In order to partition the mesh, you must select the partition method for creating the mesh partitions, set the number of partitions, select the zones and/or registers, and choose the optimizations to be used. For some methods, you can also perform pretesting to ensure that the best possible partition is performed. Once you have set all the parameters in the Partitioning and Load Balancing dialog box to your satisfaction, click the button to subdivide the mesh into the selected number of partitions using the prescribed method and optimization(s). For recommended partitioning strategies see Guidelines for Partitioning the Mesh.
You can set the relevant inputs in the Partitioning and Load Balancing dialog box (Figure 34.7: The Partitioning and Load Balancing Dialog Box) in the following manner:
Parallel → General → Partition/Load Balance...
Select the Method from the drop-down list. The choices are described in Partition Methods.
In the Options tab
Set the desired number of mesh partitions in the Number of Partitions field. You can use the counter arrows to increase or decrease the value, instead of typing in the box. The number of mesh partitions must be an integer number that is divisible by the number of processors available for parallel computing.
Set the Reporting Verbosity. This allows you to control what is displayed in the console. For details, see Reporting During Partitioning.
By default, partitioning will be done across cell zones. You can choose to independently apply partitioning to each cell zone, by disabling Across Zones. This is not recommended unless cells in different zones will require significantly different amounts of computation during the solution phase (for example, if the domain contains both solid and fluid zones).
If you are using the Metis method, you have the option of enabling Laplace Smoothing. This option can be used to prevent partition boundaries from passing through areas of high aspect ratio cells. This can improve convergence in dynamic mesh cases and other cases with regions of highly stretched cells. After enabling Laplace Smoothing, you can specify the Cutoff Aspect Ratio. The Cutoff Aspect Ratio corresponds roughly to the maximum aspect ratio allowable along a partition boundary.

Select the Reordering Method for partitions to optimize parallel performance:
Architecture Aware: This is the default option and it accounts for the system architecture and network topology in remapping the partitions to the processors.
Reverse Cuthill-McKee: This option minimizes the bandwidth of the compute-node connectivity matrix (the maximum distance between two connected processes) without incorporating the system architecture.
The reordering methods are parallel performance tuning options. After the case is initially partitioned for parallel processing, the partition reordering step will remap the partitions in a more optimal way to improve parallel performance.
Important: The Architecture-aware reordering method is not applicable when only a single machine is used for the simulation.
After initially loading the case into a parallel session, you can click the button to reorder the partitions. The necessary algorithms are executed and ANSYS Fluent will report if it can find a more optimal mapping for the partitions, as well as the potential improvement in inter-machine communications. If the reported improvement is significant (say, more than 5%), then you can click the button to use the new partition mapping. This will generally entail large data transfers amongst all the processes, and another reliable method to use the new partitions would be to write out a case file and load it back in to a new parallel session. The process is similar to re-partitioning with a new partitioning method, for example. Note that sometimes, depending on the cluster configuration and initial case partitioning, and if the partitions have already been reordered, no improvement is possible, and this will be reported in the console after clicking the button. You can simply continue in this case, and there will be no effect on the simulation. Also, note that partition reordering is specific to the current parallel configuration and should be repeated if the number of machines used changes during subsequent computations.
In the Optimization tab
You can enable and control the desired optimization methods (described in Optimizations). You can enable the Merge and Smooth schemes by enabling the check button next to each one. For each scheme, you can also set the number of Iterations. Each optimization scheme will be applied until appropriate criteria are met, or the maximum number of iterations has been executed. If the Iterations counter is set to 0, the optimization scheme will be applied until completion, with no limit on maximum number of iterations.
Choosing the Principal Axes or Cartesian Axes method, you can improve the partitioning by enabling the automatic testing of the different bisection directions before the actual partitioning occurs. To use pretesting, enable the Pre-Test option. Pretesting is described in Pretesting.
In the Zones and/or Registers lists, select the zone(s) and/or register(s) for which you want to partition. For most cases, you will select all Zones (the default) to partition the entire domain. See below for details.
