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 or a or as . Here are some guidelines:
(BEAM188/BEAM189): This option is usually a suitable option when analyzing thin to moderately thick beam structures. A variety of cross-sections can be associated with beams.
(PIPE288/PIPE289/ELBOW290): This option is suitable for analyzing initially circular cross-sections and thin to moderately thick pipe walls. Users can apply special loads on pipes such as Pipe Pressure and Pipe Temperature. Curved pipe zones or high deformation zones in pipes can be further modeled using the Pipe Idealization object.
: Thermal fluid flow models heat distribution between fluid and solid bodies during steady-state and transient thermal analyses. This selection activates the Mechanical APDL element FLUID116 with TEMP (Temperature) as the degree of freedom. Activating Fluid Flow (via Convection) is equivalent to a reduced-order model for a Computational Fluid Dynamic (CFD) analysis, for a one-dimensional fluid flow. This provides an accurate solution that does not require significant computation time. Heat flow is generated by the conduction within the fluid and the mass transport of the fluid.
To define your line body, highlight the Line Body object and set the following in the Details view:
Stiffness Behavior: As applicable, use this property to modify the stiffness behavior of the line body. Options include (default) and .
Coordinate System: As needed, use this property to change the assigned default coordinate system.
Reference Temperature: As needed, use this property to change the default reference temperature that is taken from the environment.
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.
Offset Type: to Centroid, Shear Center, Origin, or User Defined, where Offset X and Offset Y are available.
Model Type: to Beam or Pipe or (thermal analysis only). When 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 , , and . Refer to the Discretization scheme described in the Mechanical APDL Element Reference for FLUID116.
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 (default) cross-section or as a section. Selecting 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 option sends the mesh section data, generated in DesignModeler or ANSYS SpaceClaim Direct Modeler, to the solver using the SECTYPE,,BEAM,MESH command. The option enables you to post process results on the entire mesh section.
The following read-only information is used in the definition of both beam and pipe:
Cross Section
Cross Section Area
Cross Section IYY
Cross Section IZZ
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.
When you set the Beam Section Results property of the Solution object to , 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:
Beam strains/stresses always use the solution coordinate system, even if you specify the global coordinate system.
Because your model may contain solid/shell elements (which support the Global Coordinate System) as well as beams, the stress display of the entire model can contain results in different coordinate systems. Therefore, you will experience under-defined beam stress/strain results, that is, results that will not solve or evaluate, if you perform the following:
Scope a component stress/strain to any line body and;
Choose any coordinate system other than the global coordinate system or the solution coordinate system.
Note: If you have shell or solid bodies in your model, you can choose a local coordinate system as long as you do not scope it to any line body.
Pipe elbows are not supported.
User Defined and User Integrated cross-sections are not supported.
Do not currently perform Path interpolation on expanded beams or pipes for element-node-based data, like stress and strain.
Linearized stress and stress error (SERR) and equivalent strain are not supported.
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 , 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 , and under Graphics, entering the number in the Number of Circular Cross Section Divisions field.
The feature has the following characteristics:
By default, this feature is disabled. However, the setting persists as a session preference.
Only geometry displays are applicable. The feature is not available for mesh displays.
When the feature is enabled, both normal lines and solid representations are drawn.
The solid representation of the geometry cannot be selected nor meshed, and has no effect on quantitative results.
The feature supports section planes and works with all line body cross sections (primitive and user defined).
User integrated sections (direct entry of properties) will have no display.
The feature is not available for use with viewports.
This feature is not supported on the Linux platform.
When you import geometry from an External Model system, geometric edges may be collapsed and not display the actual orientations that are specified in the external model file.
Use the Mesh display to visualize the proper orientations as defined in the file. These are the orientations that the application sends to the solver.