### 16.3.4. Output Format

Default Value: CGNS

The output format selects which standard file format the output file will be written in. If a nonstandard format is required, select Custom User Export.

The sections that follow describe the available output formats.

Note: For simulations with multiple configurations, *.mres files cannot be exported by the CFX-Solver Manager.

#### 16.3.4.1. CGNS

The CFD General Notation System (CGNS) is designed to facilitate the exchange of data between sites and applications, and to help stabilize the archiving of data. The data is stored in a compact, binary format.

CGNS consists of a collection of conventions for the storage and retrieval of CFD data. The system consists of two parts:

- A standard format in which the data is recorded.

- Software that reads, writes, and modifies data in that format.

Note: To configure this option, select Tools > Export. The dialog box uses numerous common export options. For details, see Generic Export Options.

This section contains:

- CGNS Options

- Exported Files

- Contents of CGNS Files Written by ANSYS CFX

- Reading Exported Files into a Program Supporting CGNS

##### 16.3.4.1.1. CGNS Options

The following options are available when writing a file in CGNS format:

- All options specified in Generic Export Options

- Geometry Output Only

  - Default Value: Cleared.

  - If selected, only mesh information and boundary condition information is written to the destination file; result variables are not written.

- Version and File Format

  - 2.4

    The ADF file format will be used in this case.

  - 3.0

    You can select either the ADF or HDF5 format.

- When Write Transient Data to One File is selected, all transient data (grid and results) are written to one CGNS file using `BaseIterativeData_t` and `ZoneIterativeData_t` nodes within the file. When this option is not selected, transient results are exported to a separate file for each timestep.

- Output boundaries as

  - Default Value: Nodes

  - If Nodes are selected, all boundary conditions are written as collections of nodes; if Faces, then boundary conditions are written as groups of 2D elements (faces).

- When Use CGNS Variable Names is selected ANSYS CFX variable names are mapped to CGNS variable names. For example `Total Pressure` becomes `PressureStagnation`.

- When Write Full CFX Solver Name as Description is selected, CFX-Solver will write a description of the full CFX Solver Variable Name. This description is an extra data field that is used by CFD-Post when it exists. This avoids the internal variable names being used when the full CFX Solver name exceeds 32 characters.

  Whenever the name of the variable exceeds 32 characters, the internal name for the variable, which is shorter but more cryptic, is written instead. When Write Full CFX Solver Name as Description is selected, CGNS files written by CFX-Solver Manager use a new additional data tag that is not subject to the 32-character limit, and that holds the ANSYS CFX Solver Name for each variable. CFD-Post reads the new tag in preference to the old tag, if the new tag exists.

##### 16.3.4.1.2. Exported Files

The exported file set consists of either a single file for non-transient results, or multiple files for transient results. Each contains a complete mesh and flow solution. By default all files are generated with a .cgns extension. Import into a program that reads CGNS files should be done according to the importing program’s instructions.

ANSYS CFX-Export is capable of writing CGNS version 2.4 files in ADF format and version 3.0 files in both ADF and HDF5 format. These CGNS files can be read by third parties if they support the features CFX writes and are using CGNS Version 2.0 and above.

##### 16.3.4.1.3. Contents of CGNS Files Written by ANSYS CFX

The file produced contains grid and solution data. It does not contain problem setup (physics) information.

The amount of solution data and the type of grid written to the CGNS file is user controllable either on the command line or via the user interface. What is seen in the CGNS file reflects what you request. There are files that when written using some options may not be able to be reread into CFX-Pre. Caution must therefore be used if the original CFX solution files are deleted, as it may not be possible to recover all information.

Names of variables, zones, and boundary conditions are always CGNS-compliant. The name seen within the CFX application may have to be changed to achieve this. To ensure that the variable names are consistent between CFX and CGNS files, an additional data tag is written for all solution variables, starting in CFX Release 14.0. This tag, named `Ansys CFX Solver Name`, is exempt from a 32-character limit on variable names, so that the variable names displayed in CFD-Post match those in the results file.

The remainder of this sections describes the data records that are written when creating a CGNS file from ANSYS CFX.

###### 16.3.4.1.3.1. Base (Base_t)

A single base is written to each CGNS file.

- Its name is not significant.

- It is always written with a cell_dimension of 3 (that is, 3D).

If a transient file is being written, a simulation type (`SimulationType_t`) of `TimeAccurate` is specified below the base node.

A state (`ReferenceState_t`) is also written below the base node with a description of where the file was generated from and what it represents.

###### 16.3.4.1.3.2. Zones (Zone_t)

A single zone is written under each `Base_t` node for each domain you requested and is always unstructured in nature.

