Simulation of automotive wires

Hi Guys,

I am writing a bachelor thesis on the topic: "Kinking of unstable components", especially cables and automotive wires. For this purpose, the buckling load of certain cables is to be measured on a testing machine. The buckling load is also to be determined using a simulation in Ansys. The cross-section structure of the cable is identical to the picture in the link:

https://www.amazon.de/AUPROTEC%C2%AE-Fahrzeugleitung-FLRY-Fahrzeugkabel-schwarz-gelb/dp/B00W9TFXJ8

The cable consists of 19 copper wires that are stranded together and a PVC insulation. For homogeneous bodies, such as a round bar, the buckling force can easily be determined using the modulus of elasticity and the area moment of inertia. In the case of a stranded conductor, however, the situation is different since the individual wires are not permanently connected to one another and can be moved. After the static friction is exceeded, the individual wires begin to slide. It is therefore important to know the internal state of displacement.

The stiffness of a high-voltage line therefore always fluctuates between perfect adhesion and friction-free condition. The maximum stiffness arises with perfect adhesion of the individual wires. The minimum stiffness results from an ideal friction-free observation of the wire contacts. In reality the stiffness of the high-voltage line is between these two Limit values.

If I set all contacts to “Bonded” or “No Separation”, my simulation works quite well so far. "Bonded" corresponds to the maximum stiffness and "No Separation" to the minimum stiffness, i.e. the limit values mentioned above.

I am currently working on the non-linear contact type “Frictional”, to implement the influence of stranding and friction to the simulation. I have the following problem. As can be seen in the pictures, the individual wires move into one another or they penetrate one another. Isolation is also penetrated, which does not correspond to reality. How can I prevent this?


The penetration tolerance is set to 0.001 mm. The simulation is carried out in the "static mechanical analysis", the "eigenvalue buckling analysis" is linked to this. One side of the cable is anchored on the surfaces of the 19 wires and insulation with the "fixed bearing". A force acts on the opposite side of the cable, also on the 19 wire surfaces and insulation. An “external shift” also acts here, preventing the cable from breaking out in the Z and X directions. The deformation in the Y-direction is "free". This structure is intended to simulate Euler's 4th case.

 Euler's cases: https://www.maschinenbau-wissen.de/skript3/mechanik/icherungslehre/134-knicken-euler

I've already tried to combine contact types "Frictional" and "No separation". The problem with frictional is that the wires lift up too much from each other. In reality, this is prevented by isolation. The idea was that “no separation” would not allow the wires to lift up from one another and that the influence of friction could be observed through “frictional” when the wires slide against each other. However, the result here was the same as if I had set all contacts to "No separation".

Comments

  • jjdoylejjdoyle PittsburghMember

    Try the following options in a command object beneath the Frictional line-line contact pairs:

    keyo,cid,3,1  !Contact Traction Based Model

    keyo,cid,6,1  !Nominal refinement to allowable stiffness range

    keyo,cid,14,2  !Use up to eight target segments

    keyo,cid,15,2  !Activate Contact Stabilization for all steps


    For an explanation of what these commands do, please refer to the CONTA177 elements manual documentation.

Sign In or Register to comment.