Good Idea !!
Frequency is showing that there is no issue on the transition between the solid and shell, but there is something wrong going on precisely where I’m pointing. In the connection between the two shells. There is a gap. They share the nodes but are poorly connected once expanded.
That makes working with shells even harder.
¿couldn’t this be done automatically? At least for the most common 90º connection. One makes some efforts creating conformal meshes to find there is a gap in the connection anyway.
The line of nodes where the joint was defined is still together, no way the other nodes in the expansion follow exactly the same line in both parts since offset does not represent a physical connection but a representation of shell’s inertia, that’s one of the reasons why angle brackets made of shells do not have representative stiffness at the corner (less stiffer).
In fact most element shape functions have incompatible modes so in fact common element edges do not deform equally and you see them in the visualization of the post processor as the same line just for simplification, but the mathematical function does not give the same values, so you have element edges open because displacements are solved at the nodes only.
They’re only joined at the nodes, right? So you’d expect them to have different displacements in the adjacent nodes when the load is trying to bend them apart from each other. Am I missing something? The pictures with the wedge-shaped gap look correct to me.
this also known as rigid end zone, can be exist at frame or shell intersection.
for direct connection and to simplified the process without losing it’s accuracy, the zone of intersection need to be split/partition and multiplied the stiffness to be e.g ten times higher by adjustment.
multiplier factor is depend on stiffness ratio (thickness & material) between adjacent member connected.
but this approach still can over-stiffen the model at the edge line shell intersection in longitudinal direction.
look like common and simple problem were actually is not, separated the mesh and constraint equation need to be formulated for classical element type.
fortunately, CalculiX use shell continuum (expanded) so tie constraint or tied contact easy to use and give better results.
I’m joining two shells at 90º and no matter where I look at it seems to perform better to tie both shells than sharing common nodes and place them with an offset. My complain was basically that one spends some time preparing a conformal mesh to realize it might be a waste of time.
I see what you mean. It is a bit disappointing that the “worse” way ends up better.
The way I think of offset shells is as if there are rigid beams normal to the shell’s surface and connecting it to the mesh nodes, so the location of the connection can be far away from the offset elements on sharp corners.