Gap on Offset shells
Hi,
I have two shells at 90º sharing the same nodes at the connection line. When I apply some bending, the common line is rigid as it should, and they do not rotate one with respect the other. See image.
By other hand, if shells are offset, it happens that now both shells open. That makes them so separate and shows a gap. See vid.
¿Is that intentional? ¿I think that gap shouldn’t be there?
What if you switch to 2D output for that case with offset ? Does it still show a gap ?
Do you mean to request?
*NODE FILE, OUTPUT=2D
If I do that and later expand the thickness of the model it doesn’t show the Offset geometry but the original. Not sure if this is ccx or MECWAY limitation?
Yes and then take a look at the mesh consisting of 2D (not expanded) elements:
Maybe *Frequency could also help with the visualization of this gap.
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.
Here can be better seen what I mean.
2D Model. Nodes between shells perfectly connected.
it seems the deformation has shown small gaps are due to knot generation and compatibility, face at the edge of vertical plates rotation is equal to horizontal plates.
this is common in shell element at the model with sharp corner, similar to classical type also. however, in solid model it may not happen.
to get similar behavior as solid, someone can use tie constraint or ted contact type instead direct connection both members with sharing common nodes.
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.
consequently more work is needed to get better accuracy, did it uncommon in FEA?
fortunately, it seems using auto search contact surface in CGX and PrePoMax can tackle easily by single command or click.
above example are for quick testing of tie constraint, shell element (S6) still need to be layering to improve.
Mmmh.
You know displacements almost always look right. 
it’s only simple test of using tie constraint, rigid body makes over-stiffening the model and remove warping effect.
below another test in frequency analysis,
sure. this threads about shell element.
i’m using auto search contact feature in PrePoMax
however, CGX also have similar feature and capabilities.
download link of INP files of layered shell models,
Thanks, I will try to import in Pmx
i posted an INP files not PMX cause of more general, can be read on Linux also.
some notes about the model examples, always de-active any nonlinearity e.g NLGEOM. switching to tied contact type also. it will divergences.
it seems the problems are due to over-constraining in rigid body available. need to use nodal force or coupling to make it work.
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.
Thanks.
It is not intuitive at all that a contact can perform better than having a commond node.
Thanks too. I made it with Mecway, I’m more used too.
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.
HI @vicmw ,
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.
