According to the manual “The load speciﬁed in a *BUCKLE step should not contain prescribed displacements.”
I have done it and as far as I have tested it provides the correct buckling factor “and buckling shapes” except for the nodes affected by the displacement BC .

Seems like the solver doesn’t apply the overall scaling factor ( or normalization process) to the displacements on nodes affected by the BC.

¿Is this something that could be fixed, or does it comes from ARPACK?.
¿Could I use at least reliably the eigen values?

There are a few cases when the ccx documentation mentions that something isn’t possible or shouldn’t be done but it turns out that it works fine.

Here’s what Abaqus documentation says about this approach:

Nonzero boundary conditions prescribed in an eigenvalue buckling step will contribute to the incremental stress Δσ and, thus, will contribute to the differential initial stress stiffness. When prescribing nonzero boundary conditions, you must interpret the resulting eigenproblem carefully. Nonzero prescribed boundary conditions will be treated as constraints (i.e., as if they were fixed) during the eigenvalue extraction. Therefore, unless the prescribed boundary conditions are removed for the eigenvalue extraction by specifying buckling mode boundary conditions (see the discussion below), the mode shapes may be altered by these boundary conditions.

you can check the result by running a geometric nonlinear step for that “load level”. A sharp change in the displacements at the critical locations will show that buckling has happened.

I think, as Calc_em explains, that cannot be correct in general because you introduce constrains that are not there at the onset of the instability.

Ok. Just in case, I’m using the equivalent force (although it seems there is some small difference in the result).

Yep. That’s a second phase but I’m struggling with it.

As soon as I offset the flanges (Flange1 and Flange2) to start adjusting the model and get a better representation of the geometry the nonlinear convergence fails.

It’s working fine in static and in nonlineargeom too but only without the shells offset. Excluding the flange’s nodes from the rigid body definition doesn’t help. I have also tried different solvers and different versions of ccx. Linear and quadratic elements.

¿I would appreciate if you could you take it a look?. I think everything is properly set.

Maybe I should discard to solve the model with the shell elements.

the issue lies in the creation of the rigid body, from the manual:

If the participating nodes in a rigid body definition lie on a straight line,
the rigid body rotation about the line is not defined and an error will occur.
To remove the rotational degree of freedom, specify that the rotation about the
axis is zero. If a is a unit normal on the axis and uR is the displacement of the
ROT NODE, this results in a linear MPC of the form a.uR = 0 to be specified
by the user by means of a *EQUATION card.

Nevertheless the model seems to be too stiff even using S4R shells, try it with parabolic elements to catch the onset of buckling.

Thanks for looking at this. The problem has been puzzling me for some days.

I think Nonlinear analysis has some deeper issue with offset shells. I will pay attention if I find some other examples.
Just in case someone else finds some issues converging offset shells I have been able to solve it just creating three parts and connecting them with tie contact.

Problems suddenly disappear , convergence is then sweet again.

Thanks again for your help and merry Christmas everyone.