When you select the Surface to Surface (S2S) model, the Radiation Model dialog box will expand to show additional parameters (see Figure 12.14: The Radiation Model Dialog Box (S2S Model)). In these additional group boxes, you will set the solution parameters (see S2S Solution Parameters for further details), access the view factors and clustering settings, and compute the view factors for your problem or read previously computed view factors into ANSYS Fluent.
The S2S radiation model is very expensive in terms of computation effort and memory requirements when there are a large number of radiating surfaces. You can reduce the number of radiating surfaces by grouping faces together to form surface clusters. The surface cluster information (coordinates and connectivity of the nodes, surface cluster IDs) is used by ANSYS Fluent in the radiosity calculations and to compute the view factors.
You must recreate the surface cluster information whenever you do anything that changes the mesh, such as:
change the type of a boundary zone
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 Thermal Boundary Conditions at Walls for more information about shell conduction). However, enabling or disabling shell conduction in the parallel version of Fluent does cause a migration of cells and hence a change in the partition. Whenever there is cell migration, the previously read view factor file is no longer valid, and the view factor file must be read again using either the button in the Radiation Model dialog box or the File/Read/View Factors... ribbon tab item.
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 vice versa), or if a boundary zone has been merged, separated, or fused.
You can use the View Factors and Clustering dialog box (Figure 12.15: 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 12.14: The Radiation Model Dialog Box (S2S Model)) or use the File/Write/Surface Clusters... ribbon tab item.
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 12.15: 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 12.16: 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.
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.
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:
Select Automatic from the Options list in the View Factors and Clustering dialog box.
For each wall that you deem critical, perform the following actions in the Wall dialog box (Figure 12.16: The Wall Dialog Box):
Click the Radiation tab.
Enter an appropriate value for Faces Per Surface Cluster in the S2S Parameters group box.
Enable the Critical Zone option.
Click to close the Wall dialog box.
Enter the Maximum Faces per Surface Cluster value in the View Factors and Clustering dialog box and click the 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.
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.
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
or
file →
write-surface-clusters →
split-angle
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 12.15: The View Factors and Clustering Dialog Box), and are described in the sections that follow.
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 the cluster to cluster basis with non-conformal interfaces, the Faces Per Surface Cluster will be limited to one, giving no advantage to the cluster to cluster basis.
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, 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 [22].
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.
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.
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 12.17: The Participating Boundary Zones Dialog Box), which is accessed by clicking the 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.
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:
Make sure that your clustering options (see Forming Surface Clusters) are appropriate for your view factor settings:
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.
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.
Click the 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.
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 button to move all zones beyond this distance into the Non-Participating Boundary Zones list.
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 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 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. 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 in the following sections.
Important: 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.
Note: You can accelerate view factor calculations by using ANSYS Fluent in parallel. For more information see Accelerating View Factor Calculations for General Purpose Computing on Graphics Processing Units (GPGPUs).
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 to save them. When you have set the view factor and surface cluster parameters, click the 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 in which ANSYS Fluent should save the surface cluster information and the view factors. Note that the option to Write Binary Files is enabled by default, in order to reduce the time needed to write and read the view factor files. When you click in the Select File dialog box, 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 view factors Completed 50% calculation of view factors Completed 75% calculation of view factors Completed 100 % calculation of view factors
You must recompute the view factors if you take any of following actions after the initial computation:
if you alter which boundary zones participate in the view factor calculation (either by using the Participating Boundary Zones dialog box, or by enabling / disabling the Participates in View Factor Calculation option in the Radiation tab of the boundary condition dialog box)
if you scale or unscale the mesh by using the Scale Mesh dialog box
The view factor file format for this version of
ANSYS Fluent is known as the compressed row format (CRF) and is
a more efficient way of writing view factors than in versions
that are prior to Fluent 6.4. In the CRF format, only nonzero
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.
View factors using ray tracing are computed with the MPI/OpenMP hybrid model for parallel runs. By default, one OpenMP thread is used per MPI process, as specified in the Thread Control Dialog Box (see Controlling the Threads for details). To use all the available cores on your machine as OpenMP threads, select Number of Cores on Machine. A Fixed Number of cores can also be used based on your needs.
