General Mechanical

General Mechanical

Initial loading in static structural

    • kimkarimi9574
      Subscriber

      Hi there!

      Does anybody know how I can exert an initial axial load to a pipe?

      Thanks in advance!

    • peteroznewman
      Subscriber
      If the pipe is modeled as a solid, it has a planar face at each end. If the pipe is modeled as a surface, it has a circular edge at each end.
      Create a Remote Displacement (type = Deformable) on one end (face or edge). Set all six components to 0.
      Create a Remote Force (type = Deformable) on the other end (face or edge). Type in the force in the component direction that is axial and leave the others as 0.
    • kimkarimi9574
      Subscriber
      Thanks a million!
    • Rameez_ul_Haq
      Subscriber
      ,can kindly tell here that what does applying a remote boundary condition (with all six components, particularly the rotations about all the axes, being equal to 0) on the edge of a surface means what? Does it mean that the net rotation of the edge should be zero, or the rotation of each and every node itself should be zero?
      For a face of a solid body, it is clear that the net rotation of the face should be equal to zero since the nodes of a solid body don't possess any rotational DOF at all. But for a surface body (with this remote boundary condition on an edge) is slightly confusing.
    • peteroznewman
      Subscriber
      A remote boundary condition is one of two type: Rigid or Deformable. Whether it is a face of a solid body or the face of a surface body makes no difference.
      For Rigid behavior, a CERIG element can be used for small deflection analysis. CERIG creates a set of constraint equations between DOF of nodes. See this page of the ANSYS Help:
      CERIG (ansys.com)
      For Deformable behavior, an RBE3 element can be used for small deflection analysis. RBE3 distributes the force according to weighting method. See this page of the ANSYS Help:
      RBE3 (ansys.com)
    • Rameez_ul_Haq
      Subscriber
      ,yes you already mentioned the links to CERIG and RBE3 in the second last comment on this discussion:
      I hope I can also find information there on why you keep on stressing on 'small deflection analysis' for CERIG and RBE3 elements.

    • peteroznewman
      Subscriber
      I copied over the statements I made from the Remote Force discussion to the Remote Displacement discussion because the same thing is done to create the APDL code that the solver runs.
      I keep on mentioning small deflection analysis because that is a limitation on these two elements that is mentioned in their respective Help pages. This means these elements are only valid for small rotations because the equations built into the elements have used the simplifying assumption that cosine(theta) = 1. If the structure deforms enough so that this is no longer a good approximation, the accuracy of the solution will begin to degrade.
      If you have large rotations in your structure, you would not use these elements. Other elements work for large deflection. I don't know if Mechanical automatically changes from one kind of element to another when Large Deflection is turned on and a Remote Force or Remote Displacement is used in the model. I would like to think they do, but I haven't checked. You could check yourself by writing out the Input file for Large Deflection ON then again for OFF and see if there is a difference in the input files.
    • TomPhemmy
      Subscriber
      @Rameez_ul_Haq, just to expand on @peteroznewman statement about CERIG and RBE3 being small displacement elements. You should picture that these elements are interface elements., so they connect dependent nodes and the independent nodes. You apply your loads on the independent node. Now two coordinate system come in: (1) the coordinate system at the intersection of the dependent and independent node and (2) the coordinate system of the independent node where you apply the load. ANSYS Mechanical will automatically allow for Large displacement effects on coordinate system (1) but if you want coordinate system (2) to allow for large displacement effect (i.e. you want your force applied at the independent node to rotate with the changing geometry) then you must overlay a FOLLW201 element on the independent node.
      The above is true up to v19.2. I cannot speak of newer releases, I do not have access to these.
    • Rameez_ul_Haq
      Subscriber
      ,well thank you for adding valuable information to this thread. Would love to hear what do you think if the ANSYS automatically changes the behavior of the CERIG element (Rigid) and Deformable element (RBE3) from small rotation effect to large rotation effect (i.e. no simplifications are made like cos(theta) = 1) when the Large Deflection is switched from OFF to ON.
    • TomPhemmy
      Subscriber
      @Rameez_ul_Haq, you should take a look at the ANSYS contact technology guide. See the point I highlighted in green below

      By accounting for the large displacement and rotations, ANSYS is solving the exact equations of equilibrium and not the linearized one that assumes rotation is small. This has no effect on your results. If your rotations are small, you will still get the right results because the equations for large rotations contain those of small rotation as a special case. The only problem is that the large rotation equations are more cumbersome than those of small rotation and solution might be a bit longer. I doubt you will notice the difference for simple models anyway.
Viewing 9 reply threads
  • You must be logged in to reply to this topic.