You can assign selected Zones and/or Registers to a specific partition ID
by entering a value for the Set Selected Zones and Registers
to Partition ID. For example, if the Number of partitions for your mesh is 2, then
you can only use IDs of 0 or 1. If you have three partitions, then you can enter
IDs of 0, 1, or 2. This can be useful in situations where the gradient
at a region is known to be high. In such cases, you can mark the region
or zone and set the marked cells to one of the partition IDs, thereby
preventing the partition from going through that region. This in turn
will facilitate convergence. This is also useful in cases where mesh
manipulation tools are not available in parallel. In this case, you
can assign the related cells to a particular ID so that the mesh manipulation
tools are now functional.
If you are running the parallel solver, and you have marked your region and assigned an ID to the selected Zones and/or Registers, click the button to make the new partitions valid.
Refer to the example described later in this section for a demonstration of how selected registers are assigned to a partition (Example of Setting Selected Registers to Specified Partition IDs).
In the Weighting tab (Figure 34.8: The Weighting Tab in the Partitioning and Load Balancing Dialog Box), you can set the appropriate weights prior to partitioning the mesh, to improve load balancing and overall performance. You can control weights for cells, solid zones, VOF, DPM, and ISAT table lookup. You can either rely on ANSYS Fluent timers to set the weight scaling, specify the value by enabling User-Specified, or use model-weighted partitioning (so that Fluent automatically calculates the weighting based on the cell count and the models and attributes used as weights).
Enable Faces per Cell so that the partitioning assigns a weight to each cell based on its number of faces. This type of weighting is advantageous when the case has mixed or polyhedral cell zones. If you enable the User-Specified check box, the weight assigned to each cell will be the number of faces plus the Additional Cell Weight you enter in the number-entry box under Value. By default the Faces per Cell weighting is enabled with the Additional Cell Weight set to 2.
Enable Solid Zones weighting
to allow the partitioning to take solid zones into consideration.
By default, ANSYS Fluent will scale the weight based on the computational
time of the solid and fluid zones. If an iteration has not been run,
then you may need to specify a value after enabling the user-specified
check box. The value you enter is relative to the fluid weight. Typically,
it should be less than 1 (for example, 0.0001) so that the calculation will be quicker for
the solid zone compared to the fluid zone. Entering a value greater
than 1 for the Solid Zones means that the calculation will take longer and will be more computationally
expensive for the solid zone compared to the fluid zone.
Important: Setting the Solid Zones either too high or too low can cause a load imbalance, depending on which equations are being solved. If you are not sure what would be an appropriate value, have ANSYS Fluent automatically set it for you by making sure that User-Specified is disabled.
Enable VOF weighting to allow the partitioning to consider the imbalance caused by the free surface reconstruction with the geo-reconstruct scheme. Therefore, it is only available when using the VOF model with geometric reconstruction. You may use the user-specified value before timers are collected, or if you want to specify a value other than timing statistics. The specified value is the VOF proportion of the total computational effort.
Enable DPM weighting to set the weight of DPM particles relative to the continuous phase. DPM weights are valid when you have particle tracking in your simulation, where the user-specified value is the DPM proportion of the total computational effort relative to the continuous phase. Note that this is available only when you have injections defined. For details, see Modeling Discrete Phase.
The DPM weight takes into account the distribution of the tracking effort over the partitions and it is available after at least one calculation step with particle tracking. Displaying Particle Tracks does not change the weights. The computational effort is determined by the number of DPM steps performed in each cell. This weight becomes more important when the time for the particle tracking of particles exceeds the time for solving the flow. Enabling this option in the Weighting tab enables the counting of the particle steps in the cells. These values are available for contour and vector plots when using the Discrete Phase Model and DPM Steps per Cell variable. After repartitioning, the DPM weights are reset before the next particle tracking. It is generally preferable to partition along the dominant path of the particles in order to minimize particles crossing partition boundaries and thereby reducing associated communication costs. However, partitioning should also consider load balance for the other models, especially the continuous phase, and model weighting provides a means to effectively load balance the overall simulation.
Select the Hybrid Optimization option to enable the hybrid optimization partition weighting method for DPM. This method balances the load across machines, and, within each machine, the hybrid parallel DPM method is used to make sure the load is balanced by multi-threading. First, the domain is split based on the model weights of each cell and then partitioned across a number of machines. Finally, each machine is partitioned according to the number of cores. This allows you to have a balanced number of cells in each partition, at the same time having a balanced number of particles on each machine, which will be further balanced by the hybrid DPM method. This optimization option is also applicable to the discrete element method (DEM) collision model.
