Importing Mesh-Based Geometry

You can import the following finite element mesh files directly into Mechanical using the Workbench External Model system:

This feature automatically synthesizes geometry from the solids, shells, and beam element-based bodies (that have an assigned cross-sectional definition) in the specified mesh for use in Mechanical. The resulting geometry is the culmination of the use of the implicit (angle-based tolerance) and explicit (based on node-based components in the file) methods that work in combination to synthesize geometry and create surfaces that enclose the mesh volume.

This feature supports all Mechanical analysis types. For the specific instructions to import a finite element mesh file using this tool, see the Creating and Configuring an External Model System section of the Workbench Help.


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.


External Model Properties in Workbench

The External Model tab is illustrated below. From this tab, you to modify various properties prior to importing your finite element data into Mechanical. Refer to the Creating and Configuring an External Model System topic in the External Model section for a description of the properties available on the External Model tab.

Model Cell Properties in Workbench

The properties of the Model cell on the Workbench Project page are illustrated below. You use the Mesh Conversion Options group of properties to specify import processes used on the finite element data. Properly defining these properties is important for you to accurately generate the desired geometries in Mechanical.

Mesh Conversion Options include:

Geometry Specifications

This feature supports data import of lines, shells, or solids or a mix of lines, shells, and solids. See the External Model Supported Element Types section for a list of the available element types for the Mechanical APDL common database (.cdb), NASTRAN, and ABAQUS file formats.

Behaviors and Characteristics

Note the following behaviors and characteristics for importing mesh-based geometries:

Examples of a geometry that results from a synthesis for a given mesh with different Tolerance Angle settings and Component Key specifications are illustrated below.

Meshed Model

This illustration is a graphical representation from Mechanical of the node data provided by a .cdb file. Two nodal components have been processed: CylinderNodes and SideNodes.

45o Tolerance Angle and All Components Specified

This illustration represents a synthesized geometry that includes node-based components and faces created using tolerance angles. The node-based components have overridden the tolerance angles for the SideNodes and created one large face around the geometry and the tolerance angle of 45o has caused the top faces to become merged.

45o Tolerance Angle and No Components Specified

This illustration shows that when node-based components are not processed, the tolerance angle creates faces correctly around the side of the geometry. However, the tolerance angle of 45o once again has caused the top faces to become merged.

25o Tolerance Angle and No Components Specified

Here again node-based components are not processed but the tolerance angle has been reduced. This has resulted in a total of 27 faces being created. Note that although the chamfer faces on the top are correctly recovered, the cylinder is now made up of multiple faces.

25o Tolerance Angle and Cylinder Component Specified

In this illustration, the CylinderNodes Component Key was specified in the properties and the Tolerance Angle was again fine-tuned to 25o. This has resulted in an accurate synthesis of the geometry.

180o Tolerance Angle and All Components Specified

This example illustrates the geometry that is synthesized using only node-based components. The tolerance angle is essentially negligible.

180o Tolerance Angle and No Components Specified

This example illustrates how only one face is generated for the geometry when no tolerance angle (180o) is specified and no node-based components are processed. This type of result can also occur when a node-based component contains all of the nodes for a given body.


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