A Cable is a model type for line bodies in the Motion application, used to simulate flexible linear structures. It is particularly effective in systems with large curvature changes. The Motion application supports two model types for line bodies: Beam and Cable, each with distinct characteristics:
Table 14.1: Comparison between Beam and Cable in Motion
| Attributes | Beam | Cable (Beta) |
| Element Formulation | Beam | Beam |
| Geometry Representation | Discrete beam representation with hexa elements | Shape function-based beam geometry |
| Free Length | Not available | Available |
| Stiffness Scaling | Not available | Available |
| Deformation Due to Initial Curvature | Not available | Available |
Typically, cables exhibit significantly lower bending stiffness compared to axial and torsional stiffness, allowing them to bend more easily. This behavior can be accurately modeled by scaling bar, bending, and torsional stiffness. When a cable has an initial curvature, the corresponding initial deformation is reflected in the simulation. Without external forces or constraints, the cable will straighten over time during dynamic analysis.
Limitations
The following modeling limitations apply to cables:
Cables are only supported in the Mechanical Motion environment and cannot be modeled using the standalone preprocessor.
All elements within a cable must have the same size.
Multibody parts are not supported. The cable must be modeled as a single, independent line body.
Only circular cross-sections are supported.
For line bodies with high curvature (greater than 90 degrees), the initial curvature may cause incorrect orientation of the beam nodes.
The solver applies the following assumptions and limitations to cables:
The cable element inherits all constraints of the beam element, including the limitation to linear isotropic materials only.
The cable radius is assumed to remain constant, with any changes due to tension or compression being ignored.
Only the elongated side of the cable is considered for contact. Contact perpendicular to the cross-section is not accounted for.
The contact gap is always reported as 0.
Eigenvalue analysis is not supported.
Internal points within the cable are ignored.
For HPC solvers, only sparse solver types are supported.
The following limitations apply during post-processing:
Cable elements are represented as cylinders. Since the solver accounts for bending in each element, discrepancies may occur between the displayed element shape and the actual contact location when using a vector display.
During post-processing in the Mechanical environment, if the option is enabled and the cable has initial curvature, the cable element may appear visually distorted. This is a post-processing issue and does not affect the accuracy of the solution. In such cases, use the Standalone Postprocessor.
Note:
When selecting a contact region, if the cable edge is defined as the contact and the rigid body's edge or surface as the target, the solver automatically reverses the contact and target assignments, swapping their roles.
If retrieving the contact force on a cable using the
get_object_forcefunction in a user subroutine, ensure the correct module ID is used: for Flex-to-Rigid contact, use FTR-3D-Contact Type (504), and for Flex-to-Flex contact, use FTF-3D-Contact Type (506), regardless of the surface type.