Learning Forum

[lidianne.pinto]

Hello,


I'm trying to simulate this composite plate:

The article describes: Along the longitudinal edges periodic boundary conditions are implemented. Each node along the longitudinal edge on one side is coupled with all degrees of freedom to the respective node on the other side. For example, node 1 is coupled with node 1+n. Here, denotes the number of nodes along one of the longitudinal edges. As the displacement in the longitudinal direction is constrained, the shear load is applied as a line load along the longitudinal edges, as indicated in Fig. 4.

 

How can I apply periodic boundary conditions? I tried to apply a symmetric region in the ACP. however, when I transfer the model to static analysis, a question mark appears on the mesh. This message is displayed:(DP 0) The Model component in Static Structural requires user input before it can be updated. For instructions on how to address the cell in its current state, click the blue triangle in the lower right corner of the cell in the Project Schematic.

Thank you 

[dlooman]

There may be a way through the gui, but as a last resort you could create a commands object with the command CPCYC,ALL,,,,DY where DY is the distance between the two edges in the global cartesian Y direction.

[lidianne.pinto]

Thank you, Dave. Actually,  I'm trying to apply periodic boundary conditions to the right and left side of a plate. I used named section to select one edge e other edge I select with remote point. This can be correct? 

[lidianne.pinto]

Thank you, Dave. Actually,  I'm trying to apply periodic boundary conditions to the right and left side of a plate. I used named section to select one edge e other edge I select with remote point. This can be correct? 

 

[dlooman]

I don't see the purpose of the remote point.  You want to create node to node coupling across the model for each pair of nodes with the same axial location.

[lidianne.pinto]

Dear Dave, 

I managed to couple the nodes. In "mesh by Id", I verified that the command selected the

 correct nodes. The command was written like this:

But after that, the results increased a lot. The response obtained by the authors of the article was 11,8 N/mm.  Coupling the nodes, I obtained 1,2487e+018 N/mm and without the coupling 7.4 N/mm. 

I have experience with composite plate models. I don't know what could have happened for the value to increase so much after the nodes were coupled.

Can you help me?

 

[dlooman]

Coupling the nodes does not fully constrain the model.  It constrains ROTY and ROTZ, but not UX, UY, UZ and ROTX.  For example, you can imagine rigid body motion in X producing the same UX values at both edges, which is all the periodic boundaries enforce.