Comments

• Sergio

  October 2015

  I would start using beams elements for the structure and shell for the fabric. I would stitch (coincident nodes or bonded contact) al the nodes between the structure and the fabric, maybe leaving free in the opposite side to the "wind". What kind of loads will you apply and results you need?
  
  Regards
• Victor

  October 2015

  The 3 element types have different levels of completeness of their physical model. In order from most to least:
  1) solid
  2) shell (no normal stiffness)
  3) membrane (no normal, bending or shear stiffness).
  
  A shell and a thin solid can usually be used for the same things as each other. It often depends which is easiest to model. Shells don't have stiffness in the out-of-plane normal direction so they aren't as accurate as solids at joints, sharp corners and other details. They can also fail to converge on some curved geometries.
  
  Membranes only have stiffness for in-plane loading and can't support any bending or out-of-plane shear loads. In Mecway, they're always 2D so there's no way to bend them anyway, but I think in other programs you can use them to model fabric with lower computer resources to solve than shells. You can approximate a membrane element by using a very thin shell element or possibly even a thin solid as you suggested.
  
  This "membrane action" you're describing requires nonlinear analysis because the initially flat sheet will have almost zero bending stiffness so it won't support wind loads until after it begins to deform. With Mecway, that means you'll have to use solid elements for both the fabric and the poles.
  
  For bonding the fabric to the poles, you can select all the outside faces of the pole elements and use them as the master surface. The edge of the fabric will only bond to the nearest face and ignore the opposite face as in Tutorial 4.9 "Mixed Materials with CAD Assemblies" under Help -> Tutorials. You can check that it's connected properly by clicking the bonded contact item in the outline tree and that shows little lines and circles indicating all the connections that will be made.
  
  To select all outside faces of a pole, make only the pole visible, change to Select Faces mode, then press Ctrl-A.
  
• pberry

  October 2015

  Thanks for the replies. This will save a huge amount of trial-and-error time for me.
  I'm assessing various frame geometries and pole designs. I'll be taking the models to failure to determine how light I can make the assembly. To start, I'll be applying an even load over the surface. Once the basic geometry is decided, I'll add some point loads to check for premature buckling.
  Regards,
  Paul
• Victor

  October 2015

  Let us know if you have any more trouble with it. Please do a simple model of fabric first to make sure the bending stiffness isn't too high. I haven't tried making solid elements that thin before. You'll need to use quadratic elements, probably hex20.
• pberry

  October 2015

  Ok, I'll test it out on something simple to see how the fabric behaves.
  Thanks.
• pberry

  November 2015

  Is there a way to pre-tension a flexible member? The structure consists of flexible poles that are straight until assembled at which time they are arched. The flexing increases stiffness and will affect how it moves when loaded.
  I'm imagining a way to take the straight pole, then define an ending shape rather than a force. Then retaining the difference in mesh geometry as the starting conditions for the normal force based analysis.
  
  Thanks,
  Paul
• Victor

  November 2015

  I don't think you would need to define the complete arc shape - just put an initial displacement on one node, say in the middle or wherever the load is applied to bend the pole, and CCX should solve that to bend the pole. Then you can tension the fabric separately, or if the bent poles are what applies the tension, just let them do that themselves.
  
  There isn't a practical way that I know of to convert displacements from the solution to fixed displacement constraints in the input.