emission term of the radiative transfer equation for the non-gray model, as shown in Equation 5–100 in the Theory Guide. For more information, see DEFINE_EMISSIVITY_WEIGHTING_FACTOR in the Fluent Customization Manual.

For applications involving optical thicknesses greater than 10, you can enable the DO/Energy Coupling option in the Radiation Model (Figure 16.25: The Radiation Model Dialog Box with DO/Energy Coupling Enabled) in order to couple the energy and intensity equations at each cell, solving them simultaneously. This approach accelerates the convergence of the finite volume scheme for radiative heat transfer and can be used with the gray or non-gray radiation model.

Figure 16.25: The Radiation Model Dialog Box with DO/Energy Coupling Enabled

If you are using the non-gray P-1, DO, or MC model, you can specify a different constant absorption coefficient for each of the bands used by the gray-band model, as described in Radiation Properties. You cannot, however, compute a composition-dependent absorption coefficient in each band. If you use the WSGGM to compute a variable absorption coefficient, the value will be the same for all bands. Alternatively, you can specify a user-defined function (UDF) for the absorption coefficient. For more information, see DEFINE_PROPERTY UDFs in the Fluent Customization Manual.

If you are using the non-gray P-1, DO, or MC model, you can specify a different constant refractive index for each of the bands used by the gray-band model, as described in Radiation Properties. You cannot, however, compute a composition-dependent refractive index in each band.

The DTRM, S2S, Rosseland, and gray P-1 models assume all walls to be gray and diffuse. The only radiation boundary condition required in the Wall dialog box is the Internal Emissivity. For the Rosseland model, the internal emissivity is automatically set to 1. For the DTRM, S2S, and gray P-1 models, you can enter the appropriate value for Internal Emissivity in the Radiation tab of the Wall dialog box. The default value is 1. Alternatively, you can specify a user-defined function for Internal Emissivity. For more information, see DEFINE_PROFILE in the Fluent Customization Manual.

For the non-gray P-1 model, specify a constant Internal Emissivity for each wavelength band in the Radiation tab of the Wall dialog box (the default value in each band is 1). Alternatively, you can specify the internal emissivity using a boundary condition parameter (see Creating a New Parameter). See Defining Boundary Conditions for Radiation for details.

When the DO model is used, you can model opaque walls, as discussed in Boundary and Cell Zone Condition Treatment at Opaque Walls in the Theory Guide, as well as semi-transparent walls (Cell Zone and Boundary Condition Treatment at Semi-Transparent Walls in the Theory Guide).

You can use a diffuse wall to model wall boundaries in many industrial applications since, for the most part, surface roughness makes the reflection of incident radiation diffuse. For highly polished surfaces, such as reflectors or mirrors, the specular boundary condition is appropriate. The semi-transparent boundary condition can be appropriate, for example, when modeling for glass panes in air.

 

16.3.8.3.1. Opaque Wall for the DO Model

In the Radiation tab of the Wall dialog box (Figure 16.28: The Wall Dialog Box Showing Radiation Conditions for an Opaque Wall), select opaque in the BC Type drop-down list to specify an opaque wall.

Figure 16.28: The Wall Dialog Box Showing Radiation Conditions for an Opaque Wall

Specify the fraction of reflected radiation flux that is to be treated as diffuse. By default, the Diffuse Fraction is set to , indicating that all of the radiation is diffuse. A diffuse fraction equal to indicates purely specular reflected radiation. A diffuse fraction between and will result in partially diffuse and partially specular reflected energy. If the non-gray DO model is being used, the Diffuse Fraction can be specified for each band. See Boundary and Cell Zone Condition Treatment at Opaque Walls in the Theory Guide for more details.

For gray-radiation DO models, enter the appropriate value for Internal Emissivity (default value is 1). For non-gray DO models, specify a constant Internal Emissivity for each wavelength band in the Radiation tab of the Wall dialog box. (The default value in each band is 1.) Alternatively, you can specify the internal emissivity using a boundary condition parameter (see Creating a New Parameter).

You can also specify the external emissivity and external radiation temperature for an opaque wall when the thermal conditions are set to Radiation or Mixed in the Wall dialog box (Figure 16.29: The Wall Dialog Box Showing External Emissivity and External Radiation Temperature Thermal Conditions). Alternatively, you can specify a UDF for these parameters; for more information, see DEFINE_PROFILE in the Fluent Customization Manual.

Figure 16.29: The Wall Dialog Box Showing External Emissivity and External Radiation Temperature Thermal Conditions

For more information on boundary condition treatment at opaque walls, see Boundary and Cell Zone Condition Treatment at Opaque Walls in the Theory Guide.

 

16.3.8.3.2. Semi-Transparent Walls for the DO Model

To define radiation for an exterior semi-transparent wall, click the Radiation tab in the Wall dialog box and then select semi-transparent in the BC Type drop-down list (Figure 16.30: The Wall Dialog Box for a Semi-Transparent Wall Boundary). The dialog box will expand to display the semi-transparent wall inputs needed to define an external irradiation flux (Figure 16.30: The Wall Dialog Box for a Semi-Transparent Wall Boundary).