Enable ISAT weighting to balance
the load during the ISAT table lookup for the stiff-chemistry Laminar,
EDC or PDF Transport models. The ISAT algorithm builds an unstructured
table in species dimensions for storage and retrieval of
the chemistry mappings. Since chemistry is usually computationally
expensive, this storage/retrieval can be very time-consuming (for
information about ISAT, refer to In-Situ Adaptive Tabulation (ISAT) in the Theory Guide). Each
parallel node builds its own table, and there is no message passing
to tables on other nodes. As some nodes may have more chemical reactions
than others (for example one parallel node may contain just air at
a constant temperature, in which case the ISAT table will contain
only one entry and calculation will be rapid), there may be a load
imbalance. The dynamic load balancing algorithm will migrate cells
from high computational load nodes to low computational load nodes.
If you decide to specify a value, this user-specified value is the ISAT proportion of the total computational effort.
You have the option of using model-weighted partitioning. The objective of model-weighted partitioning is to balance the overall number of cells, as well as the time needed for the selected models (that is, the enabled Weight Types, described previously). This is specifically useful for cases with models that could potentially lead to a load imbalance—for example, when using the discrete phase model, the distribution of particles could be different across partitions and may cause an imbalance, or in cases with large proportion of solid zones.
Each model is considered as a constraint, and a base constraint is automatically introduced for the overall number of cells. When partitioning, ANSYS Fluent will automatically calculate the weights for these constraints, and balance each of them.
To enable model-weighted partitioning, ensure that the Metis partition method is selected, and enable the appropriate models under Weight Types in the Weighting tab. Then use the following text command prior to partitioning:
parallel → partition → set → model-weighted-partition
Note that you can get additional information specific to the constraints by setting the Reporting Verbosity to 2 in the Options tab.
When using the dynamic mesh model in your parallel simulations, the Partition dialog box includes an Auto Repartition option and a Repartition Interval setting. These parallel partitioning options are provided because ANSYS Fluent migrates cells when local remeshing and smoothing are performed. Therefore, the partition interface becomes very wrinkled and the load balance may deteriorate. By default, the Auto Repartition option is selected, where a percentage of interface faces and loads are automatically traced. When this option is selected, ANSYS Fluent automatically determines the most appropriate repartition interval based on various simulation parameters. Sometimes, using the Auto Repartition option provides insufficient results, therefore, the Repartition Interval setting can be used. The Repartition Interval setting lets you to specify the interval (in time steps or iterations respectively) when a repartition is enforced. When repartitioning is not desired, you can set the Repartition Interval to zero.
Important: Note that when dynamic meshes and local remeshing is utilized, updated meshes may be slightly different in parallel ANSYS Fluent (when compared to serial ANSYS Fluent or when compared to a parallel solution created with a different number of compute nodes), resulting in very small differences in the solutions.
Click the button to partition the mesh.
Click the button if you decide that the new partitions are better than the previous ones (if the mesh was already partitioned). If you are running in parallel, this makes the newly stored cell partitions the active cell partitions. The active cell partition is used for the current calculation, while the stored cell partition (the last partition performed) is used when you save a case file.
Start ANSYS Fluent in parallel. The case in this example was partitioned across two nodes.
Read in your case.
Display the mesh with the Partitions option enabled in the Mesh Display dialog box (Figure 34.9: The Partitioned Mesh).
Adapt your region and mark your cells (for details, see Performing Region Adaption). This creates a register.
Open the Partitioning and Load Balancing dialog box.
Set the Set Selected Zones and Registers
to Partition ID to 0 and click
the corresponding button. This displays the following output in the ANSYS Fluent console:
>> 2 Active Partitions: ---------------------------------------------------------------------- Collective Partition Statistics: Minimum Maximum Total ---------------------------------------------------------------------- Cell count 459 459 918 Mean cell count deviation 0.0% 0.0% Partition boundary cell count 11 11 22 Partition boundary cell count ratio 2.4% 2.4% 2.4% Face count 764 1714 2461 Mean face count deviation -38.3% 38.3% Partition boundary face count 13 13 17 Partition boundary face count ratio 0.8% 1.7% 0.7% Partition neighbor count 1 1 ---------------------------------------------------------------------- Partition Method Metis Stored Partition Count 2 Done.
