13.3.3 Setting Up the S2S Model

When you select the Surface to Surface (S2S) model, the Radiation Model dialog box will expand to show additional parameters (see Figure  13.3.3). In this section of the dialog box, you will compute the view factors for your problem, read previously computed view factors into ANSYS FLUENT, or set view factor parameters.

Figure 13.3.3: The Radiation Model Dialog Box (S2S Model)

The S2S radiation model is computationally very expensive when there are a large number of radiating surfaces. To reduce the memory requirement for the calculation, the number of radiating surfaces is reduced by creating surface clusters. The surface cluster information (coordinates and connectivity of the nodes, surface cluster IDs) is used by ANSYS FLUENT to compute the view factors for the surface clusters.

You should recreate the surface cluster information whenever you do anything that changes the mesh, such as: change the type of a boundary zone reorder the mesh scale the mesh Note that you do not need to recalculate view factors after shell conduction at any wall has been enabled or disabled. See Section  7.3.14 for more information about shell conduction.

ANSYS FLUENT will warn you to recreate the cluster/view factor file if a boundary zone has been changed from a wall to an internal wall (or visa versa), or if a boundary zone has been merged, separated, or fused.

Computing View Factors

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. Alternatively, you can save the surface cluster information and view factor parameters to a file, calculate the view factors outside ANSYS FLUENT, and then read the view factors into ANSYS FLUENT. These methods for computing view factors are described below.

For large meshes or complex models, it is recommended that you calculate the view factors outside ANSYS FLUENT and then read them into ANSYS FLUENT before starting your simulation.

Computing View Factors Inside ANSYS FLUENT

To compute view factors in your current ANSYS FLUENT session, you must first set the parameters for the view factor calculation in the View Factor and Cluster Parameters dialog box (see below for details). When you have set the view factor and surface cluster parameters, click Compute/Write... under Methods in the Radiation Model dialog box. A Select File dialog box will open, prompting you for the name of the file in which ANSYS FLUENT should save the surface cluster information and the view factors. After you have specified the file name, ANSYS FLUENT will write the surface cluster information to the file. ANSYS FLUENT will use 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 viewfactors

Completed 50% calculation of viewfactors

Completed 75% calculation of viewfactors

Completed 100% calculation of viewfactors

The view factor file format for this version of ANSYS FLUENT is known as the compressed row format (CRF) which is a more efficient way of writing view factors than in prior versions of ANSYS FLUENT. In the CRF format, only non-zero view factors with their associated cluster IDs are stored to the file. This reduces the size of the .s2s file, and reduces the time it takes to read the file into ANSYS FLUENT. While the CRF file format is the default, you can still use the older file format if necessary. Contact your support engineer for more information.

Computing View Factors Outside ANSYS FLUENT

To compute view factors outside ANSYS FLUENT, you must save the surface cluster information and view factor parameters to a file.

File $\rightarrow$ Write $\rightarrow$ Surface Clusters...

ANSYS FLUENT will open the View Factor and Cluster Parameters dialog box, where you will set the view factor and surface cluster parameters (see below for details). When you click OK in the View Factor and Cluster Parameters dialog box, a Select File dialog box will open, prompting you for the name of the file in which ANSYS FLUENT should save the surface cluster information and view factor parameters. After you have specified the file name, ANSYS FLUENT will write the surface cluster information and view factor parameters to the file. If the specified Filename ends in .gz or .Z, appropriate file compression will be performed.

To calculate the view factors outside ANSYS FLUENT, enter one of the following commands:

• For the serial solver:
  utility viewfac inputfile
  where inputfile is the filename, or the correct path to the filename, for the surface cluster information and view factor parameters file that you saved from ANSYS FLUENT. You can then read the view factors into ANSYS FLUENT, as described below.

• For the network parallel solver:
  utility viewfac -cnf= host1,host2, $\dots$,host $n$ inputfile
  where $n$ is the number of compute nodes, and host1, host2, $\dots$ are the names of the machines being used.

• For a dedicated parallel machine with multiple processors:
  utility viewfac -t $n$ inputfile

Reading View Factors into ANSYS FLUENT

If the view factors for your problem have already been computed (either inside or outside ANSYS FLUENT) and saved to a file, you can read them into ANSYS FLUENT. To read in the view factors, click Read... under Methods in 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. You can also manually specify the view factors file, using the File/Read/View Factors... menu item.

While the previous .s2s view factor file format can still be read seamlessly into ANSYS FLUENT, there is now a more efficient compressed row format (CRF) that can be read into ANSYS FLUENT (see the section on Computing View Factors Inside ANSYS FLUENT). You can take advantage of the reduced size of the CRF file and thus the reduced time it takes to read the file into ANSYS FLUENT, by converting the existing old file format to the new format (without having to recompute the view factors) using the following command at the command prompt in your working directory: utility viewfac -c1 -o new.s2s.gz old.s2s.gz where new.s2s.gz is the CRF format to which you want the old file format ( old.s2s.gz) converted.

