The External Model system enables you to import solid and shell finite element meshes into Workbench. These meshes can then be imported directly into ANSYS Mechanical. Geometry is automatically synthesized and available inside Mechanical. External Model supports the following file formats for import:
Mechanical APDL common database (.cdb)
Abaqus Input (.inp)
Nastran Bulk Data (.bdf, .dat, .nas)
Fluent Input (.msh, .cas)
ICEM CFD Input (.uns)
To create an External Model system:
Drag an External Model system from the Component Systems Toolbox onto the Project Schematic.
To display the External Model tab, double-click the Setup cell, or right-click and choose from the context menu.
You can now add the files in the Outline view.
To add files:
In the Location column, you may browse to local files using the Browse option or to files stored on an EKM repository using the Browse from Repository option. For more information on Browse from Repository, see Importing Repository Files.
When you click , the selected file names and locations are automatically displayed in the Data Source column. You can enter descriptions for the files in the Description column.
Optionally, you can right-click a file (or files) in the Outline view and use the context menu to duplicate them.
All files (whether imported or duplicated) can be sorted or filtered.
Once you have opened your files, use the Properties window to modify the unit system and/or coordinate system transformation properties. These properties transform the mesh coordinate systems of the sub-assemblies for proper alignment in Mechanical.
If you select multiple files in the Data Source column, the Properties view displays:
A value when that value is the same for all selected files
A blank field when values differ between selected files
A yellow field when a value is required, but not currently specified for at least one of the files.
If you edit any field in the Properties view when multiple files are selected, your change is applied to all files.
Caution: Although you can multi-select files in the Data Source view, when you click away from that view the highlighting applied to those files disappears. However, the files remain active and any subsequent operations are applied affect the files.
Table 10: Properties View: Definition Section
| Property | Description |
|---|---|
| Length Unit | The unit system in which file is defined. Source points are interpreted in this Length Unit. |
Table 11: Properties View: Transfer Settings Section
| Property | Description |
|---|---|
Number Of Copies | When set to zero (default), only the source mesh is transformed. If you specify a number of copies greater than zero, these will be in addition to the source mesh. For example, if you import a .cdb file with a single part and set Number Of Copies to 2, you will get 3 parts in Mechanical. |
Transform Original | This property is only available when Number Of Copies is set to 1 or greater. Select the checkbox if you want to apply the specified transformation to the source mesh as well as any copies. |
Origin X/Y/Z | These properties allow you to translate the origin of the model along the X, Y, or Z axis. If you specify any copies, the translation will be applied relative to the previous copy (or source mesh in the case of the first copy). |
Theta XY/YZ/ZX | These properties allow you to rotate the model about its origin in the XY, YZ, or ZX plane. If you specify any copies, the rotation will be applied relative to the previous copy (or source mesh in the case of the first copy). |
Note: These transformations are applied in the following order:
Rotation about the Y Axis
Rotation about the X Axis
Rotation about the Z Axis
Translations
Update property modifications () and return to the Project tab.
You can modify any file in the Outline view by browsing to a new file using the browse option provided in the Location column.
You can also delete files that you have selected (or multi-selected) by right-clicking one of the files in the Outline view and then choosing Delete from the context menu.
The Setup cell of the External Model system can be linked to a Model cell of a Mechanical system.
Note: If a file imported into External Model tool is updated and you want systems connected to External Model to use the data, then you must manually re-read the data by right-clicking on the External Model setup cell and selecting Re-read Data Files. Consequently, you must use care when attempting to use parameters and design points with projects that include External Model systems. Specifically, these systems will not automatically re-read imported files or be updated as parameters and design points are updated.
The next step is to open your mesh files in Mechanical.
To add a downstream Mechanical system:
Drag a valid analysis system from the Toolbox onto the project schematic.
Establish a link from the External Model [Setup] cell to the Mechanical system [Model] cell to complete the connection which will delete the Geometry cell. Multiple model cells in the Project Schematic can link to one analysis system. See External Models and Mechanical Models in the ANSYS Mechanical User's Guide for more details.
Modify the Mesh Conversion Options associated with the Mechanical Model cell as required. See Mesh-Based Geometry in the ANSYS Mechanical User's Guide for more details.
Launch Mechanical.
Geometry from External Model (.cdb) files is partially associative. When you have geometry from multiple External Model system assembled, and you refresh upstream model data into the downstream system, any geometry scoping that you have performed on an object in the downstream analysis will be lost for the modified External Model system only. That is, only External Model systems that you change lose scoping. For example, if you have two External Model systems assembled, System 1 and System 2, and you have objects scoped to geometry in the assembled system. If you modify System 1 and then refresh the upstream system, geometry scoping on objects is lost only for System 1. System 2 experiences no scoping losses. A more robust way to maintain scoping is to properly define imported Named Selections or criterion-based Named Selections. These scoping features automatically update when the upstream model updating is complete.