Concentrated Force on a Rigid body reference point

[Bradley_123]

Hello,

I try applying a concentrated force on a rigid body's reference node, but I hit the error "Zero pivot". What should I do?

In my simulation, I have two parts initially disconnected, and one part (the rigid part) will move towards and make contact with the other part.

 

[FEA way]

Zero pivot message is just a warning, not error. It often occurs due to underconstraint. In your case, it’s likely because the parts are not initially in contact and you are applying force instead of prescribed displacement. It would be much better to apply displacement and check the reaction force. But also make sure to fix all other DOFs at the reference node in which the part is not supposed to move.

 

[Vishakh_Rajendran]

Hello,

The most important point is that, in your case, as per your question, the two parts are initially disconnected and they need to move towards each other and make contact. This type of analysis will always converge if you apply a boundary condition on the rigid body reference point. But it will not converge if you apply a concentrated force on the rigid body reference point.

A boundary condition application results in a definitive movement to some fixed extent (finite movement). Thus, the boundary condition case works fine.

For the concentrated force scenario, what is happening is a kind of a balloon scenario. You apply a force on a balloon, and since the balloon is freely floating in space, without any constraints, the application of a force will result in a free – move scenario without anything to stop the motion. This leads to convergence issues. I would suggest the following workflow:

1. Split the procedure into two steps. Apply a boundary condition in the first step until contact is established (not just touching, I mean some contact pressure should be detected).

2. Now apply the concentrated force definition in the second step.

Best Regards,

Vishakh Rajendran.