Explicit Tension-Only Spar
LINK167 Element Description
LINK167 allows elastic cables to be realistically modeled; therefore, no force will develop in compression.
This element is used in explicit dynamic analyses only.
LINK167 Input Data
The geometry, node locations, and the coordinate system for this element are shown in Figure 167.1: LINK167 Geometry. Node K determines the initial orientation of the cross section.
The element is defined by nodes I and J in the global coordinate system. Node K defines a plane (with I and J) containing the element s-axis. The element r-axis runs parallel to the length of the element and through nodes I and J. Node K is always required to define the element axis system and it must not be colinear with nodes I and J. The location of node K is used only to initially orient the element.
Real constants for this element are link area (AREA) and offset for cable (OFFSET). For a slack element, the offset should be input as a negative value. For an initial tensile force, the offset should be positive.
The force, F, generated by the link is nonzero if and only if the link is in tension. The force is given by:
F = K · max (Δ L,0.)
where ΔL is the change in length
Δ L = current length - (initial length - offset)
and the stiffness is defined as:
You can use only the material type cable for this element. For this material, you need to define the density (DENS) and Young's modulus (EX) or load curve ID. If you specify a load curve ID (EDMP,CABLE,VAL1, where VAL1 is the load curve ID), the Young's modulus will be ignored and the load curve will be used instead. The points on the load curve are defined as engineering stress versus engineering strain (that is, the change in length over the initial length). Use the EDCURVE command to define the load curve ID. The unloading behavior follows the loading.
Base accelerations and angular velocities in the x, y, and z directions can be applied at the nodes using the EDLOAD command. To apply these loads, you need to first select the nodes and create a component. The load is then applied to that component.
A summary of the element input is given in "LINK167 Input Summary". Additional information about real constants for this element is provided in Table 161.1: BEAM161 Real Constants. For more information about this element, see the LS-DYNA Theoretical Manual.
LINK167 Input Summary
- Nodes
I, J, K (K is the orientation node)
- Degrees of Freedom
UX, UY, UZ, VX, VY, VZ, AX, AY, AZ
Note: For explicit dynamic analyses, V(X, Y, Z) refers to nodal velocity, and A(X, Y, Z) refers to nodal acceleration. Although V(X, Y, Z) and A(X, Y, Z) appear as DOFs, they are not actually physical DOFs. However, these quantities are computed as DOF solutions and stored for postprocessing.
- Real Constants
AREA - Cross-sectional area OFFSET - Offset value for cable - Material Properties
MP command: EX, DENS, ALPD, BETD, DMPR EDMP command: CABLE (See Material Models in the ANSYS LS-DYNA User's Guide) - Surface Loads
None
- Body Loads
None
- Special Features
All nonlinear features allowed for an explicit dynamic analysis.
- KEYOPTs
None
LINK167 Output Data
Output for LINK167 consists of the following: Axial force
To output the data, you must use the ETABLE command. For the ITEM label, specify SMISC. For the COMP label, specify 1 for axial force. Then, you can use the PRETAB command to print the output data.