modelling plywood in a geodesic dome

[vato]

I am analyzing an existing 39' dia wooden geodesic dome and I would appreciate any advice on properties and mesh size for simulating plywood. Since it is anisotropic I have used an average stiffness based on the strong and weak axis properties of the plywood for the FEM model. I am using the same averaging approach to check bending and shear as the panels are oriented in many different directions on the dome. I also constructed a simple span of plywood model and I have adjusted the mesh and stiffness to simulate the defleciton design equations for plywood results before applying those material properties to the plates in the dome model. The "check" will compare Von Mises to Fb, Fxy to shear in plane plywood strength. I have submeshed everything down to quads but can only reduce them to a little over a foot long (perhaps a limitation with Risa when you start with a triangular element?) So far the results are as I have heard with geodesic domes, pretty great, I'm just concerned that the mesh is too big. Thanks a lot for any thoughts.

 

[eduardotano]

I think you would have to model the problem using anisotropic material theory. Composite plate elements, in FEM, would be a good choice. You could use directly most of your test results to tune up the parameters of the model.
Using average stiffness and strength material values and an isotropic model may not be safe.

 

[GBor]

The dome is 39' in diameter and you are only down to 1' mesh size? I think that is probably too large, but how big is each piece of plywood?

I would agree with eduardotano about the use of composite elements or, more likely, an orthotropic plate (the difference is laminated plate vs. solid, bi-directional plate). If you don't have those options, consider running the analysis twice: Once with the lower modulus (which will give higher deflections) and once with the higher modulus (which will give greater stress). Also, how did you model the framing?

I'm not terribly familiar with Risa, but if you can't get the mesh size down so that, at a minimum, you have 10 or more elements along the edge of the plywood, and the ability to further reduce the mesh size for a mesh sensitivity analysis, I think you have to question your results unless you have some test results to which to compare your analysis.

One final comment: Unless you specifically need the stress in the plywood, model the framing as beams, calculate the load on the plywood and distribute it evenly on to the beams that surround that particular plywood sheet, and run the beams (pretty certain Risa can do that).

 

[vato]

I do agree with you both. Modeling as anisotropic would be preferred but I have not clue as to the direction of the plywood in th existing structure, it goes in many directions. The model fails as a beam only analysis, so the existing structure is distributing forces through the plywood in plane. I really need smaller elements as suggested. I can reproduce the plywood deflection equations with the current element size, but I do need to lower the modulus of elasticity. I will attempt to reduce element size and see what results are produced. Thanks for the thoughts.

 

[GregLocock]

I wouldn't bother with the anisotropic approach, and so long as you are careful that size of element is OK for regular structures.

Specifically I modelled a complex cast iron bracket back in the days when node numbers were limited, using perhaps 100 elements all up.

Agreement for the first 4 modes, and the stiffness estimate were excellent.

Also I have modelled an 'egg crate' style marine ply deck system for a yacht, using a few relatively large elements.

Again the results were good.

The reason that this works is that (thicker grades of) plywood /is/ pretty much anisotropic, and that the edges of the geodesic cells are stiff compared with the panels, more or less replicating the deficiencies in the FEA model.

A beam element approach would be a good double check.

I don't think an element length ~2.5% of the size of the model is unreasonable.


However I would point out that I'm not interested in stress usually, just stiffness and modeshapes and frequency.




Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.