Figure 16.30: The Wall Dialog Box for a Semi-Transparent Wall Boundary

Then perform the following steps:

1. Specify the value of the irradiation flux (in W/m²) under Direct or Diffuse Irradiation. If the non-gray DO model is being used, a constant Direct or Diffuse Irradiation can be specified for each band.

   ---

   Important:  Note that the external diffuse irradiation specified when using Radiation or Mixed thermal conditions (selected in the Thermal tab), or Diffuse Irradiation (in the Radiation tab) is always distributed hemispherically after transmission through semi-transparent walls (that is independent of whether the external semi-transparent boundary wall is defined as a diffusely or specularly reflecting type).

   ---

2. By default, Apply Direct Irradiation Parallel to the Beam is selected, which means Fluent assumes that the value you specify for Direct Irradiation is the irradiation flux parallel to the Beam Direction. When deselected, Ansys Fluent assumes that the value you specify for Direct Irradiation is the irradiation flux normal to the boundary. See Figure 5.12: DO Irradiation on External Semi-Transparent Wall in Semi-Transparent Exterior Walls in the Theory Guide for details.

3. Define the Beam Width by specifying the beam Theta and Phi extents. Beam width is specified as the solid angle over which the irradiation is distributed. The default value for beam width is , which is suitable for collimated beam radiation. A beam width less than this is likely to result in zero irradiation flux.

4. Specify the (X,Y,Z) vector that defines the Beam Direction. The beam direction is defined as the vector of the centroid of the solid angle (beam width). You can specify the Beam Direction as a constant, a profile or a UDF. This is especially useful in applications where the shape of the radiative source is circular or cylindrical (or nonlinear). For information about boundary profiles, see Reading and Writing Profile Files.

   Note that the actual direction of the beam of radiation that enters the domain will be further influenced by the solid angles available from the number of divisions set up; the effective direction will be the direction vector of the solid angle that the incoming beam falls into. Finally, any nonzero diffuse fraction will act to spread out (hemispherically, proportional to the diffuse fraction) the irradiation that enters the domain.

   Note that the refractive index of the external medium is assumed to be 1. Therefore, if the refractive index of the fluid or solid material adjacent to the semi-transparent boundary is greater than 1, the direction of the prescribed direct irradiation after entering the computational domain will change due to refraction, and the magnitude of the incident radiation can be determined according to Figure 16.31: Refraction of Irradiation Entering Computational Domain.

   Figure 16.31: Refraction of Irradiation Entering Computational Domain

   
   
   

   For a UDF example that specifies the beam direction, see Example 5 - Beam Direction Profile at Semi-Transparent Walls in the Fluent Customization Manual.

5. Specify the Diffuse Fraction, the fraction of the reflected radiation from the wall that is treated as diffuse between 0 and 1. By default, the Diffuse Fraction is set to 1, indicating that all of the radiation is diffuse. A Diffuse Fraction of 0 treats the reflected radiation as purely specular. If you specify a value between 0 and 1, the radiation is treated as partially diffuse and partially specular. If the non-gray DO model is being used, the Diffuse Fraction can be specified for each band. See Diffuse Semi-Transparent Walls in the Theory Guide for details.

---

Important:

• If Heat Flux conditions are specified in the Thermal tab of the Wall dialog box, the specified heat flux is considered to be only the conduction and convection portion of the boundary flux. The given irradiation specifies the incoming exterior radiative flux; the radiative flux transmitted from the domain interior to the outside is computed as a part of the calculation by Ansys Fluent. Internal emissivity is ignored for semi-transparent surfaces.

• Note that when a boundary wall is made semi-transparent Ansys Fluent calculates the amount of radiation leaving as well as entering the domain. If you do not provide a source of irradiation or a radiating thermal condition (for example Mixed or Radiation) then you are effectively radiating to a temperature of K and it is highly likely you may observe temperatures in your model that are lower than expected. Ensure that the external (incoming) radiant conditions give good account of the surroundings.

---

You can also specify the external emissivity and external radiation temperature for a semi-transparent wall when the thermal conditions are set to Radiation or Mixed in the Wall dialog box (Figure 16.29: The Wall Dialog Box Showing External Emissivity and External Radiation Temperature Thermal Conditions). Alternatively, you can specify a user-defined function (UDF) for these parameters; for more information, see DEFINE_PROFILE in the Fluent Customization Manual.

---

Important:  Note that for semi-transparent walls, Internal Emissivity is not available. If you want to include the effect of internal emissivity at semi-transparent walls, you must create a solid zone and specify that it participates in the radiation calculation; see Solid Semi-Transparent Media in the Theory Guide for details.

---

For a detailed description of boundary condition treatment at semi-transparent walls, see Cell Zone and Boundary Condition Treatment at Semi-Transparent Walls in the Theory Guide.

To define radiation for an interior (two-sided) semi-transparent wall, in the Wall dialog box, click the Radiation tab and then select semi-transparent in the BC Type drop-down list (Figure 16.32: The Wall Dialog Box for an Interior Semi-Transparent Wall). Then specify the Diffuse Fraction as described for the previous case.

