Modeling Cable and Ropes
Background •
Cables and ropes can be found in many structures
•
Examples: Hoists, bridges, winches, anchors, stays, etc.
•
In biomedical, a tendon acts much like a rope
•
This Meet your KM will showcase several solutions that will help guide the user to implementing a cable like structure into their simulation.
Attributes of a cable or rope •
•
•
•
Cable and ropes are multi stranded. Cables and ropes typically have small bending stiffness compared to axial stiffness so common to neglect i.e. use a link element. Modeling them as a beam element will typically be unconservative, i.e. taking moment loads when should not.
George Washington Bridge Cable Cross section
Thick cables are actually somewhat stiff in bending so a beam can still be used, but the Moments of Inertia can be modified to tailor as needed.
Rope Exploded View
How to model in ANSYS Mechanical •
Element type Link180 typically used – not supported directly
•
3 DOFs at each end – Axial force only
•
Option for tension or compression only
•
Stability
Secdata
– In static structural, using multiple links requires initial/stress or strain to pretension the cable
– No need to pretension in transient structural, but run time will increase
•
Use the Beam to Link ACT App
•
Use commands (as detailed in these following KMs)
– Version independent and works when customer can not use ACT •
Use secdata & seccontrol to replace real constants (legacy)
Seccontrol
1 Link Element vs Multiple 1 Element Advantages Disadvantages
•
•
•
•
Tips
•
No stability issue if single element Few elements, less complicated Can not model cable sag and proper loading as accurately Can not model complex curvature of rope around spool, guide, etc. Use Tension Only option to prevent from taking compression
Multiple Elements •
•
•
•
•
Best uses
•
•
Straight cables in line with loading, i.e. no sagging cables Pinned Truss (think truss bridge)
•
Model Sag, conforms to curvature Unstable in Static Structural – needs initial tension (inistate) Longer more complicated runs – convergence issues Tension only option is not always necessary since a pinned cable inherently can not take compression as links buckle, but can be turned on to assure no tension forces. Use transient structural for cables that will or can go slack
Tension only option showing collapse of link element – This can be reason for convergence issues
Cables or ropes that sag, will have sliding over complex guides, etc.
Transient Dynamic shows behavior of pinned links (contact not included)
ACT Extension •
ACT Extension available for 16 and 17 releases
•
Supports Initial strain (inistate command)
•
May need to use commands for prior releases and customers who can not use ACT extensions (company policy restrictions)
How to implement tension only cable in ANSYS Mechanical? Search Keywords: tension cable mechanical Customer Portal KM ID: 2044558
Use Line Body to model cable. Insert a Command Snippet under Line Body to define tension only element. Example of Command Snippet: ET,matid,LINK180 ! material number for this body is "matid" SECTYPE,matid,LINK SECDATA,0.01 ! set section area SECCONTROL,0,1 ! set section to be tension only
Why does rigid body motion often occur with LINK180 elements? Search Keywords: rigid motion link180 Customer Portal KM ID: 2045375
Answer: LINK180 elements do not have any rotational DOFs. It is a 'truss' element. It does not have any bending stiffness. If you only constrain one node, it can rotate/pivot about that point. Some ideas to consider: 1. Apply sufficient restraints to prevent rigid body rotation. 2. When meshing lines with link elements only use 1 element per edge. Without bending stiffness, multiple links in series may have stability issues. 3. If a series of link elements are required, you may need to apply an initial tension to provide stability.
Can I use the tension or compression only options of Link180's without using large deflection? Search Keywords: tension only large deflection Customer Portal KM ID: 2038832 Answer: The documentation currently says: To simulate the tension-/compression-only options, a nonlinear iterative solution approach is necessary; therefore, large-deflection effects must be activated (NLGEOM,ON) prior to the solution phase of the analysis. However, if you have small deflection but other non-linear features such as contact then an iterative solution will be triggered and the element will be tension or compression only as specified. However, the calculated force will only be based on small deflections. Therefore, large rotations are expected then the results will be wrong. The attached input file will run a single model and compare the forces against expected values. By commenting out the nlgeom,on the predicted forces from the strain and the length change will not match.
When did LINK180 change to using section properties and also using a KEYOPT for the tension/compression behavior? Search Keywords: link180 tension properties Customer Portal KM ID: 2026543
Answer: LINK180 had used real constants of AREA, ADDMASS, and TENSKEY (0 tens and comp, 1 tens. only, -1 comp. only) in Release 14.0 and earlier releases. At Release 14.5 it was changed to use sections and the keyopt but it was not noted in the release notes. Note: At 17 release, TENSKEY is now in seccontrol, not in keyopt
How to apply an initial stress state to link elements (LINK180 or LINK10)? Search Keywords: initial stress link180 Customer Portal KM ID: 2040086
Solution: APDL Input files (Not Mechanical).
How can we simulate tension-only truss members? Search Keywords: tension only truss Customer Portal KM ID: 2039634
How can we simulate truss (i.e. axial behavior only) elements? Search Keywords: truss axial elements Customer Portal KM ID: 2039635
How can I simulate a cable or rope articulating a body while it is sliding through a guide or sleeve? Search Keywords: cable sliding guide Customer Portal KM ID: 2046912
Context: User looking for detailed explanation of implementing capability in Mechanical via commands. Solution: See pdf and wbpz files
