### 33.1.2. The Details View for Execution Control

You access the details view for Execution Control from CFX-Pre by clicking Insert > Solver > Execution Control or by right-clicking on Simulation Control in the details view and selecting Insert > Execution Control.

The tabs presented in the details view for Execution Control are described in the following sections:

- Run Definition Tab

- Initial Values Tab

- Partitioner Tab

- Solver Tab

- Interpolator Tab

#### 33.1.2.1. Run Definition Tab

To configure the Run Definition tab:

Under Execution Control > Run Definition > Solver Input File, ensure that the name of a CFX-Solver input file (extension `.def` or `.mdef`) is specified.

Note that CFX-Solver input file names must not contain spaces when run with an associated ANSYS input file (.inp).

- In the Execution Control details view of CFX-Pre, there is an option to change the order of the nodes in the mesh. Depending on the case, this reordering may result in a reduction in the run time for the CFX-Solver. From Mesh Options > Node Reordering > Options, you can select `None`, `Cuthill McKee` and `Reverse Cuthill McKee`. If either `Cuthill McKee` or `Reverse Cuthill McKee` is selected, you can choose `None`, `Ascending` or `Descending` for Sorting Within Levels. Additional information is in Initial Condition Modeling in the CFX-Solver Modeling Guide.

- Set Type of Run to `Full` or `Partitioner Only`.

  - `Full` runs the partitioner if applicable, and then runs the solver.

  - `Partitioner Only` is used for parallel runs only and does not run the solver. This writes a `.par` file.

- You can select or clear Double Precision. This setting will determine the default (single or double) precision of the partitioner, solver, and interpolator executables. For details on the precision of executables, see Double-Precision Executables in the CFX-Solver Manager User's Guide. The precisions of the partitioner, solver, and interpolator executables can be optionally overridden individually on the Partitioner, Solver, and Interpolator tabs.

- You can select or clear Large Problem. This setting will determine the default (“large problem” or not) problem size capability of the partitioner, solver, and interpolator executables. For details on the problem size capability of the executables, see Large Problem Executables in the CFX-Solver Manager User's Guide. The problem size capability of the partitioner, solver, and interpolator executables can be optionally overridden individually on the Partitioner, Solver, and Interpolator tabs.

- You can configure the Parallel Environment as required (see below).

##### Parallel Environment

Under Parallel Environment, select a Run Mode option. The run mode determines whether the run is serial (the default when defining a run in which a problem is solved as one process), or parallel (problem is split into partitions).

- A serial run (the default) requires no additional configuration.

- For a local parallel run, specify the number of partitions. This value is the number of separate processes that will be executed by the host.

Note that distributed parallel runs cannot be set up in CFX-Pre. For more information on Parallel Processing, see Parallel Run in the CFX-Solver Manager User's Guide.

##### 33.1.2.1.1. Optionally Quitting CFX-Pre

You can elect to have CFX-Pre quit upon writing CFX-Solver Input file by selecting Quit CFX-Pre when Solver Input File Written > Quit.

#### 33.1.2.2. Initial Values Tab

The Initial Values tab is used for specifying initial values via results files.

If you do not specify initial values via results files, the software will use initialization data from (in order of precedence):

- In CFX-Pre on the Initialization tab in the Domain details view

- In CFX-Pre on the Initialization tab in the Global Initialization details view

- Automatically generated initial values

  However, automatically generated initial values may not be suitable for some steady-state cases and are insufficient for all transient cases.

If you do specify initial values via results files, those values will override any initial values listed above, as applicable.

You can set initial values via results files in a variety of places as listed here (in order of precedence):

- In CFX-Solver Manager in the Define Run dialog box on the Initial Values tab

- In CFX-Pre in the Configuration details view on the Initial Values tab

  Note that for cases with multiple configurations, initial values cannot be set globally (that is, in CFX-Solver Manager or in CFX-Pre in the Execution Control details view); they can only be set per configuration (that is, in CFX-Pre in the Configuration details view).

- In CFX-Pre in the Execution Control details view on the Initial Values tab

You can set initial values via results files as follows:

1. On the Initial Values tab, select the Initial Values Specification check box to show the initial values settings.

2. Click New to create an initial values object.

3. Select an initial values object from the list.

4. Choose the source of initial values for the initial values object.

   The `Results File` option is the only option available. Specify the name of the results file from which initial values should be obtained.

5. Optionally specify Interpolation Mapping settings in order to select, position, and/or replicate the data. For details, see Interpolation Mapping in the CFX-Solver Modeling Guide.