Figure 16.32: The Wall Dialog Box for an Interior Semi-Transparent Wall

With the DO or MC model, you can specify whether or not you want to solve for radiation in each cell zone in the domain. By default, the DO or MC equations are solved in all fluid zones, but not in any solid zones. If you want to model semi-transparent media, for example, you can enable radiation in the solid zone(s). To do so, enable the Participates In Radiation option in the Solid dialog box (Figure 16.41: The Solid Dialog Box).

Figure 16.41: The Solid Dialog Box

See Solid Semi-Transparent Media in the Theory Guide for more information on solid semi-transparent media.

In general, any well-posed combination of thermal boundary conditions can be used when any of the radiation models is active. The radiation model will be well-posed in combination with fixed temperature walls, conducting walls, and/or walls with set external heat transfer boundary conditions (Thermal Boundary Conditions at Walls). You can also use any of the radiation models with heat flux boundary conditions defined at walls, in which case the heat flux you define will be treated as the sum of the convective and radiative heat fluxes. The exception to this is the case of semi-transparent walls for the DO model. Here, Ansys Fluent allows you to specify the convective and radiative portions of the heat flux separately.

For the P-1 radiation model, you can control the convergence criterion and under-relaxation factor. You should also pay attention to the optical thickness, as described below.

The default convergence criterion for the P-1 model is 10^-6, the same as that for the energy equation, since the two are closely linked. See Monitoring Residuals for details about convergence criteria. You can set the Convergence Criterion for p1 in the Residual Monitors dialog box.

 Solution → Monitors → Residuals  Edit...

The under-relaxation factor for the P-1 model is set with those for other variables, as described in Setting Under-Relaxation Factors. Note that since the equation for the radiation temperature (Equation 5–60 in the Theory Guide) is a relatively stable scalar transport equation, in most cases you can safely use large values of under-relaxation (0.9–1.0).

For optimal convergence with the P-1 model, the optical thickness must be between 0.01 and 10 (preferably not larger than 5). Smaller optical thicknesses are typical for very small enclosures (characteristic size of the order of 1 cm), but for such problems you can safely increase the absorption coefficient to a value for which . Increasing the absorption coefficient will not change the physics of the problem because the difference in the level of transparency of a medium with optical thickness = 0.01 and one with optical thickness <0.01 is indistinguishable within the accuracy level of the computation.

You can control the frequency that the radiation field is updated as the continuous phase solution proceeds for steady and transient simulations. For details, see Iteration Parameters For Radiation Solve Frequency.

When the DTRM is active, Ansys Fluent updates the radiation field during the calculation and computes the resulting energy sources and heat fluxes via the ray-tracing technique described in Ray Tracing in the Theory Guide. Ansys Fluent provides several solution parameters in the expanded portion of the Radiation Model dialog box (Figure 16.42: The Radiation Model Dialog Box (DTRM)).

Figure 16.42: The Radiation Model Dialog Box (DTRM)

You can control the maximum number of iterations of the radiation calculation during each global iteration by changing the Maximum Number of Radiation Iterations. The default setting of 5 means that the radiosity will be updated up to 5 times. The actual number of iterations will be less if the residual convergence criterion is exceeded at any point during these iterations.

The Residual Convergence Criteria parameter (0.001 by default) determines when the radiation intensity update is converged. It is defined as the maximum normalized change in the surface intensity from one DTRM radiation iteration to the next (see Equation 16–4).

You can control the frequency that the radiation field is updated as the continuous phase solution proceeds for steady and transient simulations. For details, see Iteration Parameters For Radiation Solve Frequency.

You can control the maximum number of iterations of the radiation calculation during each global iteration by changing the Maximum Number of Radiation Iterations. The default setting of 5 means that the radiosity will be updated up to 5 times. The actual number of iterations will be less if the residual convergence criterion is exceeded at any point during these iterations.

The Residual Convergence Criteria (0.001 by default) determines when the radiosity update is converged. It is defined as the maximum normalized change in the radiosity from one S2S radiation iteration to the next (see Equation 16–5).

You can control the frequency that the radiation field is updated as the continuous phase solution proceeds for steady and transient simulations. For details, see Iteration Parameters For Radiation Solve Frequency.

For most problems, the default under-relaxation of 1.0 for the DO equations is adequate. For problems with large optical thicknesses (), you may experience slow convergence or solution oscillation. For such cases, under-relaxing the energy and DO equations is useful. Under-relaxation factors between 0.9 and 1.0 are recommended for both equations.

You can control the frequency that the radiation field is updated as the continuous phase solution proceeds for steady and transient simulations. For details, see Iteration Parameters For Radiation Solve Frequency.

Wall Irradiation Flux.Normalized Std Deviation and Radiation Intensity.Normalized Std Deviation (both available during postprocessing) can give an indication of the quality of the solution. They arise from the stochastic nature of the Monte Carlo model.