Note: For cases that use the S2S model and contain non-conformal interfaces, if the mesh interfaces are defined after the case has been read, then the intersection of the interface zones will occur during the initialization process, which will cause relabeling of faces throughout the domain. If you attempt to compute view factors before solution initialization in such a case, then the following message will be displayed in the console and the view factors will be computed automatically during solution initialization to avoid a mismatch with the case file:
Intersection zones for non-conformal interfaces are not created. View factors will be computed during solution initialization.
To compute view factors outside ANSYS Fluent, you must save the surface cluster information and view factor parameters to a file.
File → Write
→ Surface Clusters...
ANSYS Fluent will open the View Factors and
Clustering dialog box, where you will set the view factor and
surface cluster parameters (see View Factors and Clustering Settings for details). When you click in the
View Factors and Clustering 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 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 parallel solver:
Viewfac utility module:
utility viewfac -t
nprocs
[-p
interconnect
] [-mpi=
mpi_type
] [-cnf=
hosts
]
inputfile
where inputfile is the filename, for which you will need to provide the full path.
Raytracing utility module:
utility raytracing -t
nprocs
[-p
interconnect
] [-mpi=
mpi_type
] [-cnf=
hosts
]
[-ompthreads=
N
]
inputfile
where inputfile is the filename, for which you will need to provide the full path.
| On Windows: |
-tnprocs specifies
the number of processes to use. When the
-cnf option is present, the hosts
file argument is used to determine which machines to use for the
parallel job. For example, if there are 8 machines listed in the
hosts file and you want to run a job with 4 processes, set
nprocs to 4 (that is
-t4) and ANSYS Fluent will use the
first 4 machines listed in the hosts file. Note that this does
not apply to the Compute Cluster Server (CCS). |
-pinterconnect
(optional) specifies the type of interconnect. The ethernet
interconnect is used by default if the option is not explicitly
specified. See Table 34.2: Supported Interconnects for the Windows Platform,
Table 34.3: Available MPIs for Windows Platforms, and
Table 34.4: Supported MPIs for Windows Architectures (Per Interconnect) for more
information. |
-mpi=mpi_type
(optional) specifies the type of MPI. If the option is not
specified, the default MPI for the given interconnect (IBM MPI)
will be used (the use of the default MPI is recommended). The
available MPIs for Windows are shown in Table 34.3: Available MPIs for Windows Platforms. |
-cnf=hosts
(optional) specifies the hosts file, which contains a list of
the machines on which you want to run the parallel job. This
option functions the same as that in the command for launching
parallel Fluent; see Starting Parallel ANSYS Fluent on a Windows System Using Command
Line Options for
details. |
-ompthreads=N
(optional) specifies that the desired number of OpenMP threads
to be used per machine is N. |
| On Linux: |
-tnprocs specifies
the number of processes to used. When the
-cnf option is present, the hosts
file argument is used to determine which machines to use for the
parallel job. For example, if there are 10 machines listed in
the hosts file and you want to run a job with 5 processes, set
nprocs to 5 (that is
-t5) and ANSYS Fluent will use the
first 5 machines listed in the hosts file. |
-pinterconnect
(optional) specifies the type of interconnect. The ethernet
interconnect is used by default if the option is not explicitly
specified. See Table 34.5: Supported Interconnects for Linux Platforms (Per Platform),
Table 34.6: Available MPIs for Linux Platforms, and Table 34.7: Supported MPIs for Linux Architectures (Per Interconnect) for more
information. |
-mpi=mpi_type
(optional) specifies the type of MPI. If the option is not
specified, the default MPI for the given interconnect will be
used (the use of the default MPI is recommended). The available
MPIs for Linux are shown in Table 34.6: Available MPIs for Linux Platforms. |
-cnf=hosts
(optional) specifies the hosts file, which contains a list of
the machines on which you want to run the parallel job. This
option functions the same as that in the command for launching
parallel Fluent; see Starting Parallel ANSYS Fluent on a Linux System Using Command
Line Options for
details. |
-ompthreads=N
(optional) specifies that the desired number of OpenMP threads
to be used per machine is N. |
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 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. Alternatively, you can read the view factors file using the File/Read/View Factors... ribbon tab item.
Important: 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 therefore 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.