6. Select Continue History From if you want to continue the run history (convergence history, monitor plots, time and time step counters, etc…) and use the smoothest restart possible from the selected Initial Values File. The run will continue from the one contained in the specified initial values object. Note that, in CFX-Pre, the Continue History From option is made visible by selecting Initial Values Control. Note that the run history will reset if Continue History From is not selected.

7. The Use Mesh From setting determines which file provides the mesh that is used for the analysis: the Solver Input file or the Initial Values file. The mesh from the Initial Values file can be used in a limited set of circumstances. See Using the Mesh from the Initial Values File in the CFX-Solver Modeling Guide for details. Note that, in CFX-Pre, the Use Mesh From option is made visible by selecting Initial Values Control.

Full details for Initial Values Files can be found in Reading the Initial Conditions from a File in the CFX-Solver Modeling Guide.

#### 33.1.2.3. Partitioner Tab

Use the Partitioner tab to configure mesh partitioning options for parallel runs.

Note: Once started, the run progresses through partitioning, and then into the solution of the CFD problem. Extra information is stored in the CFX output file for a parallel run. For details, see Partitioning Information in the CFX-Solver Manager User's Guide.

You can select a partition file to load by selecting Initial Partition File and clicking Browse . The `*.par` file is only available if a model has already been partitioned. The number of partitions in the partitioning file must be the same as on the Run Definition tab.

Note: An existing partition file cannot be used if the simulation involves either the Monte Carlo or Discrete Transfer radiation model. Partitions may be viewed prior to running CFX-Solver. For details, see CFX Partition File in the CFX-Solver Manager User's Guide.

Run Priority may be set to `Idle`, `Low`, `Standard` or `High` (`Standard` is selected by default). For a discussion of these priorities, see The cfx5control Application in the CFX-Solver Manager User's Guide.

##### 33.1.2.3.1. Executable Settings

You can override the precision set on the Run Definition tab by selecting Override Default Precision and then setting the precision. For details on the precision of executables, see Double-Precision Executables in the CFX-Solver Manager User's Guide.

You can override the problem size capability (“large problem” or not) set on the Run Definition tab by selecting Override Default Large Problem Setting and then setting the problem size capability (via the Large Problem check box). For details on the problem size capability of the executables, see Large Problem Executables in the CFX-Solver Manager User's Guide.

##### 33.1.2.3.2. Partitioning Detail

Under Partitioning Detail, you can specify various partition method options.

###### 33.1.2.3.2.1. Partition Type

Configure the base partition method. Available Partition Type selections include:

- Multilevel Graph Partitioning Software - MeTiS in the CFX-Solver Modeling Guide. When first running in parallel, it is recommended that Partition Type be set to MeTiS.

- Optimized Recursive Coordinate Bisection in the CFX-Solver Modeling Guide

- Recursive Coordinate Bisection in the CFX-Solver Modeling Guide

- Directional Recursive Coordinate Bisection in the CFX-Solver Modeling Guide

- User Specified Direction in the CFX-Solver Modeling Guide

- Radial in the CFX-Solver Modeling Guide

- Circumferential in the CFX-Solver Modeling Guide

- Simple Assignment in the CFX-Solver Modeling Guide

###### 33.1.2.3.2.2. Partition Weighting

Configure how partitions are weighted between machines. Available Partition Weighting selections include:

- `Automatic` (default): Calculates partition sizes based on the Relative Speed entry specified for each machine in the `hostinfo.ccl` file. Machines with a faster relative speed than others are assigned proportionally larger partition sizes.

  Note: The entry of relative speed values is usually carried out during the CFX installation process. Parallel performance can be optimized by setting accurate entries for relative speed.

- `Uniform`: Assigns equal-sized partitions to each process.

  Note: Both `Uniform` and `Automatic` give the same results for local parallel runs; it is only for distributed runs that they differ.

- `Specified`: Only available in CFX-Solver Manager. For details, see Partitioner Tab in the CFX-Solver Manager User's Guide.

###### 33.1.2.3.2.3. Multidomain Option

Configure how domains are partitioned. Available Multidomain Option selections include:

- `Automatic` (default): If the case does not involve particle transport, this is the same as the `Coupled Partitioning` option; otherwise it is the same as the `Independent Partitioning` option.

- `Independent Partitioning`: Each domain is partitioned independently into the specified number of partitions.

- `Coupled Partitioning`: All connected domains are partitioned together, provided they are the same type (i.e. solid domains are still partitioned separately from fluid/porous domains). For details, see Optimizing Mesh Partitioning in the CFX-Solver Modeling Guide.

  Note: Coupled partitioning is often more scalable, more robust and less memory expensive than independent partitioning because fewer partition boundaries are created. However, coupled partitioning may worsen the performance of particle transport calculations.

