How to PIN a 3D rigid body? 2

[JDSOMO]

Hi all! Let's say I have some 3D rigid body that I want to "pin" through some arbitrary axis, such that the entire body rotates about this axis. Here is a sketch that may help:

Any idea how I can do this? seems simple enough but playing around with MPC and rigid body constraints led me nowhere. I am open to either Abaqus/Standard or Explicit. Thanks a lot!!!

 

[FEA way]

You can try using hinge connector for this purpose. It provides a revolute constraint between rotational degrees of freedom of two nodes and is meant for similar puproses.

 

[JDSOMO]

Thanks for the quick reply - so do you mean (1) create a wire feature between the two points on my rigid body, i.e., connect two nodes that are part of my discrete rigid mesh, and (2) define a hinge connector on this wire? I will give it a go and report back.

 

[FEA way]

Since the body is rigid, you should attach the wire to its reference point.

 

[Mustaine3]

This is a rigid body and you want a free rotation about this axis?
Just place the reference node on the axis, create a coordinate system aligned with the axis and use it to apply BC at the ref node.

 

[JDSOMO]

@Mustaine3 - I did try that, but the problem is that I cannot JUST have UR1 free AND have a local CS. For some reason, when I try setting a "Displacement/Rotation" BC in either the initial or subsequent steps, I cannot change from the global CS.

 

[FEA way]

In the Edit Boundary Condition window for Displacement/Rotation type there’s a CSYS selection tool. By default it’s set to Global but you can click the button with arrow symbol to edit CSYS. Next to it there’s also a button with coordinate system symbol that can be used to create datum CSYS.

 

[JDSOMO]

Yes I know, but the selection is only possible if I use "Symmetry/Antisymmetry/Encastre", and here I can select 1 BC which is XSYMM (U1 = UR2 = UR3); so now I just need to fix U2 and U3, but this is not possible because if I create another BC with "pinned" for example (U1=U2=U3), then it complains about double BCs on U1. Hopefully that's a bit clearer.

Additionally, if I try to apply a rotational BC to the RP; I cannot change the CSYS:

 

[FEA way]

Most likely this BC was created in a different step, you can change CSYS only in the original step (in this case it should be Initial).

 

[JDSOMO]

I tried all sorts of combinations with displacement/rotation but it didn't seem to work (also defining the BC in Step-1); however, what seems to work, i.e., allow me to select the local CSYS, is to use the "velocity/angular velocity" boundary condition. Not too sure why? But at least it's producing the desired results. Now to increase model complexity! So I will probably be back with more questions... Thanks for all your help.

 

[FEA way]

Which version of Abaqus do you use ? If you already applied some displacement BCs in global CSYS to this point then Abaqus/CAE may block you from applying BC in local CSYS for the same point.

 

[JDSOMO]

I am using 6.14-1. FYI: I just tried that to be sure: deleted all BCs at the reference point & apply a BC in step-1 (not initial) - if I use displacement I cannot change from the global CSYS, but when I use velocity, I can change it.

 

[FEA way]

It might be some limitation or bug in this quite old version. In current release (2021) there’s no such issue.