Setting View Factor and Surface Cluster Parameters

You can use the View Factor and Cluster Parameters dialog box (Figure  13.3.4) to set view factor and cluster parameters for the S2S model. To open this dialog box, click Set... under Parameters in the Radiation Model dialog box (Figure  13.3.3) or use the File/Write/Surface Clusters... menu item.

Figure 13.3.4: The View Factor and Cluster Parameters Dialog Box

Forming Clusters

There are two methods of forming clusters:

• manual

• automatic

If you select Manual in the Options group box, you will need to specify the Faces per Surface Cluster for Flow Boundary Zones value in the Parameters group box and then click Apply to All Walls, thus applying this value to all the walls. For those walls (or critical zones) which require a lower Faces per Surface Cluster for Flow Boundary Zones value, you will need to go into the boundary condition dialog box of that particular wall and modify the value. All the other (non-critical) zones will have one specific Faces per Surface Cluster value, depending on the clustering method used (Figure  13.3.5). Similarly, if you want to set a higher Faces per Surface Cluster value for a certain non-critical zone, then you will need to visit that particular boundary condition dialog box and increase the value. This process can become very cumbersome if the model involves a large number of radiating faces, which is typically the case in typical underhood models. To address this drawback, use the automatic clustering option, by selecting Automatic in the Options group box. Here, rather than having the same faces per surface cluster (FPSC) value, or having to specify different values by manually visiting the boundary condition dialog boxes, the automatic FPSC calculation calculates FPSC values based on the distance of the zones from the other critical zones. The step you will need to take are as follows:

1.   Define the critical zone and enter the Minimum Faces per Surface Cluster value in the in Radiation tab of the boundary condition dialog box for that zone.

2.   Enter the Maximum Faces per Surface Cluster value in the View Factor and Cluster Parameters dialog box and click the Compute button. ANSYS FLUENT will automatically calculate and update the FPSC values in the boundary conditions dialog box without computing the clusters.

3.   After you are satisfied with the FPSC values, then you can compute the clusters and the view factors.

Controlling the Clusters

Your input for Faces Per Surface Cluster for Flow Boundary Zones will control the number of radiating surfaces. By default, it is set to $1$, so the number of surface clusters (radiating 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 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. (See this section in the separate Theory Guide for details about clustering.)

There are certain applications that will require most or all wall boundary zones to have the same Faces Per Surface Cluster for Flow Boundary Zones. In typical underhood simulations, for example, there can be hundreds of walls to which you want to apply the same Face Per Surface Cluster for Flow Boundary Zones. To avoid visiting each Wall boundary condition dialog box, you can instead click the Apply to All Walls button in the View Factor and Cluster Parameters dialog box (Figure  13.3.4). Once you click OK, the Faces Per Surface Cluster for Flow Boundary Zones value you specify will be copied to all wall zones that are adjacent to fluid zones in your model. You can then visit only the walls you want to define different settings for and set those parameters individually.

The Faces Per Surface Cluster can be designated for a particular wall in the Wall boundary condition dialog box under the Radiation tab (Figure  13.3.5). Under the Radiation tab, you can also choose to exclude a particular wall from the radiosity calculations by deselecting Participates in S2S Radiation. Note that if the surface clusters are written with this feature turned off, then the view factors will not be computed at all for that particular wall. If you are unsure whether a wall is radiating or not ahead of time, then you should keep the Participates in S2S Radiation enabled and have the view factors computed. You can always toggle the switch at a later stage to include or exclude the particular wall for radiosity calculations.

The Faces Per Surface Cluster and Participates in S2S Radiation controls will not be visible in the GUI on wall boundary zones that are attached to a solid.

Figure 13.3.5: The Wall Dialog Box

In some cases, you may wish to modify 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 surfaces 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 $^{\circ}$. To modify the value of this parameter, you can use the split-angle text command:

define $\rightarrow$ models $\rightarrow$ radiation $\rightarrow$ s2s-parameters $\rightarrow$ split-angle

or

file $\rightarrow$ write-surface-clusters $\rightarrow$ split-angle

Radiating Zones

There are two ways in which you can enable/disable participation of S2S radiation. One of those ways is to use the Participates in S2S Radiation option in the Radiation tab of the boundary condition dialog box. The other method, is to go to the Select Radiating Boundary Zones dialog box (Figure  13.3.6) which is accessed by clicking the Select... button under Radiating Zones in the View Factor and Cluster Parameters dialog box. In cases comprising a very large number of zones, such as underhood applications, you would want to use the latter method if you want to include or exclude participation of S2S radiation.

Figure 13.3.6: The Select Radiating Boundary Zones Dialog Box

The Select Radiating Boundary Zones dialog box allows you to easily specify those zones that are participating or non-participating without having to visit each zone in the boundary conditions dialog box. The process of zone selection can also be automated by automatically moving the zones which are greater than a certain distance (user-input) to a non-participating zones list. Furthermore, you can also display the zones which are only participating, or only non-participating, or a mixture of both, or any other combination with a few simple actions.