The Monte Carlo radiation solver computes the standard deviation error based on Poisson statistics. The user-specified number of histories is divided into several groups. Histories are selected from each group and their physical interactions (emission, absorption, reflection, and so on) are tracked through the domain. At the end of the calculation, each group provides values for the quantities of interest, such as irradiation heat flux or absorbed radiation. The mean value, and standard deviation, of each quantity of interest are computed from the groups. A normalized standard deviation is computed by dividing the standard deviation by the mean value.

Because of the stochastic behavior, it can be difficult to judge the convergence of MC radiation cases based on residuals alone, particularly if the standard deviations are large. It is recommended that you create a temperature probe (for example, a Surface Report Definition) and monitor its stability during the solution. For more information, see Creating Report Definitions.

For the DTRM, S2S, DO, and MC models, you can control the frequency that the radiation field is updated as the continuous phase solution proceeds. The options available to control the radiation solve frequency depends on whether the simulation is steady or transient.

Steady Simulations

Under Iteration Parameters, the option Update Radiation Based On can only be set to iteration with the default Iteration Interval set to 10. This means that the radiation calculation is performed once every 10 iterations of the solution process. Increasing the number can speed the calculation process, but may slow overall convergence.

Figure 16.43: Iteration Parameters for Steady Simulations

Transient Simulations

Under Iteration Parameters, the option Update Radiation Based On can be set to time-step or flow-time.

Figure 16.44: Iteration Parameters for Transient Simulations

For updating radiation based on time-step, you must specify the Time Step Interval and Iteration Interval. The default value of 1 for Time Step Interval means the radiation field will be updated every time step. The default Iteration Interval of 0 means the radiation field is updated after the first iteration in a time step. For example, a Time Step Interval of 2 means the radiation field is updated every other time step. An Iteration Interval of 5 means the radiation field is updated every 5 iterations within a timestep.

For updating radiation based on flow-time, you must specify the Time Interval in seconds and Iteration Interval. The default value of 1 second for Time Interval means the radiation field will be updated once for every 1 second of flow time. The default Iteration Interval of 0 means the radiation field is only updated to satisfy the Time Interval condition. For example, a Time Interval of 2 seconds means the radiation field is updated after every 2 seconds of flow time. An Iteration Interval of 5 means the radiation field is updated every 5 iterations within a timestep.

Once the radiation problem has been set up, you can proceed as usual with the calculation. Note that while the P-1 and DO models will solve additional transport equations and report residuals, the DTRM and the Rosseland and S2S models will not (since they impact the solution only through the energy equation). Residuals for the DTRM and S2S model radiation iterations are reported by Ansys Fluent every time such an iteration is performed, as described below.

When running the S2S model with the parallel solver, note that coupled walls are encapsulated, which may cause problems with the partitioning of the mesh. See Troubleshooting for recommendations on correcting such problems.

 

16.3.9.7.3. Residual Reporting for the DTRM

Ansys Fluent does not include a DTRM residual in its usual residual report that is issued after each iteration. The effect of radiation on the solution can be gathered, instead, via its impact on the energy field and the energy residual. However, each time a DTRM iteration is performed, Ansys Fluent will print out the normalized radiation error for each DTRM radiation iteration. The normalized radiation error is defined as

(16–4)

where the error is the maximum change in the intensity () at the current radiation iteration, normalized by the maximum surface emissive power, and is the total number of radiating surfaces. Note that the default radiation convergence criterion, as noted in DTRM Solution Parameters, defines the radiation calculation to be converged when decreases to or less.

 

16.3.9.7.4. Residual Reporting for the S2S Model

Ansys Fluent does not include an S2S residual in its usual residual report that is issued after each iteration. The effect of radiation on the solution can be gathered, instead, via its impact on the energy field and the energy residual. However, each time an S2S iteration is performed, Ansys Fluent will print out the normalized radiation error for each S2S radiation iteration. The normalized radiation error is defined as

(16–5)

where the error is the maximum change in the radiosity () at the current radiation iteration, normalized by the maximum surface emissive power, and is the total number of radiating surface clusters. Note that the default radiation convergence criterion, as noted in DTRM Solution Parameters, defines the radiation calculation to be converged when decreases to or less.

Ansys Fluent provides radiation quantities that you can use in postprocessing when your model includes the solution of radiative heat transfer. You can generate graphical plots or alphanumeric reports of the following variables/functions:

In the Radiation... category:

In the Wall Fluxes... category:

See Field Function Definitions for definitions of these postprocessing variables. Note that in addition, incident radiation, transmitted, reflected and absorbed radiation flux are also available on a per-band basis for the non-gray DO model.

You can use the Flux Reports dialog box to compute the radiative heat transfer through each boundary of the domain, or to sum the radiative heat transfer through all boundaries.

 Results → Reports → Fluxes  Edit...

See Fluxes Through Boundaries for details about generating flux reports.

The DTRM yields a global heat balance and a balance of radiant heat fluxes only in the limit of a sufficient number of rays. In any given calculation, therefore, if the number of rays is insufficient you may find that the radiant fluxes do not obey a strict balance. Such imbalances are the inevitable consequence of the discrete ray tracing procedure and can be minimized by selecting a larger number of rays from each wall boundary.

