You can import the following finite element mesh files directly into Mechanical using the Workbench External Model system:
Mechanical APDL common database (.cdb)
ABAQUS Input (.inp)
Nastran Bulk Data (.bdf, .dat, .nas)
Fluent Input (.msh, .cas)
ICEM CFD Input (.uns)
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.
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.

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:
Analysis Type: defines the mesh file as (default) or . When working with 2D analysis types, make sure that all of your model’s surface normals point in the same direction using the Rigid Transformation properties available through the External Model feature.
Tolerance Angle: this value determines if adjacent elements are of the same face during the geometry creation process. The geometry creation process identifies groups of element facets on the exterior of the mesh. These generated facets create geometric faces in Mechanical. Then skin detection algorithm scans the exterior element facets and groups them based on a tolerance angle. For example, two adjacent element facets are grouped into the same face if the angle between their normals is less than or equal to the given tolerance angle. Therefore, an angle tolerance of 180o creates only a single face for the whole body while a tolerance of 1o creates an amount of geometric faces which approaches the number of element faces if any curvature is present.
Calculations to synthesize geometries using tolerance angles use the implicit method. Processing nodal components on the same topology will override this method. See the illustrations below for examples of this behavior.
The default Tolerance Angle is degrees. This is the recommended setting.
Vertex Insertion Angle: The Vertex Insertion Angle is the minimum angle to insert a vertex between two free edges of mesh. The default value is degrees. During the generation of the geometry, if two segments of an edge abruptly make an angle greater than the Vertex Insertion Angle, then the edge is split and a vertex is inserted.
Create Geometry Face/Edge/Vertex Components: These options become active when your mesh file contains node-based named selections. When active, the algorithm creates geometry (face/edge/vertex) based on the named selections if the node-based named selection covers all the nodes of a created face/edge/vertex.
Component Key: If you select one or more of the Create Geometry Face/Edge/Vertex Components option, this property enables you to generate geometric components specific to the key name that you enter. The application evaluates keys from the beginning of the string value. For example, a given mesh file has the following components: Fixed_Support1, Fixed_Support2, and Force1. If you enter "Fixed_Support", Mechanical automatically produces Named Selections for Fixed_Support1 and Fixed_Support2, but not Force1.
Process Line Bodies: This property requires that you first select the option of the Body Grouping property as well as selecting the Create Geometry option. The Process Line Bodies property enables you to import finite element line bodies (see Line Bodies) that have a properly defined cross-section. For these finite element line bodies, the following element types are supported.
For CDB files: see the Beam Shape Category in the External Model Supported Element Types section of the Help.
For NASTRAN files: the CBAR and CBEAM element types are supported and require a cross-section property defined via PBAR, PBARL, PBEAM, or PBEAML.
For ABAQUS files: multiple options are available. Primary properties include: *BEAM SECTION, *FRAME SECTION, and *BEAM GENERAL SECTION.
Body Grouping: The setting of this property tells Mechanical how to group the elements of the same type from your data file. The options include:
(default): This option enables you to group elements based on material number assigned to the elements.
: This option enables you to group elements that have same material number and same thickness number to the same body.
Note: Elements are always grouped by shape and elements of different shape are placed in separate groups.
The body grouping option therefore controls the number of element groups / bodies created in Mechanical. Using the option, the application creates a groups for each .
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.
Note the following behaviors and characteristics for importing mesh-based geometries:
Geometry construction is for 3D lines, solids, and shells and 2D planar bodies only. Mechanical ignores any other element types contained in the mesh file.
Mechanical only processes node-based components when attempting to create geometry-based Named Selections for the faces. The application ignores element components.
You cannot change the meshes. That is, you cannot change, clear, or re-mesh once the file has been imported into Mechanical.
Mesh controls (Refinement, etc.) are not supported.
Adaptive Mesh Refinement is not supported.
Geometry is not associative. As a result, if you update the environment, for example, by adding another mesh file, any scoping that you have performed on an object will be lost. To avoid losses to your analysis environment, make sure that you have properly defined the imported Named Selections or criterion-based Named Selections.
The Stiffness Behavior of bodies can be set to only.
The Scale Factor Value property on the Geometry object is not supported.
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.