Coordinates of node data are always written in double precision. Due to the nature of the grid being unstructured, there is no implicit ordering in how the grid is written.

###### 16.3.4.1.3.3. Elements (Elements_t)

Element sections are written on a one per domain/subdomain basis as well as a one per boundary condition basis. Due to the nature of CFX data, a single element cannot appear in more than one element section. Element numbering is unique and consecutive.

You can control whether volume mesh (with surface mesh) or a surface mesh is written to the file.

###### 16.3.4.1.3.4. Boundary Conditions (BC_t)

Boundary Conditions are written. The location of each boundary condition is specified as set of 2D elements (faces) or a set of nodes. The former is generally preferred as the latter can have some restrictions for the program that reads the file.

No properties of the boundary condition are written other than its type.

###### 16.3.4.1.3.5. Solution Data (FlowSolution_t)

Solution data is written where requested. Names are mapped to be CGNS compliant. No discrete data is currently written. Where `Wall Only` data is present, “missing” solution data is written as 0.0.

###### 16.3.4.1.3.6. Transient Data

Transient data is written to separate CGNS files by writing the Grid and Solution data for each CFX transient file that is available to the cfx5export process.

###### 16.3.4.1.3.7. ANSYS CFX Connectivity using CGNS for Aerodynamic Noise Analysis

Further information on exporting files is contained in Aerodynamic Noise Analysis in the CFX-Solver Modeling Guide.

##### 16.3.4.1.4. Reading Exported Files into a Program Supporting CGNS

There is a wide range of products that can import CGNS files. Consult user documentation for the product being used for further information.

Note: An issue was detected while reading a CGNS file in TecPlot 10 and earlier that prevented the files written by ANSYS CFX being read by TecPlot. If a problem is encountered, try setting the environment variable CFX5_EXPORT_CGNS_TECPLOT to a value of 1, restart ANSYS CFX, and export the CGNS file again. If the problem persists, contact either ANSYS support or TecPlot support.

#### 16.3.4.2. MSC.Patran

MSC.Patran is a general-purpose CAE simulation tool.

Note: To configure this option, select Tools > Export. The dialog box uses numerous common export options. For details, see Generic Export Options.

This section contains:

- Available Options

- Exported Files

- Reading Exported Files into MSC.Patran

- Exporting Boundary Conditions to MSC.Patran

- Example Procedure

##### 16.3.4.2.1. Available Options

The following options are available when writing a file in MSC.Patran format:

- All options specified in Generic Export Options

- Geometry Output Only (Neutral File)

  - Default Value: Cleared.

    If selected, the mesh from the ANSYS CFX results file is written to a Neutral file; solution variables are not written to the Neutral file. For more details about MSC.Patran Neutral files, refer to your documentation from MSC.Patran.

##### 16.3.4.2.2. Exported Files

The file set for this export option consists of three files:

File Name | File Type
--- | ---
<basename>.out | PATRAN Neutral File
<basename>.nod | PATRAN 2.5 Nodal Results File
<basename>.results_tmpl | PATRAN Results Template File

ANSYS CFX writes files in ASCII format using a subset of the record types to be found in the full definition of the PATRAN file formats. The full definition of the PATRAN file formats can be found in the MSC.Patran documentation.

Faces associated with the CFX boundaries and elements associated with subdomains are transferred into PATRAN named components. The boundary/subdomain components are named using their CFX name.

Exported nodes are associated only with the PATRAN default_group, unless `-nodes` is used when cfx5export is used from the command line.

##### 16.3.4.2.3. Reading Exported Files into MSC.Patran

You should use the following procedure to import results into MSC.Patran Version 2001r2. However, this may need to be adapted depending on what MSC.Patran is used for. For more details about reading MSC.Patran Neutral files, see the MSC.Patran documentation.

Note: An MSC.Patran warning may appear when importing the Neutral file that reads No element type could be found for element property set <P_SET.1>. You do not need to take any action.

1. Prepare the required PATRAN files.

   Run `cfx5export` on the CFX-Solver Results file, either using CFX-Solver Manager or directly from the command line.

2. Start PATRAN and create a new database.

   Use File > New to create a new database. Click Enable NFS access (on UNIX systems only). Enter a new database name and click OK.

   In New Model Preferences, choose the appropriate Analysis Code option for the analysis.

3. Import the mesh and results.

   Use File > Import to access Import. Set Object/Source to `Model/Neutral`. Enter the name of the neutral file produced by ANSYS CFX and click Apply. Acknowledge the first message and answer Yes to the second to continue.