When you use the DTRM, Ansys Fluent allows you to display surface or volume clusters, as well as the rays that emanate from a particular surface cluster. You can use the DTRM Graphics dialog box (Figure 16.45: The DTRM Graphics Dialog Box) for all of these displays.

 Results → Model Specific → DTRM Graphics...

Figure 16.45: The DTRM Graphics Dialog Box

 

16.3.10.4.2. Displaying Rays

To display the rays emanating from the surface cluster nearest to the specified point, select Ray under Display Type. Set the appropriate values for Theta and Phi Divisions under Ray Parameters (see Setting Up the DTRM for details), and then click the Display button. Figure 16.46: Ray Display shows a ray plot for a simple 2D geometry.

Figure 16.46: Ray Display

When you use the S2S model, Ansys Fluent allows you to view the values of the view factor and radiation emitted from one zone to any other zone. You can use the S2S Information dialog box (Figure 16.47: The S2S Information Dialog Box) to generate a report of these values in the console or as a separate file.

 Results → Model Specific → S2S Information...

Figure 16.47: The S2S Information Dialog Box

The steps for generating the report are as follows:

The following is an example of how the data is presented:

S2S Information
From wall1 to:
                    View factor       Incident Radiation
          wall1          0.0000                   0.0000
          wall2          0.2929              171387.7813
          wall3          0.2929              155305.7969
          wall4          0.4142               29055.9023

From wall2 to:
                    View factor       Incident Radiation
          wall1          0.2929              306451.9688
          wall2          0.0000                   0.0000
          wall3          0.4142              214195.0938
          wall4          0.2929               19153.2715

Note that the header listed above (S2S Information) is not displayed in the console.

Typical applications that are well-suited for solar load simulations include the following:

The effects of solar loading are needed in many ACC applications, where the temperature, humidity, and velocity fields around passengers (and drivers) are desired. ACC systems are tested for their capacity to cool down passenger compartments after they have been “soaked” in intense solar radiation. Ansys Fluent’s solar load model will enable you to simulate solar loading effects and predict the time it will take to reasonably cool down the cabin of a car that has been exposed to solar radiation, as well as predict the time interval needed to lower the temperature in specified points and areas within the domain.

In the analysis of buildings, solar loading provides a significant burden on the cooling requirement in warm climates, particularly where architects want to use the aesthetics of glazed facades. Even in cooler climates, solar loading can provide a burden during warmer seasons where modern buildings are well insulated against thermal loss during winter months. As well as providing an engineer with a practical tool for determining the solar heating effect inside a building, Ansys Fluent’s solar load model will allow the solar transmission through all glazed surfaces to be determined over the course of a day, allowing important decisions to be made before undertaking any flow studies. Ansys Fluent’s solar load model also allows you to simulate porous blinds, which can transmit a portion of the solar radiation while also allowing fluid flow.

The solar load model’s ray tracing algorithm can be used to predict the direct illumination energy source that results from incident solar radiation. It takes a beam that is modeled using the sun position vector and illumination parameters, applies it to any or all wall, porous jump, and inlet/outlet boundary zones that you specify, performs a face-by-face shading analysis to determine well-defined shadows on all boundary faces and interior walls, and computes the heat flux on the boundary faces that results from the incident radiation.

The resulting heat flux that is computed by the solar ray tracing algorithm is coupled to the Ansys Fluent calculation via a source term in the energy equation. The heat sources are added directly to computational cells bordering each face and are assigned to adjacent cells in the following order: shell conduction cells, solid cells, and fluid cells. Heat sources are assigned to one of these types of adjacent cells, only. You can choose to override this order and include adjacent fluid cells in the solar load calculation by issuing a command in the text user interface (see Text Interface-Only Commands for details). Note that the sun position vector and solar intensity can be entered either directly by you or computed from the solar calculator. Direct and diffuse irradiation parameters can also be specified using a user-defined function (UDF) and hooked to Ansys Fluent in the Radiation Model dialog box.

The solar ray tracing option allows you to include the effects of direct solar illumination as well as diffuse solar radiation in your Ansys Fluent model. A two-band spectral model is used for direct solar illumination and accounts for separate material properties in the visible and infrared bands. A single-band hemispherical-averaged spectral model is used for diffuse radiation. Opaque materials are characterized in terms of two-band absorptivities. A semi-transparent material requires specification of absorptivity and transmissivity. Values that you specify for transmissivity and absorptivity are defined for normal incident rays. Ansys Fluent recomputes/interpolates these values for the given angle of incidence.

The solar ray tracing algorithm also accounts for internal scattered and diffusive loading. The reflected component of direct solar irradiation is tracked. A fraction of this radiative heat flux, called internally scattered energy is applied to all the surfaces participating in the solar load calculation, weighted by area. The internally scattered energy depends on the scattering fraction that is specified in the TUI, whose default value is . Depending on the reflectivity of the primary surface, the scattering fraction can be responsible for the inclusion (or exclusion) of a large amount of radiation within the rest of the domain.

