Triple Shells/Plates structure

WjasiewWjasiew
Hi,all!
I'm trying to simulate the triple Shells/Plates structure in face-to-face bonded contact.First problem I can't answer is how to define shell to shell distance.I searched through the forum and manual and found no solution.It seems that the distance should be equal to half the sum of the declared shell thicknesses,but it is not stated clearly anywhere.The second problem in above structure is that central shell should be the "master" and external ones should be the "slaves".Is it allowed?
Any suggestions?Regards,Wjasiew

Comments

  • VictorVictor
    You can position the element nodes with a sum of half-thickness separation and use bonded contact with the Constraint equations option.

    The master surface should have a coarser mesh so that all master nodes belong to a face that has a slave node attached to it.

    Or if you use matching meshes with common nodes, you can specify a shell offset in Element properties to account for their thicknesses.
  • WjasiewWjasiew
    Hi Victor,thank you for express answer!
    It seems to me that I don't feel the problem.My Master and Slave meshes are exactly the same.Doesn't it mean that "all master nodes belong to a face that has a slave node attached to it."?Regards,Wjasiew
  • VictorVictor
    Yes, that's fine if the meshes are the same or similar. Just when there are big differences in element size, some nodes can get missed if they're the wrong way around.
  • WjasiewWjasiew
    Hi Victor,I quickly proceeded simulation and result was rather surprising.Solver error is presented (attached). Single shell simulation with the same border constrains was OK. Would you,please,kindly look at the results (.liml file attached) as I can't understand it at all.Regards,Wjasiew
  • VictorVictor
    Excuse me, I didn't notice the word triple before. Yes, the middle one should be the master.

    The problem here is the constraints on the corner are also on contact slave nodes which it can't do. I would probably extrude a thin strip of high stiffness shells or many beams (extrude from nodes to create beams on all of them) out from each edge and put the constraints on them instead of the nodes that belong to the contact.
  • disladisla
    Hi Wjasiew

    ¿Have you consider using a Laminate material model ?

    Regards
  • VictorVictor
    I agree with Disla that laminate would avoid this problem. Several approaches are:
    • Laminate material
    • Common nodes with shell offset on the skin elements
    • Shells connected by bonded contact
    • Solids
    Laminate has risks with sandwich materials because of the constant shear strain assumption of shells. This bonded approach might help with that but I imagine offset shells would too. I favor shell offset for being easier and probably no less accurate than bonded.
  • WjasiewWjasiew
    Hi Disla ,Victor,
    Thank You for your remarks.Laminate works OK (attachment).I tried crosssectional force load (Y force).In reality,Y-force should force Y-displacement but in the model Y-symmetry constraint (free version limit!) holds Y=0 nodes on Y=0 plane.Is the only solution to model whole spring without applying symmetry constrains?
    I tried also solid-shell bonded contact (attachment)."Improper constraint" warning appears as before.This occurs on part of "Bottom Shell" edge nodes.Warning looks like the solver stopped after these several nodes calculation and the warning is much wide in fact.
    What is tour opinion?Regards,Wjasiew
  • VictorVictor
    A Y direction force or displacement on the Y=0 edge is not symmetric so you can't use symmetry there. You would have to model at least one more segment.

    Contact will have problems with constraints on the same nodes. I usually suggest high-stiffness elastic support instead. But contact doesn't seem necessary here anyway because you already have identical meshes.
  • WjasiewWjasiew
    Hi Victor,thanks again.I will try to apply your suggestions.Regards,Wjasiew
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register