Comments

• Victor

  December 2017

  Two problems:
  
  1) The elements at the center are collapsed quadrilaterals that are shaped like triangles, and all their center nodes are disconnected. To correct it, drag to select all 80 center nodes located at (0,0,13 mm) then use Mesh tools -> Merge nearby nodes to merge them to one. Then use Mesh tools -> Correct collapsed elements to change quad8 to tri6.
  
  2) The elements on the dome part are flat in the radial/axial directions, so the dome is faceted rather than a smooth curve. If the shape should be a sphere, correct it using Mesh tools -> Fit to curved surface. I haven't changed this because I'm not sure what the correct shape is.
  
  and two suggestions that aren't really problems:
  
  3) Since it's axially symmetric, you can improve the performance a lot by modeling only one segment and using frictionless support to enforce the symmetry boundary conditions.
  
  4)There's no need for the flat rings of elements around the outer edges that have fixed supports on them. You can put the fixed support directly on the edges.
  
  

  cone shell model 2 - dynamic Damping one segment.liml 42.9K

  solution.png 26.4K
• suktan

  January 2018

  Dear Victor,
  
  Happy New Year! Thanks for your new year gift pointing the issues and giving suggestions.
  
  Should I scale materials' mass accordingly of the one-segment model for modal analysis? I got very strange result without doing so.
  
  Cheers.
  Suktan
• Victor

  January 2018 edited January 2018

  No, you shouldn't scale the density because the mass will be reduced in proportion to the volume. But you do need to scale the force down since you're only modelling a small part of the structure along with its small part of the force.
  
  
• suktan

  January 2018

  Without scaling the mass, mode 1 of modal analysis doesn't seem right.
  
  Did I make anything wrong?

  cone shell model 2 - dynamic Damping one segment Modal.liml 487.1K

  picture1.png 61.2K
• Victor

  January 2018

  It looks reasonable for the rubber surround to have the lowest frequency mode because it has a high mass and low stiffness compared to the other parts. Or is it the shape of the deformation that's the problem?
  
  Beware that modal vibration won't find any of the non-axisymmetric modes. It was OK for dynamic response because none of those modes would be activated.
  
• suktan

  January 2018 edited January 2018

  Hi Victor,
  
  Full 3D model's first mode is at 65.52 Hz. On the other hand, first mode of the one-segment mode is 279 Hz. Any idea?
  
  Thanks.

  picture2.png 452.4K
• Victor

  January 2018

  I see. Mode 1 is missing in the 1-segment model and both have the 279 Hz mode. This does look like a problem and it seems to be something to do with the frictionless support on the tri6 element at the center. I'll look into it further to see if it's a bug - thanks for bringing it up.
  
  I worked around it by removing the boundary condition from one edge of that element. That introduces a small error and the frequency is off by about 2%.
  

  cone shell model 2 - dynamic Damping one segment Modal removed BC.liml 42.9K
• suktan

  January 2018

  Thank you Victor.
• Victor

  August 2018

  Just a follow up after investigating. I think Mecway is behaving correctly here and the problem is caused by the shape of the tri6 element at the axis of symmetry. Its surface normal is not quite parallel to the axis of symmetry so the frictionless supports constrain it onto this incorrect tilted axis as shown in the attached picture.
  
  A general warning - Frictionless support is not exactly the same as mirror symmetry because it allows the symmetry "plane" to be non-planar if the elements are not perfectly shaped, which is what's happening here. Ways around that:

  • Make the mesh use the true curvature instead of faceted flat elements.
    
  • Flatten the center element by setting all nodes to the same Z coordinate.
    
  • Use separate displacement and node rotation constraints instead of frictionless support.
    

  cone.png 9.8K
• Sergio

  August 2018

  Hi, have you tried with CalculiX solver and *CYCLIC SYMMETRY MODEL card? I have tested for static analysis and works very well, it allow you to create a very good model (fine mesh) of one sector and then compute the results for the whole part (even postprocessing it, and works for Mecway using CCX custom input data). According to the documentation, for dynamic analysis it will find also the non symetric modes.
  Regards