Model shell together with frame element so that their connection work

[kristjan]

I must repeat my question on another way.
Last time i asked how we can model wall of brick together with other frame element in software sap 2000.
I try to shell + frame element. But their connection didn’t work.
If I assume simple egzample: simple beam(frame) and wall of brick(shell) above. And if I divide beam as mesh shell by 10 elements I get their connection. So when i run analysis i get results which not coinside with results get by hand. M of sap not equal M by hand (M hand=(1/8)*q*l^2) Only reactions is correct. What can i do? Is this software have solution whose i don’t know!
I be appreciate if anyone says something more about this problem.

 

[vonlueke]

The following answer assumes your beam is simply-supported, which would indeed have a midspan moment of M = (1/8)*q*L^2.

My assumption is, you are misinterpreting the output of your software and/or computing the resultant moment from the results of your finite elements at midspan incorrectly. Let's say the beam axial direction is the global x direction in your model and the y direction is the vertical axis.

Unless your software will compute the moment resultant of multiple elements at a section cut for you, you must obtain the x-direction element forces in your model at midspan, and the beam element moment about the z axis, draw these forces on a free-body diagram, calculate the centroid of your elements at the midspan section cut, then calculate the resultant moment of all x-direction element forces and the z-direction beam element moment about the centroid of the section-cut cross section.

When you do this correctly, it's supposed to produce approximately the same answer as your hand analysis, M = (1/8)*q*L^2. If it is only slightly inaccurate, then you might try repeating it again except dividing the beam into 20 or 30 elements instead of 10. Good luck.

 

[vonlueke]

Note: If your beam (material 1) and shell (material 2) elements have different moduli of elasticity (E1 and E2, respectively), to find the centroid (or rather neutral axis), mentioned above, of the composite cross section at the midspan section cut, you must first transform (in your hand calculations) one of the two materials to the other material.

To transform material 2 to material 1, multiply the width b of material 2 in the cross section by n = E2/E1. Then proceed as described in the previous post to calculate the centroid of your elements at the midspan section cut. (Width b here in my example would be thickness t of your shell elements.)

By the way, forces and moments will come out correctly on the transformed cross section, as will stresses on the nontransformed material (material 1), but stresses on the transformed material (material 2)--if you calculate any stresses by hand on the transformed cross section--must be transformed back by multiplying any computed stress on material 2 by n.

 

[ishvaaag]

The case where you want a simply supported beam you easily solve by releasing bending moments at ends.

When you want to portrait elastical fixity to the shell, if the shell elements are defined only by vertices you need to use finer mesh and therein suplementary rigid link members artistically joined to your end of member to pass the forces readily to the shell. This may happen with both in-plane and out of plane members, but it is not very difficult to get reasonable values of the end forces in the member with not too much complicated models. Of course, the fake zone in the shell and around has incorrect stress values and this needs be accounted for with extrapolation, some acceptance of redistribution (only maybe) and wahatever sound engineering judgement deems proper.