# Export/Import for CFD Solvers

Click the Export icon to open the Export tab to export CFD files. Similarly, click the Import icon to open the Import tab.
• The File type field should be automatically set to CFD.
• In the Solver type field, make a selection from the drop-down menu of which solver type to export.

## Export for CFX

CAS Mesh
This utility saves Fluent CAS/MSH files. These files contain volume and surface components used to specify boundary conditions. CAS/MSH files are imported by CFX with the added advantage that names used for all boundary zones (to impose boundary conditions) are imported into CFX without change. This facilitates the task of specifying boundary conditions for large models.

## Fluent CAS/MSH Files

Reads Fluent .cas/.msh files in BINARY or ASCII format. Both 3D and 2D (plane/axisymmetric) models are supported.
Write
Writes Fluent .cas or .msh files containing all the elements currently displayed. Before you start this writing process, display only the components/collectors that you want to export, such as the final 3D fluid domains (and any solid domains if present) and the components containing boundary zones (surface) to specify boundary conditions. Surface components should be extracted from ^faces collectors generated from the volume elements. In the case of 2D (plane or axisymmetric) models, all nodes in the mesh should have the same Z coordinate and perimeter zones for boundary conditions should be defined with components extracted from ^edges collectors generated from the 2D components defining the flow domain.
If the current mesh was previously imported from a .cas file (for example to make mesh modifications), you can reuse simulation settings and boundary conditions from the original/existing .cas file. While exporting, you are asked if you want to reuse model settings/boundary conditions. If you do, then you will be prompted for the name of the .cas file.
If the component name starts with "Interior-<Comp name>" it is considered as "Interior." If the name of the component starts with "Interface-<Comp name>" it is considered as "Interface."
If the component between two volumes is defined as "Interface", it will split the domain in Fluent.
Write (batch mode)
Execute the following command:
hmbatch.exe-tclfluent_batch.tcl

where fluent_batch.tcl has the following contents:

set ALTAIR_HOME [hm_info -appinfo ALTAIR_HOME]

set output_template "$ALTAIR_HOME/templates/feoutput/cfd/general" *templatefileset "$output_template"
*set fileName "C:/home/pipe_out.cas"
*evaltclscript "$ALTAIR_HOME/hm/scripts/cfd/cfd_comm_proc.tcl" 0 *evaltclscript "$ALTAIR_HOME/hm/scripts/cfd/cfd_proc.tbc" 0
*evaltclstring "CfdCommProc_Fluent_save_msh$fileName"0 This will read in pipe.hm and export the mesh as pipe_out.cas in Fluent format. ## STAR CD Vertex-Cell Files Read Reads native STAR CD .vrt, .cel, and optionally .bnd files in BINARY or ASCII format. Write Writes STAR CD .vrt, .cel, and .bnd files and also a .setup file that can be executed in pro-Star as an input file; this setup file imports the mesh from the .vrt / .cel files and creates all the boundary condition zones with default settings. Before you start this writing process, display only the components / collectors that you want to export, such as the final 3D fluid domains (any solid domains if present) and the components containing boundary zones to specify boundary conditions. Currently only STAR CD V3 is supported for import/export. ## CFD++ Files Read Reads native BINARY CFD++ files: cellsin.bin, nodesin.bin, exbcin.bin, mcfd.bc, and so on. Both 3D and 2D (plane/axisymmetric) models are supported. Write Writes displayed components as native BINARY CFD++ files: cellsin.bin, nodesin.bin, exbcin.bin, mcfd.bc, and so on. Before you start this writing process, display only the components/collectors that you want to export, such as the final 3D fluid domains (and any solid domains, if present) and the components containing boundary zones (surface) to specify boundary conditions. Surface components should be extracted from ^faces collectors generated from the volume elements. In the case of 2D (plane or axisymmetric) models, all nodes in the mesh should have the same Z coordinate and perimeter zones for boundary conditions should be defined with components extracted from ^edges collectors generated from the 2D components defining the flow domain. ## CGNS Files Read Reads CGNS files. Both 3D and 2D (plane/axisymmetric) models are supported. Write Writes all the displayed components to a CGNS file. Typically you will display only the 3D components / collectors representing fluid domains (any solid domains if present) and the components containing boundary zones (surface) to specify boundary conditions. Surface components should be extracted from ^faces collectors generated from volume components. Write (batch mode) Execute the following command: hmbatch.exe-tclcgns_batch.tcl where cgns_batch.tcl has the following contents: set ALTAIR_HOME [hm_info -appinfo ALTAIR_HOME] set output_template "$ALTAIR_HOME/templates/feoutput/cfd/general"
*templatefileset "$output_template" *readfile "C:/home/pipe.hm" set fileName "C:/home/pipe_out.cgns" *evaltclscript "$ALTAIR_HOME/hm/scripts/cfd/cfd_comm_proc.tcl" 0
*evaltclscript "$ALTAIR_HOME/hm/scripts/cfd/cfd_proc.tbc" 0 *evaltclstring "CfdCommProc_cgns_write$fileName" 0
This will read in pipe.hm and export the mesh as pipe_out.cgns in CGNS format.

## CGNS (Structured) Files

Write
Both 3D and 2D (plane/axisymmetric) models are supported. Writes all the displayed elements to a structured CGNS file. Typically you will display only the 3D components / collectors representing fluid domains (any solid domains if present) and the components containing boundary zones (surface) to specify boundary conditions. Surface components should be extracted from the ^faces collectors generated from volume components. The name of a surface component should contain the name of the volume component to which the shells are attached to and the type of boundary condition applied to this zone, for example, fluid_wall, fluid_inlet, or interface_fluid_solid.