Hi disco,
the corrected input file follows. I have made several modifications:
missing second line: job description
3dshell domain has 6 DOFs per node (adjusted bc arrays accordingly)
shell element is "rershell" - this is a triangular element, not quadrilateral,  I split each rectangle to two triangles.
Sixth DOF (rotation around normal) has to be supported, since elements do not  have any stiffness in this dof.
I additionally prescribe all dof corresponding to membrane behavior (u,v) and rotation around x-axis as zero, to get better results on this coarse grid. NIP allows to alter default number of integration points on element. NIP 1 is default, so can be removed.

On output the membrane and shear forces as well as the moments are related to unit length.
their order (as printed in gauss point) is: membrane forces, shear forces, bending moments, torsion moments:
nx, ny, nz (always zero),      qyz, qzx, qxy,           mx, my, mz (zero),             myz, mxz, mxy;

bp

test1_5elm.out
job description: small beam test
LinearStatic nsteps 1
domain 3dShell
OutputManager tstep_all dofman_all element_all
ndofman 12 nelem 10 ncrossSect 1 nmat 1 nbc 2 nic 0 nltf 1
node 1 coords 3  0.0   0.0   0.0  bc 6 1 1 1 1 1 1
node 2 coords 3  20.0  0.0   0.0  bc 6 1 1 0 1 0 1
node 3 coords 3  40.0  0.0   0.0  bc 6 1 1 0 1 0 1
node 4 coords 3  60.0  0.0   0.0  bc 6 1 1 0 1 0 1
node 5 coords 3  80.0  0.0   0.0  bc 6 1 1 0 1 0 1
node 6 coords 3  100.0 0.0   0.0  bc 6 1 1 0 1 0 1 load 1 2
node 7 coords 3  0.0   8.0   0.0  bc 6 1 1 1 1 1 1
node 8 coords 3  20.0  8.0   0.0  bc 6 1 1 0 1 0 1
node 9 coords 3  40.0  8.0   0.0  bc 6 1 1 0 1 0 1
node 10 coords 3 60.0  8.0   0.0  bc 6 1 1 0 1 0 1
node 11 coords 3 80.0  8.0   0.0  bc 6 1 1 0 1 0 1
node 12 coords 3 100.0 8.0   0.0  bc 6 1 1 0 1 0 1 load 1 2
rershell 1 nodes 3 1 8 7  crossSect 1 mat 1 NIP 1
rershell 2 nodes 3 1 2 8  crossSect 1 mat 1 NIP 1
rershell 3 nodes 3 2 9 8  crossSect 1 mat 1 NIP 1
rershell 4 nodes 3 2 3 9  crossSect 1 mat 1 NIP 1
rershell 5 nodes 3 3 10 9 crossSect 1 mat 1 NIP 1
rershell 6 nodes 3 3 4 10 crossSect 1 mat 1 NIP 1
rershell 7 nodes 3 4 11 10 crossSect 1 mat 1 NIP 1
rershell 8 nodes 3 4 5 11  crossSect 1 mat 1 NIP 1
rershell 9 nodes 3 5 12 11 crossSect 1 mat 1 NIP 1
rershell 10 nodes 3 5 6 12 crossSect 1 mat 1 NIP 1
SimpleCS 1 thick 2.0
IsoLE 1 d 7.85e-9 E 2.1e5 n 0.3 talpha 0.0
BoundaryCondition 1 loadTimeFunction 1 prescribedvalue 0.0
NodalLoad 2 loadTimeFunction 1 Components 6 0.0 0.0 1.0 0.0 0.0 0.0
ConstantFunction 1 f(t) 1.0

The shell element can be placed arbitrarily in space. The DOFs that I have described were related to the example, where all elements were in xy plane. To be more general, the shell element has 5 DOFs per node: three displacements and two rotations around local axes that lie in element plane.

Borek

Hi Disco,

The shell element we are using is simply constant curvature plate+constant strain membrane. Suppose that the element is in xy plane, then DOFs that came from membrane are u_x, u_y displacements, and from plate behaviour u_w, fi_x, fi_y. What is missing, is DOF related to rotation around z axis. Since there is no DOF related to this, there is no stiffness. And since you have in each node six DOFs, then the solver will assemble also an equilibrium equation for rotation around z-axis, but there will be no stiffness associated to this.
The solution is to avoid assembling equlibrium equations related to rotation aroun z-axis, i.e., to prescribe these DOFS to zero by imposing boundary condition on sixth DOF.

Borek

got it

bc 6 1 1 1 1 1 1

ok thanks