Click the button to make the new partitions valid. This migrates the partitions to the compute-nodes. The following output is then displayed in the ANSYS Fluent console:
Migrating partitions to compute-nodes.
>> 2 Active Partitions:
P Cells I-Cells Cell Ratio Faces I-Faces Face Ratio Neighbors
0 672 24 0.036 2085 29 0.014 1
1 246 24 0.098 425 29 0.068 1
----------------------------------------------------------------------
Collective Partition Statistics: Minimum Maximum Total
----------------------------------------------------------------------
Cell count 246 672 918
Mean cell count deviation -46.4% 46.4%
Partition boundary cell count 24 24 48
Partition boundary cell count ratio 3.6% 9.8% 5.2%
Face count 425 2085 2461
Mean face count deviation -66.1% 66.1%
Partition boundary face count 29 29 49
Partition boundary face count ratio 1.4% 6.8% 2.0%
Partition neighbor count 1 1
----------------------------------------------------------------------
Partition Method Metis
Stored Partition Count 2
Done.
Display the mesh (Figure 34.10: The Partitioned ID Set to Zero).
This time, set the Set Selected Zones and
Registers to Partition ID to 1 and click the corresponding button. This displays a report in the ANSYS Fluent console.
Click the button to make the new partitions valid and to migrate the partitions to the compute-nodes.
Display the mesh (Figure 34.11: The Partitioned ID Set to 1). Notice now that the partition appears in a different location as specified by your partition ID.
Important: Although this example demonstrates setting selected registers to specific partition IDs in parallel, it can be similarly applied in serial.
The ability to restrict partitioning to cell zones or registers gives you the flexibility to apply different partitioning strategies to subregions of a domain. For example, if your geometry consists of a cylindrical plenum connected to a rectangular duct, you may want to partition the plenum using the Cylindrical Axes method, and the duct using the Cartesian Axes method.
If the plenum and the duct are contained in two different cell zones, you can select one at a time and perform the desired partitioning, as described in Using the Partitioning and Load Balancing Dialog Box. If they are not in two different cell zones, you can create a cell register (basically a list of cells) for each region using the functions that are used to mark cells for adaption. These functions allow you to mark cells based on physical location, cell volume, gradient or isovalue of a particular variable, and other parameters. See Adapting the Mesh for information about marking cells for adaption. Manipulating Adaption Registers provides information about manipulating different registers to create new ones. Once you have created a register, you can partition within it as described in Example of Setting Selected Registers to Specified Partition IDs.
Important: Note that partitioning within zones or registers is not available when Metis is selected as the partition Method.
For dynamic mesh applications, ANSYS Fluent stores the partition method used to partition the respective zone. Therefore, if repartitioning is done, ANSYS Fluent uses the same method that was used to partition the mesh.
As the mesh is partitioned, information about the partitioning process will be displayed in the console. By default, the number of partitions created, the time required for the partitioning, and the minimum and maximum cell, face, interface, and face-ratio variations will be displayed (for details, see Interpreting Partition Statistics). If you increase the Reporting Verbosity to 2 from the default value of 1, the partition method used, the partition ID, number of cells, faces, and interfaces, and the ratio of interfaces to faces for each partition will also be displayed in the console. If you decrease the Reporting Verbosity to 0, only the number of partitions created and the time required for the partitioning will be reported.
You can request a portion of this report to be displayed again after the partitioning is completed. When you click the or button in the serial or parallel solver, ANSYS Fluent will display the partition ID, number of cells, faces, and interfaces, and the ratio of interfaces to faces for each active or stored partition in the console. In addition, it will display the minimum and maximum cell, face, interface, and face-ratio variations. For details, see Interpreting Partition Statistics.
Important: Recall that to make the stored cell partitions the active cell partitions you must click the button in the parallel version of ANSYS Fluent. The active cell partition is used for the current calculation, while the stored cell partition (the last partition performed) is used when you save a case file.
If you change your mind about your partition parameter settings, you can easily return to the default settings assigned by ANSYS Fluent by clicking on the button. When you click the button, it will become the Reset button. The Reset button allows you to return to the most recently saved settings (that is, the values that were set before you clicked on ). After execution, the button will become the button again.