Also included as internally scattered energy is the contribution of the transmitted component of diffuse solar irradiation (which enters a domain through semi-transparent walls depending upon the hemispherical transmissivity). The total value of internally scattered energy is reported to the Ansys Fluent console. The ambient flux is obtained by dividing the internally scattered energy by the total surface area of the faces participating in the solar load calculation.

Note that Solar Ray Tracing is not a participating radiation model. It does not deal with emission from surfaces, and the reflecting component of the primary incident load is distributed uniformly across all surfaces rather than being local to the surfaces reflected to. If surface emission is an important factor in your case then you can consider implementing a radiation model (for example, P-1) in conjunction with Solar Ray Tracing.

Note the following limitation when using the solar ray tracing model:

 

16.3.11.2.2. Glazing Materials

Incident solar radiation can be applied to glass and plastic glazing materials of various types at wall boundaries, and the effects of coated glazings modeled using the solar ray tracing algorithm. To model solar optical properties, you will need to specify the transmissivity and reflectivity of the material in the Wall boundary conditions dialog box. You can obtain these values from the glass (or plastic) manufacturer or use data from another source (for example, ASHRAE Handbook).

Glazing optical properties are dependent on incident angle, and the variation is significant for an incident angle greater than degrees. As the incident angle increases from zero, transmissivity decreases, reflectivity increases, and absorptivity increases initially due to lengthened optical path, and then decreases as more incident radiation is reflected. The shape of the property curve varies with glass type and thickness. This difference is more pronounced for coated glass or for a multiple-pane glazing system. It cannot be assumed that all glazing systems have a universal angular dependence.

For coated glazings, the spectral transmissivity and reflectivity at any incident angle are approximated in the solar load model from the normal angle of incidence  [45].

Transmissivity is given by

(16–6)

where

(16–7)

Reflectivity is given by

(16–8)

where

(16–9)

The constants used in Equation 16–6 and Equation 16–8 are for coated glazings and are taken from Finlayson and Arasteh.  [45]. The normal transmissivity and reflectivity, and are specified in the Wall boundary conditions dialog box.

The solar load model’s Solar Irradiation option provides you with an easy means of applying a solar load directly to the DO or MC model. Unlike the ray tracing solar load option, the Solar Irradiation method does not compute heat fluxes and apply them as heat sources to the energy equation. Instead, the irradiation flux is applied directly to semi-transparent walls (which you specify) as a boundary condition, and the radiative heat transfer is derived from the solution of the radiation model itself.

The following inputs are required for Solar Irradiation at semi-transparent walls:

In the Wall boundary condition dialog box for each semi-transparent wall you want to participate in Solar Irradiation, you can specify that the beam direction, direct irradiation, and diffuse irradiation be derived from the solar parameters (for example, solar calculator) that you set (or compute) in the Radiation Model dialog box. This is done by checking the Use Beam Direction from Solar Load Model Settings and Use Irradiation from Solar Load Model Settings boxes. When selected, Ansys Fluent sets the beam width (the angle subtended by the sun) to the default value of degrees when using the DO model.

Ansys Fluent provides a solar calculator that can be used to compute solar beam direction and irradiation for a given time, date, and position. These values can be used as inputs to the solar ray tracing algorithm or as semi-transparent wall boundary conditions for solar irradiation.

 

16.3.11.4.2. Theory

Ansys Fluent provides two options for computing the solar load: Fair Weather Conditions method and Theoretical Maximum method. Although these methods are similar, there is a key difference. The Fair Weather Conditions method imposes greater attenuation on the solar load, which is representative of atmospheric conditions that are fair–but not completely clear.

The equation for normal direct irradiation applying the Fair Weather Conditions Method is taken from the ASHRAE Handbook:

(16–10)

where and are apparent solar irradiation at air mass and atmospheric extinction coefficient, respectively. These values are based on the earth’s surface on a clear day. is the solar altitude (in degrees) above the horizontal.

The equation for direct normal irradiation that is used for the Theoretical Maximum Method is taken from NREL’s Solar Position and Intensity Code (Solpos):

(16–11)

where is the top of the atmosphere direct normal solar irradiance and is the correction factor used to account for reduction in solar load through the atmosphere.

The calculation for the diffuse load in the solar model is based on the approach suggested in the 2001 ASHRAE Fundamental Handbook (Chapter 20, Fenestration). The equation for diffuse solar irradiation on a vertical surface is given by:

(16–12)

where is a constant whose values are given in Table 7 from Chapter 30 of the 2001 ASHRAE Handbook of Fundamentals, is the ratio of sky diffuse radiation on a vertical surface to that on a horizontal surface (calculated as a function of incident angle), and is the direct normal irradiation at the earth’s surface on a clear day.

The equation for diffuse solar irradiation for surfaces other than vertical surfaces is given by:

(16–13)

where is the tilt angle of the surface (in degrees) from the horizontal plane.

The equation for ground reflected solar irradiation on a surface is given by:

(16–14)

where is the ground reflectivity. The total diffuse irradiation on a given surface will be the sum of and when the input for diffuse solar radiation is taken from the solar calculator. Otherwise, if the constant option is selected in the Radiation dialog box, then the total diffuse irradiation will be the same as specified in the dialog box.

