The External Model component system enables you to import finite element files created outside of Workbench into Workbench. Supported file formats include:
Mechanical APDL common database (.cdb)
Workbench mesh data file (.acmo)
Abaqus Input (.inp)
NASTRAN Bulk Data (.bdf, .dat, .nas)
Fluent Input (.msh, .cas)
ICEM CFD Input (.uns)
LS-DYNA Input (.k and .key)
Important: The External Model system only supports .cdb files archived from the Mechanical APDL application using the Blocked format. As needed, you can import your model into the Mechanical APDL application and properly archive the model. Use the PREP7 command CDWRITE,DB to create a compatible file. Or, there is a python script available: <install_dir>\Addins\ExternalLoad\Scripts that will automatically convert files to the Blocked CDB format. Execute the script using the File menu option .
Requirements and Restrictions
Review the following processing requirements and restrictions:
Only data included in the selected External Model file is imported. Furthermore:
Model assembly is not supported for Ansys data. That is, the /INPUT and CDREAD commands are not supported for Mechanical APDL files.
The *include command for NASTRAN, Abaqus, and LS-Dyna files are supported.
For Abaqus files, if you are using the *Instance command, only the data from the very first command contained in the file is read. All other data from any additional *Instance command is ignored. The element and node sets, as well as the materials, that are associated with the first *Instance command are processed. Any data that follows the first *End Part of *End Instance commands is ignored.
Scripting commands used to loop over data or generate additional items are not supported.
The Abaqus scripting command *NGEN is not supported. The commands *NSET, *ELSET, and *NODAL THICKNESS are the only commands that support the GENERATE parameter.
Only the first load step of the Abaqus file is read by the External Model system.
The following capabilities are not supported on the Linux operating systems:
Data transfer from the Engineering Data workspace.
Import of LS-DYNA input (.k and .key) files is not supported on Linux.
Geometry
For the listed file types, you can import solid, shell, and line body finite element meshes. The geometry is automatically synthesized and made available inside Mechanical.
See the Importing Mesh-Based Geometry section in the Mechanical User's Guide for additional information about how to process and work with imported geometry data.
Finite Element Data
For Mechanical APDL common database (.cdb), Abaqus Input (.inp), and Nastran Bulk Data (.bdf, .dat, .nas) files, you can import the following finite element data for use within your simulation.
See Importing Mesh-Based Geometry in the Mechanical User's Guide for additional information about the data types and how to use the data in Mechanical.
Working with the External Model System
Select a link below to jump to steps for working with finite element data from the External Model system:
Note: If you open Mechanical in such a way that the simulation does not yet include a mesh, you can use the Open option of the File tab to import an External Model file.
To specify an External Model system:
To add an External Model component system, drag the system from the Toolbox to the Project Schematic or double-click the system in the Toolbox.
Note: You can drag and drop your mesh file directly onto the Workbench Project Schematic. The application automatically creates an External Model system linked to a Mechanical Model system. Any further specification is still required.
Double-click the Setup cell or right-click the Setup cell and select from the context menu. This opens the External Model tab in order to select a desired file or files.
In the Outline of Schematic pane, in the Location column, click the icon to add a data source file (
).Browse to the location of your source files.
Select one or more files and click . The selected file names and locations are automatically displayed in the Data Source column and an entry appears in the Identifier column.
Note: The application does not copy input files specified in External Model into the project folders of downstream systems. The application references these files by absolute path only. Be sure you don’t move or rename these files.
If required, update the name in the Identifier column. By default this is Filen.
If required, enter descriptions for the files in the Description column.
For the ABAQUS (.inp), NASTRAN Bulk Data (.bdf, .dat, .nas), and LS-DYNA Input (.k and .key) file, a row labeled Click here to add a supporting file is added to the schematic that enables you to select and attach additional files to the parent file, such as node and element files. These attached files are included in the same import group as the parent file and Mechanical treats them as a package. There is no limit on the number of files you can add and/or attach.
If your parent file contains an "Include" command, property formatted, that references the desired supporting files, the application software can automatically complete the supporting files list for you if you update the Setup cell (RMB > Update) of the External Model system. The supporting file list is auto-filled only if it is empty. In addition, if the parent file references a file that is not found in the target directory, a warning message is issued. Note that you can also delete files from the supporting files list. Any supporting file that appears in the parent file (as "included") but not in the supporting file list will be ignored.
Optionally, you can right-click a file (or files) in the Outline pane 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 pane to modify the unit system, components, 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 of File pane 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 pane when multiple files are selected, your change is applied to all files.
