Hinge simulation in three bodies

[flyforever85]

I need to simulate an hinge in three bodies. I've seen some video in two bodies but I can't figure out how to connect the third one. Pics are linked.

My idea was: RP for each of body 1 and 2 and an hinge connection between them. Them another hinge than connects the RPs of 2 and 3. It that correct? I tried to check the reaction forces of the body in the middle and it was 0 so I'm not sure this is correct.

https://files.engineering.com/getfi...5e-2b35-4fe7-8bd2-6480ed6062dc&file=view1.tif

https://files.engineering.com/getfi...01-4ae6-486f-a185-b4849b3bd65e&file=view2.tif

 

[Mustaine3]

Your plan seems to be ok. You create one coupling with one RP for each body. Then you built 2 hinge connector elements between the 3 RP. So the RP in the middle is end node for one connector and start node for the other.

 

[FEA way]

If you’re only interested in kinematic analysis of the motion of rigid bodies you can use Display Body —> Follow single point apart from hinge connectors. Take a look at the „Flap mechanism” chapter of Example Problems Guide in Abaqus documentation.

But if you are interested in regular stress analysis with deformable bodies then create RP in the center of each of the 3 parts’ holes, add two wires (between first side part and middle part and between second side part and middle part). So that the wires will share one point (RP belonging to the middle part). Assign hinge connector section to these wires.
Don’t forget to create user CSYS with X axis along the rotation axis of the hinge. Then select this CSYS in the connector assignement window. That’s because hinge connector only rotates about the 1 axis.
And apply contacts between the side parts and middle one if they is a relative sliding between their faces.

 

[flyforever85]

Thank you both.

Shall I couple the RP with the inner surfaces of the holes? In every tutorial I saw online, no one couples RP with surfaces but when I don't, I get "3 regions are not connected in the model"

 

[FEA way]

Yes, couple RPs to the inner surfaces of the holes. This is a standard approach.

 

[flyforever85]

Thanks again. One last question: I'm trying to check the reaction forces, but only 1 node of the three has a value different than 0. Do i have to assume that the same force is in the other 2 nodes?

 

[Mustaine3]

When you connect the reference nodes with couplings to the structure and then with connectors to each other, then you should look at the connector output. CRF is the connector reaction force. Request it as field and history output for the set that contain the connectors/wires.

 

[flyforever85]

Thank you!! I don't see CRF appearing in the last version of ABAQUS, I wonder if they unified them in RF. I can chek the reaction forces for the wire connectors which I think is the equivalent of CRF, isn't it?

 

[FEA way]

Yes, to obtain CRF define history output request for a set containing wire with connector assigned. Then in the Connector section of history output request window you can find CRF variables.

 

[flyforever85]

Found it!! Thanks!!