   Use Import again with Object/Source set to `Results/PATRAN2.nod`, to read the nodal results file produced by cfx5export. Template for PATRAN 2.5 Import Results appears. Type the name of the template file produced by cfx5export and click OK. Enter the nodal results filename in Import and click Apply.

4. Continue to use MSC.Patran as required.

##### 16.3.4.2.4. Exporting Boundary Conditions to MSC.Patran

CFX can be used to provide data to be used as boundary conditions for other types of analysis in MSC.Patran.

MSC.Patran enables models to be prepared for several different kinds of analysis. It also has facilities for using imported data to define data fields suitable for interpolating loads and boundary conditions onto the geometry or the mesh of a new model.

A description of the relevant PATRAN facilities, in particular the Fields function and its applications, can be found in the MSC.Patran documentation.

##### 16.3.4.2.5. Example Procedure

Here is an outline of some guidelines for one possible procedure for incorporating CFX results into a PATRAN model. CFX temperature predictions will be used to define a temperature distribution on a geometry surface of a new model. Details about any of the options can be found in the MSC.Patran documentation.

Points to note in this example are:

- Files generated by ANSYS CFX should be read into a new database first before any PATRAN model grid. This ensures that the node numbers of the Neutral file correspond to the nodal result file. The nodes and elements in the new model mesh will be numbered or renumbered to follow on from those in the CFX data.

- The CFX model should not be included in the new model analysis, but the CFX data must not be deleted until the boundary values have been interpolated onto the new grid.

The example assumes exported results include the Temperature variable.

1. Prepare PATRAN Neutral and Nodal results files containing boundary data only.

   Export the ANSYS CFX results file to MSC.Patran format, either using CFX-Solver Manager or directly from the command line. Toggle Boundary Data Output Only on if using CFX-Solver Manager, or use the `-boundary` option if using cfx5export from the command line.

2. Start PATRAN and create a new database.

   Use File > New to create a new database. Click Enable NFS access (on UNIX systems only). Enter a new database name and click OK.

   On New Model Preferences, choose the appropriate Analysis Code option, for example, `PATRAN 2 NF`.

3. Import the mesh and results.

   Use File > Import. Set Object/Source to `Model/Neutral`. Enter the name of the Neutral file produced by ANSYS CFX and click Apply. Acknowledge the message to continue.

   Use Import again with Object/Format set to `Results/PATRAN2.nod`, to read the nodal results file produced by ANSYS CFX. Template for PATRAN 2.5 Import Results appears. Enter the name of the template file produced by ANSYS CFX, and click OK. Enter the nodal results filename and click Apply.

4. Display temperature results as a fringe plot.

   Select Group/Post to post just the group containing the boundary condition nodes to use. Select Results. On Results, select the temperature results, and click Apply.

5. Create a continuous FEM field from the displayed variable.

   Select the Fields option. Set Action/Object/Method to `Create/Spatial/FEM`. Enter a new name under Field Name. Click the Continuous option. Select the relevant group under Mesh/Results Group Filter. Click Apply.

6. Add the geometry for the new model.

   Post the default_group and make it current using Group/Post. Use the toolbar icons to ensure the display will be in wireframe mode rather than in hidden line mode. Then either create a geometry for the new PATRAN model using the Geometry option to open the Geometry form or import the geometry from a previously prepared database using File > Import with Object/Source set to `Model/ MSC/PATRAN DB`.

7. Define a temperature boundary condition on new geometry surfaces.

   Select the Load/BCs option. Set Action/Object/Type to `Create/Temperature/Nodal`. Enter a name under New Set Name. Click Input Data. Select the field in the Spatial Fields box and click OK. Under Load/Boundary Conditions, click Select Application Region to display Select Application Region. Click the Geometry option under Geometry Filter. In Select Geometric Entities, pick the surfaces to apply the boundary condition to. Click Add and then OK. In Load/Boundary Conditions, click Apply. A temperature distribution should now be visible on the relevant geometry surfaces, in the form of values shown at the intersections of the surface display lines.

8. Complete the PATRAN model.

#### 16.3.4.3. FIELDVIEW

FIELDVIEW is a stand-alone CFD postprocessor supplied by Intelligent Light.

Note: To configure this option, select Tools > Export. The dialog box uses numerous common export options. For details, see Generic Export Options.

This section contains:

- Available Options

- Exported Files

- Reading Exported Files in FIELDVIEW

##### 16.3.4.3.1. Available Options

The following options are available when writing a file for use in FIELDVIEW Unstructured format:

- All Options specified in Generic Export Options.