Caution: Although you can multi-select files in the Data Source pane, when you click away from that pane the highlighting applied to those files disappears. However, the files remain active and any subsequent operations that are applied affect the files.
Table 1: Properties Pane: Description Section
Property Description Application Source This property provides a drop-down list of available file types. Table 2: Properties Pane: Definition Section
Property Description Unit System The unit system in which the file is defined. Source points are interpreted in these units. Important: When you import a project from a previous release that contains an External Model system, the Length Unit from that project is converted to a compatible Unit System. You must confirm that the Unit System chosen is appropriate; if it is not, choose the correct system from the dropdown list of consistent unit systems.
The External Model system must have a consistent unit system before you can perform an update.
Process Nodal Components Enables the External Model system to import node-based components defined in the mesh files. The application transfers the data to downstream Mechanical systems as node-based Named Selections. The application renames the node-based Named Selection objects in Mechanical based on the selection made in the Object Renaming property. Nodal Component Key This entry field enables you to filter and import only those node-based components that start with a specified name/string value in the mesh files. For example, you want to import only node-based components that start with the prefix string " nodal_*." Enter that string into this field and the application filters through all component names and returns only the components that begin with this key string value.Process Element Components Enables the External Model system to import any element-based components defined in the mesh files. The application transfers data to downstream Mechanical systems as elemental-based Named Selections. The application renames the element-based Named Selection objects in Mechanical based on the selection made in the Object Renaming property. Element Component Key This entry field enables you to filter and import only those element-based components that start with a specified name/string value in the mesh files. For example, you want to import only element-based components that start with the prefix string " elemental_*." Enter that string into this field and the application filters through all component names and returns only the components that begin with this string value.Process Face Components Enables the External Model system to import any face components defined in the mesh files. The application transfers data to downstream Mechanical systems as face-based Named Selections. The application renames the face-based Named Selection objects in Mechanical based on the selection made in the Object Renaming property. Face Component Key This entry field enables you to filter and import only those face components that start with a specified name/string value in the mesh files. For example, you want to import only face components that start with the prefix string " face_*." Enter that string into this field and the application filters through all component names and returns only the components that begin with this string value.Process Model Data When you uncheck/deactivate this option, the application will only process data directly needed for the creation of the mesh and geometry of the external file. All other data from the external file will be skipped. This includes data such as Connections and engineering abstractions such as plies, bolt pretensions, boundary conditions, etc. By default, this the option is active/checked and the application processes all data.
Process Mesh200 Elements This option supports .cdb files only. When selected, Mesh200 elements present in your mesh file are included with your geometry in Mechanical. Check Valid Blocked CBD File This property displays when the Application Source property is set to (default). This property instructs the application to verify that the specified file is a valid Blocked .cdb file. External Model only supports Blocked format. If the property is checked and the file is not a valid blocked file, an error message displays. As needed, you can import your model into the Mechanical APDL application and properly archive the model. Use the PREP7 command CDWRITE,DB to create a compatible file. You can also automatically convert files to the Blocked CDB format using the script file contained in this directory: <install_dir>\Addins\ExternalLoad\Scripts. Execute the script using the File menu option .note Important: If you unselect this property and your file is not a valid Blocked cdb file, the application may not properly import your model.
Node and Element Renumbering Method When you connect the Setup cell of an External Model to a Mechanical system, this property controls whether mesh nodes and elements are automatically renumbered to prevent conflicts. The property's options include (default) and . The application does not renumber nodes and elements if you specify . In this case, and in order to avoid conflicts, use the Node Offset and Element Offset fields to prepend your node and element IDs with the positive number of your choice.
This property requires that the Number of Copies property is set to
0. If you enter a value in the Number of Copies property, other than zero, the application requires automatic node and element ID renumbering.Transformation Type Use this property to apply a transformation to your upstream model. The transformation options for this property include (default) and . The option enables you to translate the origin of the upstream model along the X, Y, or Z axis or to rotate the model about its origin in the XY, YZ, or ZX plane.
Using the option enables you to import your upstream model as well as a mirror copy of the model about a specified plane.
Table 3: Properties Pane: Rigid Transformation 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 available only when Number Of Copies is set to 1 or greater. Select the check box 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: For the option, transformations are applied in the following order:
Rotation about the Y Axis
Rotation about the X Axis
Rotation about the Z Axis
Translations
Note: The application does not apply Rigid Transform values if they expand to the "identity transformation." The identity transformation is when the values for Origin X, Origin Y, Origin Z are all zero (within a tolerance) and Theta XY, Theta YZ, Theta ZX are all multiples of 360 degrees (within a tolerance). The application uses an absolute and relative tolerance equal to the 2D Tolerance specified in the Geometry category of the Options preferences. You can change the specified default value (1e-5) using the preference dialog.
