External Model

The External Model system enables you to import finite element models created outside of Workbench such as models created in Mechanical APDL, Abaqus, or NASTRAN. External Model supports the following file formats for import:


Important:  Note the following Workbench support limitations when importing Abaqus Input files:

  • Parts and Assemblies are not supported. That is:

    • Only the data from the very first *Instance command is read by External Model. 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 or *End Instance commands is ignored.

  • Workbench does not support keywords that generate additional items, such as keyword *NGEN. The commands *NSET, *ELSET, and *NODAL THICKNESS are the only commands that support the Generation parameter.

  • Only the first load step of the Abaqus file is read by External Model.


Geometry

For these file type, you can import solid, shell, and line body finite element meshes. These meshes can then be imported directly into ANSYS Mechanical. The Geometry is automatically synthesized and made available inside Mechanical.

Refer to the Importing Mesh-Based Geometry section of the Mechanical Help for additional information about how to process and 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.

Refer to the Importing Mesh-Based Databases section of the Mechanical Help 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 External Model:

Creating and Configuring an External Model System

To create an External Model system:

  1. Drag an External Model system from the Component Systems Toolbox onto the Project Schematic.

  2. To display the External Model tab, double-click the Setup cell, or right-click and choose Edit from the context menu.

    You can now add the files in the Outline view.

  3. To add files:

    1. 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 Open, 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. An entry appears in the Identifier column; by default this is Filen, but you can change the name.

    2. For ABAQUS files (.inp), a row labeled Click here to add support file is added to the schematic that enables you to select and attach additional files to the parent .inp 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 .inp files you can add and/or attach.

    3. 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.

    4. 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.

    5. 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

      PropertyDescription

      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 this option is selected (default), external mesh files are imported into Mechanical. Deselect this option to exclude external mesh files.​ This feature does not apply to imported Named Selections, Nodal Orientations, Point Masses, Shell Thicknesses, or Spring Connectors.

      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.

      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 Automatic (default) and Offset. The application does not renumber nodes and elements if you specify Offset. 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.


      Table 11:  Properties View: Rigid Transformation Section

      PropertyDescription

      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:  These transformations are applied in the following order:

      1. Rotation about the Y Axis

      2. Rotation about the X Axis

      3. Rotation about the Z Axis

      4. Translations


    6. Update property modifications (Update Project) and return to the Project tab.


    Note:
    • 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.


  4. The Setup cell of the External Model system can be linked to the following cells of a Mechanical Model or a Mechanical analysis 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.


Transferring Data to Mechanical

The next step is to open your mesh files in Mechanical.

  1. To add a downstream Mechanical system:

    1. Drag a valid analysis system from the Toolbox onto the project schematic.

    2. 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 Assembling External Models and Mechanical Models in the ANSYS Mechanical User's Guide for more details.

    3. Modify the Mesh Conversion Options associated with the Mechanical Model cell as required. See Importing Mesh-Based Geometry in the ANSYS Mechanical User's Guide for more details.

  2. 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 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.

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. Therefore, you must reread your External Data file (Setup cell option Re-read Data Files) and then also update the system (Setup cell option Update) in order to re-import the changed data.

Transferring Data to Engineering Data

As desired, you can incorporate Engineering Data.

  1. To add a downstream Engineering Data system:

    1. Drag a valid analysis system from the Toolbox or an Engineering Data system onto the project schematic.

    2. Establish a link from the External Model [Setup] cell to the Engineering Data system. You can link the Setup cell to multiple Engineering Data cells.

  2. Launch Engineering Data.


    Note:  

    • Review the supported MAPDL, NASTRAN, and ABAQUSD material commands listed in the subsections below.

    • 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.


MAPDL Material Commands

The following MAPDL material commands are supported when importing material data into the Engineering Data workspace.

MPTEMP and MPDATA

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

TB and TBDATA

Bilinear isotropic hardening (BISO) is the only non-linear material property and label supported.

NASTRAN Supported Material Specifications

The following NASTRAN material properties are supported when importing material data into the Engineering Data workspace.

MAT1

The Material 1 Card supports the following properties:

  • Young's Modulus

  • Shear Modulus

  • Poisson's Ratio

  • Mass Density

  • Thermal Expansion Coefficient

  • Reference Temperature


Note:  If one value of the Young's modulus, shear modulus, or Poisson's ratio is not specified, it is calculated from the other two.


MAT2

The Material 2 Card supports the following properties:

  • 3 X 3 symmetric material property matrix

  • Mass density is supported

  • Thermal expansion coefficient vector

  • Reference temperature for thermal expansion, if thermal expansion is defined

MAT3

No data is supported for the Material 3 Card. Only the material id is maintained.

MAT4

The Material 4 Card supports Thermal conductivity and Specific Heat.

MAT5

No data is supported for the Material 5 Card. Only the material id is maintained.

MAT8

The Material 8 Card supports the following properties:

  • Moduli of elasticity

  • Poisson’s ratio

  • Shear moduli

  • Mass density

  • Thermal expansion coefficients

  • Reference temperature for thermal expansion, if thermal expansion is defined

MAT9

The Material 9 Card supports the following properties:

  • 6 X 6 symmetric material property matrix

  • Mass density is supported


Note:  The stiffness terms must be positive (which requires that all determinants to be positive). Otherwise, the properties will not be imported.


MAT10

No data is supported for the Material 10 Card. Only the material id is maintained.

ABAQUS Supported Materials Keywords

The following ABAQUS Materials Keywords are supported when importing material data into the Engineering Data workspace.

  • *MATERIAL

    • The NAME parameter is supported.

  • *ELASTIC

    • Supported for TYPE = ISOTROPIC, ENGINEERING CONSTANTS, and LAMINA.

    • The DEPENDENCIES parameter is NOT supported.

      • Material property definition is NOT processed.

    • For TYPE = ISOTROPIC:

      • Young's Modulus and Poisson's Ratio are supported.

      • If Poisson's Ratio is not specified, 0.3 is the value that is used.

      • Temperature is dependency supported.

    • For TYPE = ENGINEERING CONSTANTS and TYPE = LAMINA:

      • Young's Moduli, Poisson's Ratios, and the Shear Moduli in the principal directions is supported.

      • Temperature dependency is NOT supported - the data for the first temperature is used.

  • *DENSITY

    • The DEPENDENCIES parameter is NOT supported.

      • Material property definition is NOT processed.

    • Temperature dependency is supported.

  • *EXPANSION

    • TYPE = ISOTROPIC only

    • The DEPENDENCIES parameter is NOT supported.

      • Material property definition is NOT processed.

    • Temperature dependency is supported.

  • *PLASTIC

    • HARDENING = ISOTROPIC only.

    • Temperature dependency is NOT supported - the data for the first temperature is used.

    • The RATE parameter is not supported.

      • These stress-strain curves will be ignored.

    • Curve must have a positive slope.

  • *CONDUCTIVITY

    • Supported for TYPE = ISOTROPIC and ORTHO.

    • The DEPENDENCIES parameter is NOT supported.

      • Material property definition is NOT processed.

    • For TYPE = ISOTROPIC, temperature dependency is supported.

    • For TYPE = ORTHO, temperature dependency NOT supported. The data for the first temperature is used.

  • *SPECIFIC HEAT

    • The DEPENDENCIES parameter is NOT supported.

      • Material property definition is NOT processed.

    • The temperature dependency is supported.


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