General Mechanical

General Mechanical

Stiffness of connection

    • Aslinn
      Subscriber

      Hi all, is there a way to define the connection stiffness when analysing a wireframe? For example, I have a wireframe of gridshell. I assigned the cross section in SpaceClaim and set the topology to Share. In theory, the stiffness of the connection between two members can vary from a pin connection and a fixed connection. Is there anyway to control this stiffness manually?

    • peteroznewman
      Subscriber

      Please insert an image of "wireframe of gridshell" and show where you are trying to define the connection.

    • Aslinn
      Subscriber

      Thank you for your reply. This is kind of a general question, not specific to any one wireframe. It can be a regular building frame like figure 1, or a roof structure like figure 2. In either cases, the wireframe represents steel members, and the red points are connections. The rigidity of connection depends on the connection design. I'm interested in knowing if such rigidity can be defined in ANSYS. Or more straightforward, how do I distinguish a pinned connection and a moment connection in such scale analysis?



      Figure 1


       



      Figure 2

    • jj77
      Subscriber
      Pinned beam would have an end release and moment will not have that so just two beam elements connected. Stiffness I have not seen like you have in many frame civil, structural fea packages. So it is not straight forward in ansys.
    • Aslinn
      Subscriber

      Hi jj77, thank you for your reply. Does it mean there is no control of the connection rigidity in Ansys? For example, I have a steel frame, by default rigidity in Ansys, the deflection of the structure is too large. In theory, I could try to increase the rigidity of connection to reduce the deflection. Is such simulation achievable in Ansys?

    • jj77
      Subscriber

      So use end release for pinned beams, nothing for fully moment connected beams, and for released with a moment connection stiffness is not straightforward in ansys, since it is not a frame software (more of general purpose FEA).


      Below is a simple example of where the two beams (marked as 1 and 2) at the right side and at the common connection which is encircled in red are moment released thus in these two beams at their common node (encircled) the bending moment is zero (distributed line load on these two beams). This is what the results show - so end release for a pinned connection. On the opposite corner (marked in blue), the beams are fully connected and hence the moment is non zero as there is no end release there.


       


       


      Now back to the last item, moment connection with certain stiffness. Ansys has a lot of capabilities, so It is of course possible but it involves some work. One method is:


       


      Have the beams or line bodies if you are using WB with nodes vertices that are almost on top of each other (say they have an out of plane offset of 0.1 mm or something small). Then one needs to define springs (combin element with torsional stiffness), between every vertex or node that is almost coincident and where the moment stiffness is found. Finally couple all  dof (for the almost coincident nodes) except of the torsional/rotational that is taken care of by the torsion spring. CPINTF command will do that (use UX,UY,UZ,ROTX,ROTY, but not the torsional dof).


       


      That is one way of creating connections with a certain moment stiffness. It takes some work.

    • Aslinn
      Subscriber

      Hi jj77, that's very clear. Thank you for the explanation. 

Viewing 6 reply threads
  • You must be logged in to reply to this topic.