In the Select Radiating Boundary Zones dialog box

Compute   calculates the distance from the critical zone to all the other zones and displays it in the Maximum of distances between Critical Zone and other Zones field and the Maximum distance of Participating Zone from Critical Zone field. It requires the definition of the critical zone.

Maximum of distances between Critical Zone and other Zones   displays the maximum of the distances between critical and other zones (non-editable). This is available when using the Automatic option for clustering.

Maximum distance of Participating Zone from Critical Zone   displays the maximum distance (similar to the Maximum of distances between Critical Zone and other Zones when Compute is clicked). You can edit this field. You will enter a distance, such that all the zones having a distance from the critical zone greater than the specified distance will be made non-participating and will therefore be placed in the non-participation boundary list. Note that this field is available when using the Automatic option for clustering.

All the distances are calculated based on the centroid of the zone.

If the Manual option is selected in the View Factor and Cluster Parameters dialog box, then Maximum of distances between Critical Zone and other Zones and Maximum distance of Participating Zone from Critical Zone will not be available because they require the definition of a critical zone which is only available when the Automatic option is selected in the View Factor and Cluster Parameters dialog box. However, if you want to perform clustering manually, but still want to select the zones based on automatic selection, then you can briefly switch to the Automatic option in the View Factor and Cluster Parameters dialog box. You can now define the critical zones and select zones based on distance criteria. After the zones are selected, you can switch back to the manual method of clustering.

Apply   is similar to the Compute button in that it actually calculates the Maximum distance of Participating Zone from Critical Zone and moves the zones to the Non-Participating Boundary Zones list.

Participating Boundary Zones   shows all the participating zones.

Non-Participating Boundary Zones   shows all the non-participating zones.

Display Zones   allows you to display all participating zones, non-participating zones, or a mixture of both to find out visually if you have missed any zones.

OK   stores all the settings and closes the Select Radiating Boundary Zones dialog box.

Specifying the Orientation of Surface Pairs

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 "non-blocking'' 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 under Surfaces in the View Factor and Cluster Parameters dialog box. For cases with non-blocking 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.

Selecting the Method for Smoothing

In order to enforce reciprocity and conservation (see this section in the separate Theory Guide), smoothing can be performed on the view factor matrix. To use the least-squares method for smoothing of the view factor matrix, select Least Squares under Smoothing in the View Factor and Cluster Parameters dialog box. If you do not wish to smooth the view factor matrix, select None under Smoothing.

Selecting the Method for Computing View Factors

ANSYS FLUENT provides three methods for computing view factors: the adaptive method, the hemicube method, and the ray tracing method. The following limitations apply:

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

• The ray tracing method should not be used when any of the zones are defined as periodic, as this type of zone is not currently supported.

The adaptive method calculates the view factors on a pair-by-pair basis using a variety of algorithms (analytic or Gauss quadrature) that are chosen adaptively depending on the proximity of the surfaces. To maintain accuracy, the order of the quadrature increases the closer the faces are together. For surfaces that are very close to each other, the analytic method is used. ANSYS FLUENT determines the method to use by performing a visibility calculation. The Gaussian quadrature method is used if none of the rays from a surface are blocked by the other surface. If some of the rays are blocked by the other surface, then either a Monte Carlo integration method or a quasi-Monte Carlo integration method is used.

To use the adaptive method to compute the view factors, select Adaptive in the View Factor and Cluster Parameters dialog box. It is recommended that you use the adaptive method for simple models, because it is the fastest method under such circumstances. As the complexity and size of the geometry grows, however, you should consider using either the hemicube or ray tracing methods.

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 [ 16].

To use the hemicube method to compute the view factors, select Hemicube in the View Factor and Cluster Parameters dialog box. It is recommended that you use the hemicube method for large, complex models with few obstructing surfaces between the radiating surfaces, because it is faster than the adaptive method or ray tracing method for these types of models.

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 over- or under-estimated. Aliasing effects can be reduced by increasing the value of the Resolution of the hemicube under Hemicube Parameters.

• Visibility--The visibility between any two faces does not change. In some cases, face $i$ has a complete view of face $k$ from its centroid, but some other face $j$ occludes much of face $k$ from face $i$. In such a case, the hemicube method will overestimate the view factor between face $i$ and face $k$ calculated from the centroid of face $i$. This error can be reduced by subdividing face $i$ into smaller subfaces. You can specify the number of subfaces by entering a value for Subdivisions under Hemicube Parameters.

• 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 non-linear, the result is a poor estimate of the view factor.

  Under Hemicube Parameters, 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. Also, the ray tracing method is OpenMP parallelized and will therefore use all available processors when performing the ray tracing calculations (for further details, visit http://www.openmp.orgwww.openmp.org). As a result, the calculation time is reduced for large, complex geometries that have obstructions between the radiating surfaces (such as automotive underhood simulations). 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 in the View Factor and Cluster Parameters dialog box. You can adjust the value of the Resolution in the Hemicube Parameters group box in order to reduce the impact of aliasing effects, as described previously.