Table 4: Properties Pane: Mirror Transformation Section
Property Description Plane Point X/Y/Z These properties enable you to define the coordinates of a point on the mirroring plane. Plane Normal X/Y/Z These properties enable you to define a vector that is normal (orthogonal) to the mirroring plane. Note: The Plane Point Z and Plane Normal Z properties are hidden for 2D models.
To modify any file in the Outline of Schematic pane, in the Location column, click
and select a new file. To delete files that you have selected (or multi-selected) right-click one of the files in the Outline of Schematic pane and select Delete from the context menu.
Return to the Project tab.
If required, link the Setup cell of the External Model to the following cells of a Mechanical Model or a Mechanical analysis system:
Model
Engineering Data (Windows Platform Only)
Once the External Model system is created, open your mesh files in Mechanical.
To add a downstream Mechanical system:
Drag a valid analysis system from the Toolbox onto the Project Schematic.
Link the External Model system Setup cell to the Mechanical system Model cell to complete the connection.
This action deletes the Geometry cell. Multiple model cells in the Project Schematic can link to one analysis system. See Assembling External Models and Mechanical Models in the Mechanical User's Guide for more details.
Modify the Mesh Conversion Options associated with the Mechanical Model cell as required.
See the Importing Mesh-Based Geometry section in the Mechanical User's Guide for more details.
Launch Mechanical.
Associativity between External Model and 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 is 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.
Re-reading Modified External Mesh Files
If you change your mesh file, such as making a manual change or as a result of an automated tool, these types of changes are not automatically updated in Workbench. You must reread your external data file and update the system to re-import the changed data.
To re-read modified external mesh files:
Right-click the Setup cell
Select Re-read Input Files from the context menu.
Right-click the Setup cell
Select Update from the context menu.
The Re-read Input Files operation causes Workbench to regard the file as having changed whether the file has changed or not, and the status of the Setup cell changes appropriately.
As required, you can incorporate Engineering Data.
To add a downstream Engineering Data system:
Drag a valid analysis system, or an Engineering Data system, from the Toolbox onto the Project Schematic.
Link the External Model system Setup cell to the Engineering Data system.
You can link the Setup cell to multiple Engineering Data cells.
Launch Engineering Data.
Note:
Review the supported MAPDL, NASTRAN, and ABAQUS material commands listed in the following subsections.
The application creates material names in the Engineering Data workspace based on the material identifier in the imported file (.cdb, ABAQUS Input, or NASTRAN Bulk Data). The names include the corresponding (linked) Workbench cell and number as well as the value in the Identifier column in the External Model setup interface.
The following MAPDL material commands are supported when importing material data into the Engineering Data workspace.
| Command | Description |
|---|---|
| MPTEMP | The following temperature-dependent material
property labels are supported for these commands: ALPX, ALPY, ALPZ, C, DENS, EX, EY, EZ, GXY, GYZ, GXZ, KXX, KYY, KZZ, NUXY, NUYZ, NUXZ, PRXY, PRYZ, PRXZ, REFT, MU, MURX, MURY, MURZ, RSVX, RSVY, RSVZ, MGXX |
| MPDATA | |
| TB | Bilinear isotropic hardening (BISO) is the only non-linear material property and label supported. |
| TBDATA |
The following NASTRAN material properties are supported when importing material data into the Engineering Data workspace.
| Card | Properties |
|---|---|
| MAT1 (Material 1) |
|
| MAT2 (Material 2) |
|
| MAT3 (Material 3) | No data is supported. Only the material ID is maintained. |
| MAT4 (Material 4) |
|
| MAT5 (Material 5) | No data is supported. Only the material ID is maintained. |
| MAT8 (Material 8) |
|
| MAT9 (Material 9) |
Note: The stiffness terms must be positive (which requires that all determinants to be positive). Otherwise, the properties are not imported. |
| MAT10 (Material 10) | No data is supported. Only the material ID is maintained. |
The following ABAQUS Materials Keywords are supported when importing material data into the Engineering Data workspace.
| Keyword | Description | |||
|---|---|---|---|---|
| *MATERIAL |
The NAME parameter is supported. | |||
|
*ELASTIC |
| |||
|
*HYPERELASTIC |
The following mutually exclusive parameters (material models) are supported:
Limitation: Temperature dependence is not supported. | |||
|
*DENSITY |
| |||
|
*EXPANSION |
| |||
|
*PLASTIC |
| |||
|
*CONDUCTIVITY |
| |||
|
*SPECIFIC HEAT |
|