Line Bodies

A line body consists entirely of edges and does not have a surface area or volume. Although multiple CAD sources can provide line bodies to ANSYS Workbench, only DesignModeler and ANSYS SpaceClaim Direct Modeler provide the additional cross section data needed to use line bodies in an analysis. For those CAD sources that cannot provide the cross section data, you need to import them into DesignModeler or ANSYS SpaceClaim Direct Modeler, define the cross sections, and then send the geometry to the Mechanical application in ANSYS Workbench. Cross sectional data is imported into Mechanical and provided by Cross Section Objects.

In addition to specifying the cross section type and offset, DesignModeler and SpaceClaim also allow you to align cross sections to ensure they have the proper orientation. For more information on Frame Alignment and how to override the default alignment algorithm, see Cross Section Alignment. Illustrated below are examples of the alignment algorithm options from DesignModeler.

Once imported, a line body is represented by a Line Body object in the tree, where the Details view includes the associated cross section information of the line body that was defined in SpaceClaim Direct Modeler, DesignModeler, or the supported CAD system. Depending on your application, you can further define the line body as either a Beam or a Pipe or as Thermal Fluid. Here are some guidelines:

To define your line body, highlight the Line Body object and set the following in the Details view:

  1. Stiffness Behavior: As applicable, use this property to modify the stiffness behavior of the line body. Options include Flexible (default) and Stiff Beam.

  2. Coordinate System: As needed, use this property to change the assigned default coordinate system.

  3. Reference Temperature: As needed, use this property to change the default reference temperature that is taken from the environment.

  4. Offset Mode: to Refresh on Update (default) to enable the values in the Details view to update when the CAD system updates, or to Manual, to enable the Details view values to override the CAD system updates.

  5. Offset Type: to Centroid, Shear Center, Origin, or User Defined, where Offset X and Offset Y are available.

  6. Model Type: to Beam or Pipe or Thermal Fluid (thermal analysis only). When Thermal Fluid is selected, you need to evaluate the following additional properties:

    • Fluid Cross Area: defines the fluid cross-section area of the Line Body. You can modify this value, however; by default, the application uses the value provided by your geometry application. And, updating your source Geometry resets this property to the default value.

    • Discretization: options include Upwind/Linear, Central/Linear, and Upwind/Exponential. Refer to the Discretization scheme described in the Mechanical APDL Element Reference for FLUID116.

  7. Cross Section (For Solver): This property displays when your Line Body includes a user-defined cross-section. It enables you to send user-defined cross-sections to the MAPDL solver as either a Pre-Integrated (default) cross-section or as a Mesh section. Selecting Pre-Integrated sends the integrated cross-section inertia properties, calculated in DesignModeler or ANSYS SpaceClaim Direct Modeler, to the solver using the SECTYPE,,BEAM,ASEC command. The Mesh option sends the mesh section data, generated in DesignModeler or ANSYS SpaceClaim Direct Modeler, to the solver using the SECTYPE,,BEAM,MESH command. The Mesh option enables you to post process results on the entire mesh section.


    Note:  You can change the default setting for this property in the Geometry preference of the application Options.


The following read-only information is used in the definition of both beam and pipe:


Note:
  • As illustrated below, you can increase the thickness of a line body's graphical display in the Geometry window by changing the default setting of the Line Body Thickness property in the Graphics preference of the application Options.

  • Beams can also be used as connections within a model. See Beam Connections for further information on this application.

  • Pipes are only realized in structural analyses. All line bodies defined in other analysis types are always realized as beams. This extends to linked analyses as well. For example, in a thermal-structural linked analysis where line bodies are defined as pipes, the thermal component of the analysis will only realize the line bodies as beams.


Line Body Strain and Stress Results

When you set the Beam Section Results property of the Solution object to Yes, you can evaluate for strain and stress results, in addition to deformation, when your line body model is specified as a beam/pipe that includes cross sections (SECDATA).

Limitations

These result capabilities have certain limitations, including:

Viewing Line Body Cross Sections

By default, line bodies are displayed simply as lines in the Geometry window, with no graphical indication of cross sections. If cross sections are defined in line bodies and you choose View> Cross Section Solids (Geometry), you enable a feature where line bodies are displayed as solids (3D), allowing you to visually inspect the cross sections. This visualization can be useful in determining the correct orientation of the line bodies. For circular and circular tube cross sections, the number of divisions used for rendering the line bodies as solids has an adjustable range from 6 to 360 with a default of 16. You can make this adjustment by choosing Tools> Options, and under Graphics, entering the number in the Number of Circular Cross Section Divisions field.

The Cross Section Solids (Geometry) feature has the following characteristics:


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