- FV-UNS File Options: The options in this section detail the formatting of the separate grid and results files or combined grid and results files that are written in FV-UNS (FIELDVIEW Unstructured) file format.

- Version:

  - Default Value: 3.0

  - The value selected details which version of the format should be used when writing the grid and results to files for use within FIELDVIEW. You should use the most recent version of the file format supported by your FIELDVIEW installation. Refer to the FIELDVIEW documentation for this information.

- Split Grid and Results Format:

  - Default Value: Selected

  - When selected, the grid from the ANSYS CFX results file is written to one file and the results to a second or subsequent files. If not selected, a single combined file is written containing both the grid and the results.

    Note:

    - This option is not available when the version is less than 2.7.

    - If the number of variables that are to be written to the file exceeds 200, the results will be written to more than one results file. Refer to FIELDVIEW 9 and later to learn how to load multiple files into FIELDVIEW.

- Format:

  - Default Value: Unstructured Binary

  - This option enables a choice of whether the FV-UNS are written as in binary or ASCII format. The ASCII format is human-readable but larger than the binary format. It is therefore recommended by ANSYS and FIELDVIEW that binary format files be written in most cases.

- FV-REG Version:

  - Default Value: 2.0

  - The version specified here details the version of the format used when writing the region file for use in FIELDVIEW. You should specify the highest version that is supported by the version of FIELDVIEW you have installed.

##### 16.3.4.3.2. Exported Files

The file set for this export option consists of several files, depending on the format options selected.

If the output format is selected to be Split Grid and Results Format, more than one file will be generated with the grid in one file and results in at least one other. Optionally, a region file will also be generated:

File Name | File Type
--- | ---
<basename>_grid.fv | FIELDVIEW Grid File
<basename>_results.fv | FIELDVIEW Results File
<basename>_region.fv | FIELDVIEW Region File

If Split Grid and Results Format (see Available Options) is not selected, then at least one combined grid and results file will be generated:

File Name | File Type
--- | ---
<basename>.fv | FIELDVIEW Combined Grid and Results File
<basename>_grid.fv.fvreg | FIELDVIEW Region File

Optionally, if particle tracks have been written in the ANSYS CFX results file, then these will be written to one or more FIELDVIEW particle track files:

File Name | File Type
--- | ---
<basename>_n.fv | FIELDVIEW Particle Track File

ANSYS CFX writes a subset of record types that are available in the full FIELDVIEW file formats. The documentation supplied with FIELDVIEW describes all the record types that can be read by different versions of FIELDVIEW.

##### 16.3.4.3.3. Reading Exported Files in FIELDVIEW

Files can be read into EnSight 5, 6, 7, and 8 as required:

- FIELDVIEW Versions 10.1 and Later

- FIELDVIEW Versions 9 and 10

- FIELDVIEW Versions 6, 7, 8

###### 16.3.4.3.3.1. FIELDVIEW Versions 10.1 and Later

If the exported file is split into more than one file, it is necessary to follow a procedure similar to the following to read each file in FIELDVIEW:

1. Select File > Data Input > ANSYS-CFX[FV-UNS Export]….

2. On the ANSYS-CFX[FV-UNS Export] form, ensure that the INPUT MODE is `Replace`.

3. If the file written is in Split Grid and Results format:

   1. Click Read Grid or Combined Data.

   2. Select the grid file from the file popup and click OK.

   3. Click Read Results Data.

   4. Select the first results file and click OK.

   5. If further grid or results files are to be loaded, change the INPUT MODE to `Append` on the ANSYS-CFX[FV-UNS Export] form and repeat from step “a” until all grid or results files have been loaded.

4. If the file is a combined file:

   1. Click Read Grid or Combined Data.

   2. Select the combined file from the file popup and click OK.

###### 16.3.4.3.3.2. FIELDVIEW Versions 9 and 10

If the exported file is split into more than one file, it is necessary to follow a procedure similar to the following to read each file in FIELDVIEW:

1. Select File > Data Input > Unstructured.

2. On the FV Unstructured form ensure that the INPUT MODE is `Replace`.

3. If the file written is in Split Grid and Results format:

   1. Click Read Grid or Combined Data.

   2. Select the grid file from the file popup and click OK.

   3. Click Read Results Data.

   4. Select the first results file and click OK.

   5. If further grid or results files are to be loaded, change the INPUT MODE to Append on the FV Unstructured form and repeat from step “a” until all grid or results files have been loaded.

4. If the file is a combined file:

   1. Click Read Grid or Combined Data.

   2. Select the combined file from the file popup and click OK.

###### 16.3.4.3.3.3. FIELDVIEW Versions 6, 7, 8

The following procedure enables importing results into FIELDVIEW Version 6, 7 and 8.