A dynamic load balancing capability is available in ANSYS Fluent. The principal reason for using parallel processing is to reduce the turnaround time of your simulation, which may be achieved by the following means:
Faster machines, for example, faster CPU, memory, cache, and communication bandwidth between the CPU and memory
Faster interconnects, for example, smaller latency and larger bandwidth
Better Load balancing, for example, load is evenly distributed and CPUs are not idled during calculation
The first two evolve at the pace of computer technology, which is beyond the scope of this document. The third item is regarding optimization of available computation power. Here we are mainly talking about load balancing on dedicated homogeneous resources, which is often the case nowadays. If you are not using a dedicated homogeneous resource, you may need to account for differences in CPU speeds during partitioning by specifying a load distribution (for details, see Load Distribution).
On a dedicated homogeneous system, the key for load balancing is how to evaluate the computational requirement of each cell. By default, ANSYS Fluent assumes that each cell requires the same computational work, but this is often not the case. For example
A hexahedral cell demands more CPU and memory than a tetrahedral cell.
A cell with particle tracking will use more time than a cell without particle tracking.
ISAT species model cells may have magnitude differences in time usage.
To balance these differences, ideally, the time used in each cell could be recorded and load balance achieved based on these detailed timing statistics. However, this can be expensive and such low level timings can be unreliable in any case. Instead, we identify features causing computational imbalance and record time usage for these models in aggregate. For a more detailed description of this, refer to Partitioning in the discussion of the Weighting tab. In addition, the imbalance may happen dynamically during run time, for example
The mesh may be changed by adaption or mesh movement.
In unsteady cases, particle tracking may move from one region to another region.
Dynamic load balancing has been implemented for better scalability of cases with imbalanced physical or geometrical models, thereby reducing the simulation time. The implementation considers weights from these models scaled by CPU time usage. Load balancing for DPM, VOF, cell type (number of faces per cell), and solid zones can be performed. In addition, cell weight based load balancing and machine load distribution can also be specified (for details, see Load Distribution). ANSYS Fluent takes the weights from physical models and considers them for partitioning. The weights are assembled based on the time used by each physical model. For dynamic load balancing, the load is checked and balanced based on your specified imbalance threshold. To apply dynamic load balancing on the various models, click the Dynamic Load Balancing tab and select the required balancing as follows:
Enable Physical Models load balancing during iterations so that the load will be evaluated for time usage and weight distribution, based on the Interval that you provide. If the imbalance exceeds the specified Threshold, then repartitioning will be performed by considering the selected weights. Physical Models load balancing will only be available when you have the specific physical models enabled in the case. You will be prompted to enable the weights for those models. When weights for the physical models are all disabled, you will be prompted to disable Physical Models load balancing.
Note: Applying load balancing too frequently may cause performance degradation due to the additional cost of migrating cells for the new partition layout.
Enable Dynamic Mesh if there is any dynamic mesh movement. Load balancing, based on the number of cells, will be checked and balanced if the imbalance threshold is exceeded. These parallel partitioning options are provided because with mesh motion, when local remeshing and smoothing are performed, the partition interface can become very wrinkled and load balance may deteriorate. By default, the Auto option is selected, where a percentage of interface faces and loads are automatically traced. When this option is selected, ANSYS Fluent automatically determines the most appropriate repartitioning interval based on various simulation parameters. However, sometimes, the frequency of load balancing from the Auto option may be inadequate, and then the Interval setting can be explicitly set. The Interval setting lets you specify the interval (in time steps or iterations, respectively) when load balancing is enforced. When load balancing is not desired, you may disable Dynamic Mesh load balancing. Dynamic Mesh load balancing is only available when you have dynamic models enabled in your case.
Important: Note that when dynamic meshes and local remeshing are utilized, updated meshes may be slightly different in parallel ANSYS Fluent (when compared to serial ANSYS Fluent or when compared to a parallel solution created with a different number of compute nodes), resulting in very small differences in the solutions.
Enable Mesh Adaption. Any time mesh adaption occurs, load balancing, based on the number of cells, will be checked and balanced if the imbalance threshold is exceeded. If problems arise in your computations due to adaption, you can disable the load balancing for Mesh Adaption.