###### 33.1.2.3.2.4. Multipass Partitioning

When `Coupled Partitioning` is activated, you can further choose to set the Multipass Partitioning option. The `Transient Rotor Stator` option is relevant only for simulations having transient rotor stator interfaces. It uses a special multipass algorithm to further optimize the partition boundaries. This approach generates circumferentially-banded partitions adjacent to each transient rotor stator interface, which ensures that interface nodes remain in the same partition as the two domains slide relative to each other. Away from the interface, the partitioning is handled using whichever method is specified for the Partition Type.

##### 33.1.2.3.3. Partition Smoothing

Partition smoothing attempts to minimize the surface area of partition boundaries by swapping vertices between partitions. Partition smoothing reduces communication overhead and improves solver robustness. Smoothing is enabled by default, but may be disabled by changing Partition Smoothing > Option.

If smoothing is enabled, the algorithm will, by default, perform a maximum of 100 sweeps. The maximum number of smoothing sweeps can be specified by changing the value of Partition Smoothing > Max. Smooth. Sweeps. The smoothing algorithm will stop before this value is reached if it finds no improvement between successive sweeps.

For further details on partition smoothing, see Optimizing Mesh Partitioning in the CFX-Solver Modeling Guide.

##### 33.1.2.3.4. Partitioner Memory

If required, you can adjust the memory configuration under Partitioner Memory. For details, see Configuring Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.

#### 33.1.2.4. Solver Tab

Select the Solver tab to configure solver settings.

- Under Run Priority, you can select `Idle`, `Low`, `Standard` or `High`. For a discussion of these priorities as well as how you can change them after the execution of the solver has started, see The cfx5control Application in the CFX-Solver Manager User's Guide.

- You can override the precision set on the Run Definition tab. From Executable Settings > Override Default Precision, select or clear Double Precision. For details on the precision of executables, see Double-Precision Executables in the CFX-Solver Manager User's Guide.

- You can override the problem size capability (“large problem” or not) set on the Run Definition tab by selecting Override Default Large Problem Setting and then setting the problem size capability (via the Large Problem check box). For details on the problem size capability of the executables, see Large Problem Executables in the CFX-Solver Manager User's Guide.

- If required, you can adjust the memory configuration under Solver Memory. For details, see Configuring Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.

#### 33.1.2.5. Interpolator Tab

Select the Interpolator tab.

- Under Run Priority, you can select `Idle`, `Low`, `Standard` or `High`. For a discussion of these priorities, see The cfx5control Application in the CFX-Solver Manager User's Guide.

- You can override the precision set on the Run Definition tab by selecting Override Default Precision and then setting the precision. For details on the precision of executables, see Double-Precision Executables in the CFX-Solver Manager User's Guide.

- You can override the problem size capability (“large problem” or not) set on the Run Definition tab by selecting Override Default Large Problem Setting and then setting the problem size capability (via the Large Problem check box). For details on the problem size capability of the executables, see Large Problem Executables in the CFX-Solver Manager User's Guide.

- If required, under Interpolator Memory, you can adjust the memory configuration. For details, see Configuring Memory for the CFX-Solver in the CFX-Solver Manager User's Guide.

- You can select Domain Search Control to access the Bounding Box Tolerance setting (see below).

- You can select Interpolation Model Control to access the Enforce Strict Name Mapping for Phases, Particle Relocalization Tolerance, and Mesh Deformation Option settings (see below).

The Bounding Box Tolerance and Particle Relocalization Tolerance settings are described in Adjusting the Bounding Box Tolerance in the CFX-Solver Modeling Guide.

The Enforce Strict Name Mapping for Phases setting controls how fluids are mapped between the Initial Values files and the Solver Input File. By default, when interpolating from multiple Initial Values files onto a single Solver Input File, if each Initial Values file contains just one fluid, then the CFX-Interpolator regards all of these fluids as being the same fluid, regardless of the Fluid Definition name. You can change this default behavior by turning on the Enforce Strict Name Mapping for Phases setting. This forces the CFX-Interpolator to use the Fluid Definition names to match each fluid from each Initial Values file with the appropriate fluid in the Solver Input File.

The Mesh Deformation Option setting controls which mesh in the Initial Values File is used to check the mesh displacements: the initial mesh or the final mesh. The options are `Automatic`, `Use Latest Mesh`, and `Use Initial Mesh`. When the `Automatic` option is selected, the initial mesh will be used if the Continue History From check box is selected, and the latest mesh will be used if the Continue History From check box is cleared.

Release 18.2 - © ANSYS, Inc. All rights reserved.