ANSYS Hull Strength Analysis Support - Multi-node constraints

Discussion in 'Software' started by Iain Young, Nov 24, 2022.

  1. Iain Young
    Joined: Nov 2022
    Posts: 4
    Likes: 0, Points: 1
    Location: United Kingdom

    Iain Young New Member

    Hi all,

    Currently have a ship hull which I have modelled in SpaceClaim and meshed in mechanical.

    In Mechanical, I am trying to constrain all of the nodes at fore and aft ends of the hull (see photo attached) in order to carry out stress/strain analyses.

    These nodes will be constrained at midships and at the neutral axis.

    However, I am struggling to work out how to do this.

    Can anyone give me any help in how to carry out a this multinode constraint?

    Thanks in advance.
     

    Attached Files:

    • 45.png
      45.png
      File size:
      444 KB
      Views:
      19
  2. Ad Hoc
    Joined: Oct 2008
    Posts: 7,431
    Likes: 1,316, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Welcome to the forum Iain

    Those regions you show in red shade, these would be conditions of symmetry.
    That means the displacements - at the nodes - will be constrained in the z axis in translation, and then in the x and y axis in rotation.

    You don't need nodal constraints at the neutral axis!

    But with 2 boundary conditions of symmetry, the model will be free to "float" away, as it has insufficient constraints, and as such, your stiffness matrix will be singular. In other words, you'll get endless rigid body motion.
    Simple solution, place one node, far away from where you are investigating and add the constraint to ensure the matrix is no longer singular, in this case the y -axis.
     
  3. Iain Young
    Joined: Nov 2022
    Posts: 4
    Likes: 0, Points: 1
    Location: United Kingdom

    Iain Young New Member

    Thank you for the welcome, but more importantly, thanks for the response.

    I will attempt to constrain the nodes using the displacement constraint and use your tip for the endless body motion problem.

    Could you elaborate on why you don't need to constrain the nodes to the neutral axis?

    To confirm: I am doing this to analyse the structural strength of the hull when applying the still water and wave loads (and eventually topside weights) in a similar manner to this paper - JMSE | Free Full-Text | Structural Analysis of a Barge Midship Section Considering the Still Water and Wave Load Effects (mdpi.com)
     
  4. Ad Hoc
    Joined: Oct 2008
    Posts: 7,431
    Likes: 1,316, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Hi Iain,

    Consider a simple I-beam, that is simply supported.
    If you apply a UDL...it will deflect bend and experience stress as a result.

    If you were to "hold" the part of the web - that is coincident - with the neutral axis, what do you think will happen?
    It wont move, it is restrained.

    So...if it is restrained, how can the beam bending into the natural curve/shape that is would otherwise do, if unrestrained at the NA?
     
  5. Iain Young
    Joined: Nov 2022
    Posts: 4
    Likes: 0, Points: 1
    Location: United Kingdom

    Iain Young New Member

    Understood.

    I've managed to do all the constraint set-up correctly, but as you said, I am getting the endless rigid body motion.

    So in terms of adding the constraint in to prevent the endless rigid body motion, how would this be applied on ANSYS?

    Is it a Nodal Displacement for the end nodes at each end attached to the 'far away point' constrained in the y-axis?
     
  6. Ad Hoc
    Joined: Oct 2008
    Posts: 7,431
    Likes: 1,316, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    Hi Iain,

    Ok, so I assume you have now set up your FEM like so:
    upload_2022-11-29_8-38-24.png

    The central; section, is the area under investigation. The extend parts, either side, are "copies" of the central section and simply mirrored.
    Thus, you end up with 3 identical sections.

    The regions shaded blue, these are the boundary conditions of symmetry, noted above.
    This being the displacements - at the nodes - will be constrained in the z axis (longitudinal) in translation, and then in the x (transverse) and y (vertical) axis in rotation.

    So, as noted before, that means the FEM is only constrained in translation in the z-axis. But it is contained in rotation in the x, y axis.
    However, sometimes, depending upon the accuracy of the model and the type of solver you select and how your loads are applied, adding just 1 more constraint is insufficient - because a force boundary condition may also be insufficient. Therefore you will need to add 2 more constraints in translation.
    So the FEM will now be fixed in 3 axis of translation. This will then allow the matrix to be solved as it is no longer singular.

    So, how do you do that?...well, you have restrained the model in the z-axis, longitudinal....so, now you need to restrain the model in the y and z axis. But to do so, without influencing the results in the region you are investigating.
    upload_2022-11-29_8-56-42.png

    At the ends of the mirrored sections, the area you are not worried about, you have the location of the neutral axis - this is perhaps where you misunderstood this concept.
    On the centreline of the NA, select one, only one node, at one end and one at the other end, noted by the arrows.

    Select one to be restrained in the y axis, and the other in the z axis.
    This then gives the FEM 3 nodes that are constrained, and thus, the model, under an applied load will not experience rigid body motion.

    So, why is this?
    The physical meaning of this, is that the structure, is free to undergo unlimited rigid body motion unless some support constraints are imposed to keep the body or structure in equilibrium under the loads. Hence, some boundary or support conditions must be applied before being solved. Because, If the structure has insufficient constraints to prevent rigid body motion, there are then an infinite number of solutions to the model (equations) that exist; each having the same deformation, but a different location in space.

    Hope this makes sense now?
     
  7. Iain Young
    Joined: Nov 2022
    Posts: 4
    Likes: 0, Points: 1
    Location: United Kingdom

    Iain Young New Member

    This makes sense, but I'm honestly struggling with the constraint set-up on ANSYS in order to achieve the model.

    Do you use this software? If so, could you share what kind of constraints are needed?

    Furthermore, for expanding the model, I'm presuming that I would need to go back into SpaceClaim to mirror both ends, then re-mesh, then apply the constraints and run the simulation?
     
    Last edited: Nov 29, 2022 at 4:17 PM

  8. Ad Hoc
    Joined: Oct 2008
    Posts: 7,431
    Likes: 1,316, Points: 113, Legacy Rep: 2488
    Location: Japan

    Ad Hoc Naval Architect

    I us two softwares, one is Ansys, but i haven't used it in years.
    Simply because i keep going back to the one I have been using for almost 30years. It is much easier to use, so I have forgotten most Ansys commands/procedures.

    For constraints, you go to the constraints tool box, and there are listed a range from Horizontal (applied to a line) to Midpoint (mid point of a line) etc etc.
    There is where and how to apply them.

    As for mirroring/copying, ive forgotten the 'easiest' way, perhaps this'll help:
     
Loading...
Forum posts represent the experience, opinion, and view of individual users. Boat Design Net does not necessarily endorse nor share the view of each individual post.
When making potentially dangerous or financial decisions, always employ and consult appropriate professionals. Your circumstances or experience may be different.