When you want to run a steady-state solution with solar load enabled, you simply set up the solar load model (Setting Up the Solar Load Model) and boundary conditions (Setting Boundary Conditions for Solar Loading) for your case, and then run the simulation. The solution data file will contain the solar fluxes that you can use for postprocessing. For a steady-state solution, the solar loads are computed on initialization. If you want to initially solve a case without solar loading (say, for stability) and then add the effects of solar loading afterward, you will need to enable the solar load model through the text user interface (TUI).

When you want to run a transient solar load simulation, the process is the same as for the steady-state case but you will need to specify the additional Time Steps per Solar Load Update parameter in the Radiation Model dialog box. Ansys Fluent will re-compute the sun position and irradiation and update solar loads with this specified frequency.

 

16.3.11.5.2. Setting Up the Solar Load Model

The solar load model is enabled in the Radiation Model dialog box (Figure 16.48: The Radiation Model Dialog Box).

 Setup → Models → Radiation  Edit...

Figure 16.48: The Radiation Model Dialog Box

---

Important:  Solar load is available in the 3D solver only, and can be used to model steady and unsteady flows.

---

The solar load model has two options: Solar Ray Tracing and Solar Irradiation. Solar Ray Tracing can be applied as a stand-alone solar loading model, or it can be used in conjunction with one of the Ansys Fluent radiation models. Solar Irradiation is available only when the Discrete Ordinates (DO) or Monte Carlo (MC)radiation model is enabled.

To set up the solar load model, perform the following steps:

1. Enable the solar load model in the Radiation Model Dialog Box.

   1. To enable the solar ray tracing algorithm, select Solar Ray Tracing under Solar Load (Figure 16.49: The Radiation Model Dialog Box (With Solar Load Model Solar Ray Tracing Option)).

      Figure 16.49: The Radiation Model Dialog Box (With Solar Load Model Solar Ray Tracing Option)

      
      
      

   2. To enable the Solar Irradiation option, first select the DO or MC model, and then select Solar Irradiation under Solar Load (Figure 16.50: The Radiation Model Dialog Box (with Solar Load Model Solar Irradiation Option)).

      Figure 16.50: The Radiation Model Dialog Box (with Solar Load Model Solar Irradiation Option)

      
      
      

2. When using the non-gray DO or MC model, if the wavelengths of the specified bands do not cover the entire solar spectrum, a message is written to the console displaying what percentage of the full solar model has been covered. It is recommended that the full solar spectrum is considered.

   When using the non-gray MC model, if you only specify one band then Fluent will automatically cover the entire solar spectrum

3. Define the solar parameters.

   1. Enter values for the X, Y, and Z components of the Sun Direction Vector. Alternatively, you can choose to have this vector computed from the solar calculator by enabling the Use Direction Computed from Solar Calculator option.

   2. Specify the illumination parameters.

      1. Enter a value for Direct Solar Irradiation under Illumination Parameters. This parameter is the amount of energy per unit area in due to direct solar irradiation. This value may depend on the time of year and the clearness of the sky. Make your selection in the drop-down list next to Direct Solar Irradiation and either enter a constant value, have the value computed from the solar calculator, or specify it using a user-defined function. Note that only compiled (not interpreted) UDFs can be used to specify Direct Solar Irradiation. (For more information on writing solar intensity UDFs, see DEFINE_SOLAR_INTENSITY in the Fluent Customization Manual.) For transient simulations, you have the additional option of specifying a time-dependent piecewise-linear and polynomial profile for direct solar irradiation.

      2. Enter a value for Diffuse Solar Irradiation for the DO model only, which is the amount of energy per unit area in due to diffuse solar irradiation. This value may depend on the time of year, the clearness of the sky, and also on ground reflectivity. Make your selection in the drop-down list next to Diffuse Solar Irradiation and either enter a constant value, have the value computed from the solar calculator, or specify it using a user-defined function. Note that only compiled (not interpreted) UDFs can be used to specify Diffuse Solar Irradiation. (For more information on writing solar intensity UDFs, see DEFINE_SOLAR_INTENSITY in the Fluent Customization Manual.) For transient simulations, you have the additional option of specifying a time-dependent piecewise-linear and polynomial profile for diffuse solar irradiation.

      3. If you are using the Solar Ray Tracing solar load model (Figure 16.49: The Radiation Model Dialog Box (With Solar Load Model Solar Ray Tracing Option)), then you will need to enter a value for Spectral Fraction. The spectral fraction is the fraction of incident solar radiation in the visible part of the solar radiation spectrum.

         (16–15)

         where is the visible incident solar radiation, and is the total incident solar radiation (visible plus infrared).

4. Use the solar calculator to compute solar beam direction and irradiation.

   1. Click Solar Calculator... in the Radiation Model dialog box to open the Solar Calculator dialog box (Figure 16.51: The Solar Calculator Dialog Box).

      Figure 16.51: The Solar Calculator Dialog Box

      
      
      

   2. In the Solar Calculator dialog box, define the Global Position by the following parameters:

      1. Enter a real number in degrees for Longitude. Values may range from to where negative values indicate the Western hemisphere and positive values indicate the Eastern hemisphere.

