## General Mechanical

#### how to couple nodes to move along plane directions?

• LidiannedePaula
Subscriber

I'm making the model :

• peteroznewman
Subscriber
A symmetry boundary condition in 2D along the top and bottom edges of this domain would be Y=0 and RotZ = 0.
If it is a 3D space, then there would also be RotX = 0.
• LidiannedePaula
Subscriber

I understand. Thank you! I'm wanting obtain the curve stress x deformation of this model that was discretizeted in beam elements (2D) in a article. The strain occurred up to 0.05. Is importantedefine the self contactfor linear analysis?
In this model,the authors say that Nodes at the upper and lower boundaries have been coupled to move along in plane directions. I understood that this nodes have the same displacement i this plane. Do you how apply this boundary condition?
Here is my model:

• Erik Kostson
Ansys Employee
Hi
Yes, if they are coupled, then one needs as you sow in the first image posted.
The coupling they mean is probably the CP command, so coupled (dof) of points (Say point1 x = point2 x). You can do that in WB as shown below where the two end of the beams are coupled in X, via the coupling objects and only one beam is loaded via FE displacement - because of the coupling, the end of both beams move in the same way along UX.

Sometimes if this does not work, you can insert the command object (as shown below), where say we have a named selection called CPVERT containing all of the vertices/points to be coupled (it does the same as above):
CMSEL,S,CPVERT,NODE
CP,NEXT,UX,ALL
ALLSEL,ALL

As for the contact, run it first without any and then, see which beam elements might come into contact and apply a frictional contact between these contacting beams.

Thank you

Erik