General Mechanical

General Mechanical

Pivoting Error on Structural Analysis of One dimensional Framed Structure

    • Lillo
      Subscriber

      Hi,

      I have a problem with the solution of the statical analysis of a one-dimensional framed structure (only beam elements). As you can see from the attached figures I created a structure in Design Modeler using line bodies in three different modes: 1) share topology to connect the line bodies, 2) joining all the line bodies in one part, 3) leaving the line bodies "free". After that, for all three cases, I applied the boundary conditions you see in the figure: 1) gravity, 2) two concentrated loads, 3) a fixed support for the four node at the base of the structure.Then, going to solve the structure, in all three cases, I get a pivoting error (as you can see in the figure). What could be the problem?

      Thank you so much in advance for the answers!


    • Lillo
      Subscriber
      A little edit just to add two screen

    • Mike Rife
      Ansys Employee
      That shorter beam with node 118 at its middle - the end nodes do not appear to line up and be shared with the vertical beams. I expect you mean nodes 60 and 116 should not be separate nodes. You already know the assembly is not fully connected. But one way to find out all the ways it is not connected is to add a Modal analysis to the WB Project, sharing the same model. Then constrain the model just against rigid body motion. Solve and post process the mode shapes. There will be zero or near zero modes with the unconnected parts rigidly translating.
      Mike
    • Erik Kostson
      Ansys Employee
      make sure all the beams share a vertex, and are thus all connected - then you can use multi-body parts in DM to merge all the common vertices and hence obtain a compatible connected mesh between beams (but first they need to share vertices).
      multi body parts - so select all parts in the tree right mouse button lick and select form a new part



      All the best

      Erik
    • Lillo
      Subscriber
      Thank you so much for the advice. I fixed it using the "merge node" command.
      But now I have another problem. Going to run a buckling analysis I get weird results. I explain myself better. I run the buckling analysis in two different modes: 1) assigning two loads of total value equal to 1 N, 2) going to assign the actual values of the two symmetrical loads (12250 N). In the first case I get a load multiplier of 384,14 (which corresponds to a critical load of 384 N) and in the second a load multiplier of 32 (which corresponds to 784000 N). Why this large discrepancy?


    • peteroznewman
      Subscriber
      I see three loads, not two. The third load is Standard Earth Gravity. The load multiplier applies to gravity as well as the two forces.
      Increase the applied force loads and rerun the buckling analysis. Find the force that delivers a load multiplier of 1.0 then you have found the critical buckling load with standard earth gravity.

Viewing 5 reply threads
  • You must be logged in to reply to this topic.