      2. Enter a real number for Latitude in degrees. Values can range from (the South Pole) to (the North Pole), with defined as the equator.

      3. Enter an integer for Timezone that is the local time zone in hours relative to Greenwich Mean Time (+-GMT). This value can range from to .

      ---

      Important:  Note that you must specify all three Global Position parameters for the solar calculator.

      ---

   3. Define the local Date and Time by the following parameters:

      1. Enter an integer for Day and Month under Day of Year.

      2. Enter an integer for Hour that ranges from to under Time of Day. Enter an integer or floating point number for Minute.

         The time of day is based on a 24-hour clock: hours and minutes corresponds to 12:00 a.m. and hours min corresponds to 11:59.99 p.m. For example, if the local time was 12:01:30 a.m., you would enter 0 for Hour and 1.5 for Minute. If the local time was 4:17 p.m., you would enter 16 for Hour and 17 for Minute.

   4. Define the Mesh Orientation as the vectors for North and East in the CFD mesh system of coordinates.

   5. Select the appropriate Solar Irradiation Method. The Fair Weather Conditions is the default method.

   6. Enter an integer for Sunshine Fraction (default = ).

   7. Click Apply.

      The solar calculator output parameters are computed and the results are reported in the console. The default values are shown below:

       Fair Weather Conditions:
        Sun Direction Vector: X: -0.0785396, Y: 0.170758, X: 0.982178
        Sunshine Fraction: 1
        Direct Normal Solar Irradiation (at Earth’s surface) [W/m^2]:
        881.635
        Diffuse Solar Irradiation - vertical surface: [W/m^2]:
        152.107
        Diffuse Solar Irradiation - horizontal surface: [W/m^2]:
        118.727
        Ground Reflected Solar Irradiation - vertical surface: [W/m^2]:
        96.4649 
      

5. For transient simulations, enter the Time Steps Per Solar Load Update under Update Parameters. The number of time steps that you specify will direct the Ansys Fluent solver to update the solar load data for the specified flow-time intervals in the unsteady solution process.

 /define/models/radiation/solar-parameters> autosave-solar-data
  Autosave Solar Data File Frequency [0] 1
  Enter Filename [""] "solar" 

 /define/models/radiation/solar-parameters> autoread-solar-data
  Autoread Solar Data File Frequency [0] 1
  Enter Filename [""] "solar"
  Use Binary Format for Reading Data Files [yes]  

 /define/models/radiation/solar-parameters> scattering-fraction
  Scattering Fraction [1] .5 

 /define/models/radiation/solar-parameters> sol-adjacent-fluidcells
  Apply Solar Load on adjacent Fluid Cells? [no] y 

 /define/models/radiation/solar-parameters> quad-tree-parameters
  Maximum Quad-Tree Refinement [7] 10 

 /define/models/radiation/solar-parameters> ground-reflectivity
  Ground Reflectivity [0.2] 0.5 

  /define/models/radiation/apply-full-solar-irradiation?
Apply full solar irradiation to first band? [no] yes

The following solar load quantities can be used to visualize the illuminated areas and shadows created by solar radiation.

These quantities are available for postprocessing of solar loading at wall boundaries and can be displayed as contours of Wall Fluxes in the Contours dialog box. For steady-state simulations, the solar flux data is computed at solution initialization and is available for postprocessing. You can also compute the solar load at any time during your Ansys Fluent session, after you have set up the model and applied boundary conditions. To compute the solar load on demand, you can issue the sol-on-demand command in the text interface (see Additional Text Interface Commands for details).

Solar heat flux, for example, can be displayed for surfaces using the Contours dialog box. A sample dialog box is shown below (Figure 16.57: The Contours Dialog Box).

 Results → Graphics → Contours  New...

Figure 16.57: The Contours Dialog Box

 

16.3.11.6.1. Solar Load Animation at Different Sun Positions

The solar camera alignment command is useful when you want to take timed pictures of solar loading effects of your model during transient simulations, and later create animations of the image files using an external program. Follow the procedure below.

1. Read (or set up) your transient case file in Ansys Fluent.

2. Set up the automatic execution of solution commands in the Execute Commands dialog box that will: 1) display solar load parameter graphics, 2) re-position the solar camera such that the view is aligned with the instantaneous sun direction, and 3) generate a picture image file (.tiff) during the solution process in the Execute Commands dialog box.

    Solution → Calculation Activities → Execute Commands  Edit...

3. Initialize and run the solution.

4. Animate the .tiff files using an external animation tool.

The following commands entered in the Execute Commands dialog box will direct Ansys Fluent to display contours of solar heat flux, align the camera with the current direction of the sun, and then generate a picture image file (.tiff) of the solar heat flux contour every 300 time steps during the unsteady simulation. See Figure 16.58: The Execute Commands Dialog Box.

 /di/cont solar-heat-flux ,,
 /def/mod/rad/solar-para/sol-camera-pos
 /di/hc "flux-%t.tiff" 

Figure 16.58: The Execute Commands Dialog Box