Note: FIELDVIEW reads the version number from within the input file; however, some file formats that can be generated by ANSYS CFX cannot be read by all version of FIELDVIEW. Refer to FIELDVIEW documentation for exact details of which file formats can be processed by FIELDVIEW.

1. Select Data Files > Unstructured Data Input from the menu bar. In File Selection, select the file created using cfx5export and then click OK. In Function Subset Selection, select All and click OK. Click Exit in Unstructured Data Input.

2. The results can now be analyzed as required.

Note: The Region file written by ANSYS CFX to these versions of FIELDVIEW may have to be modified to ensure correct axes of rotation and rotational velocities in FIELDVIEW.

If the ANSYS CFX file contains multiple rotation axes, it is not possible to write a single FIELDVIEW file that can be correctly used in FIELDVIEW. In this case, you must write the file in “Split Grid and Results Format”. For more details about reading FIELDVIEW Unstructured files, see the FIELDVIEW documentation.

#### 16.3.4.4. EnSight

EnSight is a suite of tools for engineering and scientific simulation.

Note: To configure this option, select Tools > Export. The dialog box uses numerous common export options. For details, see Generic Export Options.

This section contains:

- Available Options

- Export Files

- Reading Exported Files into EnSight

##### 16.3.4.4.1. Available Options

The following options are available when writing files for use in EnSight:

- All options specified in Generic Export Options

- EnSight Version:

  - Default Value: Gold

  - The selection specifies the EnSight file format version to which the output will adhere. It is recommended that Gold be selected wherever possible. Refer to the EnSight documentation for differences between the different formats.

- Format:

  - Default Value: Unstructured Binary

  - This option enables you to choose whether the EnSight data files are written as in binary or ASCII format. The ASCII format is human-readable but larger than the binary format. It is therefore recommended by ANSYS that binary format files are written in most cases.

##### 16.3.4.4.2. Export Files

The file set for this export option consists of the following files:

File Name | File Type
--- | ---
<basename>.geom | EnSight Geometry File
<basename>.results | EnSight Results File (version 5 only)
<basename>.s01 (and so on) | EnSight Variable Files for scalar variable
<basename>.v01 (and so on) | EnSight Variable Files for vector variables
<basename>.case | EnSight case files (EnSight 6 and later).

Note:

- Each subdomain and boundary condition is exported as one EnSight part.

- CFX variable aliases have to be modified (by removing spaces and special characters and by limiting the name length) to create valid EnSight variable names. In some cases the names that result may not be human recognizable; in all cases the mapping from the name used in ANSYS CFX to that written to the EnSight file is displayed in the progress window of the Solver Manager.

ANSYS CFX uses a subset of record types that are available in the full EnSight file formats. The documentation supplied with EnSight describes all the record types that can be used.

##### 16.3.4.4.3. Reading Exported Files into EnSight

Files can be read into EnSight 5, 6, 7, and 8 as required.

- EnSight 8.2 and Later

- EnSight 6, 7, and 8.0

- EnSight 5

###### 16.3.4.4.3.1. EnSight 8.2 and Later

The following procedure enables importing results into EnSight 8.2 and later. For more details about importing, see the EnSight documentation.

1. Select File > Open.

2. Select the Format as `Case`.

3. Choose the case file that has been exported. All files produced by CFX-Solver Manager are automatically loaded.

###### 16.3.4.4.3.2. EnSight 6, 7, and 8.0

The following procedure enables importing results into EnSight 6, 7, or 8.0. Results files may need modification, depending on how they are to be used with EnSight. For more details about importing, see the EnSight documentation.

1. Select File > Data Reader.

2. Select the Format as `Case`.

3. Choose the case file that has been exported. All files produced by CFX-Solver Manager are automatically loaded.

###### 16.3.4.4.3.3. EnSight 5

The following procedure enables importing results into EnSight 5. Results files may need modification, depending on how they are to be used with EnSight. For more details about importing, see the EnSight documentation.

1. Select File > Data (Reader). In File Selection, click the name of the geometry file created using cfx5export, and then click (Set) Geometry.

2. Click the name of the EnSight results file. Click (Set) Result and then click Okay.

3. In Data Part Loader, click Load All, and then click Close.

4. The results can now be analyzed as required.

#### 16.3.4.5. Custom User Export

Files can be exported to a custom format from CFX-Solver Manager. To do so, a custom export program must be created. For information on all the ways of using a custom export program, see Using a Customized Export Program. For details on creating a custom export program, see Creating a Customized Export Program.

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