Rotation on expanded nodes on a shell


I have imposed a rotation around Z axis on a thick shell around point 1.
It is a thick QUAD8 shell element.
I have scaled the deformation view just some steps before blowing

¿How is it possible that new expanded middle nodes 36 and 37 are rotating?. I thought that once expanded, shells became solids and lose their rotational internal degrees of freedom?

¿By other hand, Is it possible to check how the normal (normals) change on a node during the nonlinear analisys.?

Thank you.

Note: I have managed to make a shell rotate eight revolutions but I still do not fully understand why it works.

I just realized that this is happening in Linear shells too. Nodes belonging to the same elements as the reference node probably keep their rotational degree of freedom (the one needed by the ref node to rotate). That makes the normal on the REF point to misalign and mess the convergence.
¿Could some developer check if the rotational degrees of freedom of contiguous node to the REF node are constrained.?

i’m only quick view and took simple test. it seems shell element can not be imposed in plane rotational, only out of plane rotational movement is accepted.

this may similar to 2D classical shell element, in plane rotational stifness only given as fictitious and small values for numerical stability purpose. but i may look further about drilling d.o.f

Hi Xyont,

I have stiffed the area with two beam elements to see if I can control de Z rotation of those two neighbors to the Reference node and I can see the effect propagates then to all the shell.(See vid). It is not a local effect. It is a global effect. The Z rotation (drillin) on the nodes of the shell are not constrained although I have impose an Homogeneous Condition *BOUNDARY before the step for all the plate nodes except the reference node





For all the nodes except



¿Am I understanding something wrong?.

I have the same effect on Rigid body on shells. Manual says : “The rigid body definition ensures that the distance between any pair of nodes belonging to the body does not change during deformation. This means that the degrees of freedom are reduced to six: three translational and three rotational degrees of freedom.”

This doesn’t seem to be satisfied here.

This are a very good news!!. ¿Do you have any simple example of a rotating shell out of plane.?

maybe i misunderstood, looking the deformation and displacement arrow of expanded shell element shown an imposed rotation around X axis not Z axis as you described. so it does out of plane rotation, not in plane rotation.

my model using quadratic triangular shell element adapt to similar cases, shown only node with imposed rotation affected. how about 2D classical element results, also continuum shell in Abaqus and solid-shell in Ansys?

for shell and beam element, the result shown this only apply to nodes at midside plane and center lines of element respectively.

According to the documentation, CalculiX’s new classical shell element is meant only for linear analyses with small deformations. Its formulation is based on the article “A three-node shell element based on the discrete shear gap and assumed natural deviatoric strain approaches” by G. Rama et al. so it should be rather easy to find the details.

Continuum shell elements in Abaqus have only 3 DOFs. Here’s what the documentation says about conventional shells in that software:

Shell elements in Abaqus use a small penalty stiffness to control drill rotations. When used, the drill stiffness is proportional to the transverse shear stiffness. Drill stiffness is not needed for a five degree-of-freedom shell element unless three global rotation components are active on the element.

Thanks Xyont and Calc_em for your comments,


Sorry Xyont, probably the view was not the best. I confirm I’m rotating around Z axis not X. In plane rotation. You can see the global Axis Coordinate in the right bottom corner of the first two pictures.

I have identified two issues that made my rotations failed.

1-ISSUE- Nodes drilling around the axis of revolution. It is a global effect but especially in the REF node. From my point of view the Drill should be constrained or artificially stiffened as Calc_em suggest. An ortho shell with high stiffness in transverse direction partially helps but would need to be recoded. I have no other way to fix it.

2-ISSUE -It is related with the update of the local axis on the ref node. If the local coordinates XY doesn’t update during the rotation, the displacement vector is always pointing in the initial direction in such a way that the plate rotates but only up to the point (close to 70º) where the plate finds its equilibrium. See vid. To fix this I forced the REF node to update its local axis on each iteration. It works with plane shells. Curved shells are giving me problems.

This is where I have arrived so far.
My approach to the rigid body rotation of shells is completely based on their behavior just before the convergence failed and probably not very rigurous.
Rigid Body rotation is in my opinion very simple to compare with other software. It works, or not. There is no midterm or % of accuracy to compare like it happens with Stresses, energy or temperature outputs. I hope it help other users or maybe suggest other approaches.

it’s puzzling me. 2D meshed plate models at fig.1 shown lie in XY plane, node 1 is apply rotation. then expanded result shown in fig2. node 1 (old) at the first become node 1,2&3 shown with displacement arrow. node 1 (new) displaced -Y (neg) and node 3 displaced +Y. (pos) so this mean rotational has been applied around X axes not Z. it does out of plane rotation not in plane (drilling)

please, attach some input file rather than videos (i’m not yet download &seeing). thanks

No, that shows the issue number 1, the nodes that define the axis of rotation 1,3, missalign because 36 and 37 are drilling. Constraining nodes at midside plane and centerlines is not enought. You have a children’s rocker there.