Axisymetrix pressure vessel constraints

GermanGerman
Hi,

I'm trying to model a pressure vessel in Static Axisymetric Analysis, but I can't constraint Z node rotation in the center of the head to zero.
So resulting Y displacement at the top of the vessel are greater than expected. (See unconstrained configutarion in the model)
The only way I could do some similar constraint was using constraint equations to make Y displacement in the nodes on the rotation axis equal to Y displacements of the neighbour node. (See constrained configuration in the model)
Is there another way to do this?
Shouldn't node rotation constraint be possible in axisymetric analysis?

Thank you for your help.

Comments

  • VictorVictor
    Constraining the on-axis edge in the X direction like you have done also constrains it against rotation. So it's already OK and there's no need for any extra constraints.

    If you refine the mesh, you'll see that boundary's displacement looks more reasonable.
    axi.png 12.2K
  • GermanGerman
    It works this way, but when I refine the mesh I have to fix the constraints (because the neighbour node is a new one) and add constraints for the new nodes.
    It would be much easier if node rotation were possible.
  • VictorVictor
    edited June 2017
    Don't use constraint equations. Those will artificially stiffen the element adjacent to the axis. Just use the X-displacement constraint on the axis. That also constrains rotation about Z. This way, for the model you sent, there's no need to adjust anything after refining.

    Actually, you don't even really need the X constraint because points on the axis can't move radially in theory. However, there tends to be a small error which vanishes with mesh refinement, so it can help a little to constrain it like you did.
  • GermanGerman
    I compared Internal solver vs. CCX and I found very different results.
    CCX with coarse mesh.
    CCX seems to be more precise. At least deformed profile has the correct shape.
  • VictorVictor
    I see. I think it's at least partly because of an approximation in how the pressure load is applied in the internal solver - uniformly across the element instead of concentrated near the larger radius. They both approach the same solution with mesh refinement though, especially refinement at the part on the axis, so it's not a serious problem.
  • VictorVictor
    This poor load distribution will be fixed in version 8.
  • GermanGerman
    Victor,

    I wanted just to confirm that with version 8 the deformed profile has a much better shape in this case.
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