Simple Pin and Roller Constraints

[Anonymous]

What's the best way to set "pin and roller" constraints in simulation?

I've already run too many iterations, and the final results are still not matching reality.

[whunter]

What doesn't match? Displacement or stress?

Your displacement value at the point of load application should be within 1% or less. Stresses will be different depending on mesh size, element type, material properties, stress criteria and constraints. Also, on a wide beam like the one you have, Poisson's ratio is going to affect your results too (try setting it to zero).

The only thing you should be concerned about is the deflection, if you can get that right or get confidence in the value, the stresses will be correct.

If F360 had beam elements, you'd get exactly the same results as the ones out of beam tables. But a solid mesh will give slightly or massively different results, depending on where/how you inspect results in the mesh.

Do a benchmark analysis with a simply supported beam of very simple geometry, e.g., a solid rectangular beam without fillets, holes, etc, and make it quite long so that it looks like a beam). Then compare this with the result form a hand calculation for the same beam. Once you get confidence in the result, apply the same approach to your more complicated model.

--

whunter

[Anonymous]

Thank you. The example in screencast is actually already a very simplified basic form of our complex design. But yes I agree that to gain confidence in simulation results, I should try a super simple, easy-to-calculate-by-hand rectangular section beam.

The key question for this discussion is probably how to add (or reduce if it's the case) the proper constraints and constraint types. So whether it's relatively simple corrugated box beam or super simple rectangular cross section beam, what should the constraints be?

My example seems almost correct with two "edges" each with restricted Y and Z axis (assuming load comes down along Z axis), and a third "vertex" constraint restricting all X, Y, Z axes. However, there's still the seemingly unwanted restriction of material elongation (or contraction) along the Y axis. This would reduce the displacement, which is the first (and only for now) result that I seek. How to overcome this (if it's the proper question)?

[whunter]

I think your restraints are probably adequate. I ran a comparison FEA (Beam details: 200x100 solid rectangular beam, 2500 long, E = 200 GPa, Poisson's ratio = 0.25) using dedicated FEA software, and with a bit of tweaking I can get F360 Simulation to give the same results.

The main difference is that in my FEA software I can constrain per element node, which is obviously a big advantage.

Results from dedicated FEA software below: The Beam result is what you'd expect to get from a hand calc, exactly the same value. As a check, I = (b*d^3)/12 = 66.67E-6 m^4, F = 1000 N, L = 2.5 m, displacement = F*L^3/(48*E*I) = 24.41E-6 m = 24.41E-3 mm, so spot on for the beam element. The brick mesh is within 2.5% for deflection.

 

F360 Sim results: You have to use a fine mesh for linear elements (absolute size to 25 mm), for parabolic elements you can use a much coarser mesh.

Displacement is just about spot-on.

Stress is plotted for ZZ direction (along the length of the beam).

[John_Holtz]

Hi OldVWXer,

The constraints should duplicate whatever the "reality" is, where the reality may be different. For example,

• The "engineering" drawing that you showed in the original post probably does not have constraints on the bottom of the beam. Almost all hand calculations are based on the beam being restrained at the neutral axis (generally the mid height).
• A physical test of the beam sitting between two saw horses would have constraints more like what I think you have in the screencast.

If the direction between the two end supports is X, then restraining one edge in X, Y, Z and restraining the opposite edge in Z should be sufficient. For the first case, you would need to split the end faces to create an edge at the neutral axis. For the second case, you can apply the constraints along the bottom edge.

Also, you wrote "there's still the seemingly unwanted restriction of material elongation (or contraction) along the Y axis". Did you mean X - along the length of the beam between the two supports? In theory, if you push with enough force, the two ends of the beam will get closer together. But if you are doing a linear static analysis, that behavior is ignored because of the "small deformation theory" that is used in all linear static stress. It doesn't matter if the vertical displacement is 1/100 of the span or 1000 times the span, the distance between the ends will remain the same -- in linear static stress. Mathematically, the beam gets longer as it deflects.

If you are pushing the beam enough that the change in distance between the ends of the beam is important, then you need to perform a nonlinear analysis where "large displacement" affect the results.