@Disla, thank you for your reply and further information.
How did you capture the axisymmetric (n=0) buckling image with 15 longitudinal waves? Was that intentional, i.e. a pre-arranged geometric imperfection which produced this?
I did not quite understand the volume integral graphic under this image, which seems to be exponentially increasing towards the end of the analysis but suddenly went back to its initial value.
No, the BC were not changed when moving to nonlinear analysis and the base was still fixed. There is a large amount of deformation at the lower edge which is probably the reason you assumed the edge was not constrained.
I had not realized that Donnell’s theory has a nonlinear side as well as linear. I am not sure which one is used to obtain the above formula to predict the buckling load for a thin cylindrical shell under axial compression.
i did several tests on nonlinear buckling with shell element, assign rotational restraint in local coordinates is working expected overal, only few sections type with small radii at corner have some problem in convergences.
That emerge naturally when I perform the NLBA without imperfections.
Thats the overall Internal Strain Energy. It helps me to identify the buckling triggering point. In some cases it’s cleaner than looking at deformations.
Maybe you have scaled the imperfections too far or aplied the axial compression to agressively.
Displacement added 1000?¿?. Thats a lot.
Did you transfer the modeshape directly from the result?
The state of perfect geometry did not buckle is not always true. Allthough imperfection not being used, still buckling can occors due to geometry or mesh is not perfectly simetric, numerical rounding by the solver known as the reason even in symetric conditon..
Order of displacements in the mode is 10^-3 which ends up in adding a displacement in the order of 10 mm to a mesh with diameter 3200+ mm, thickness 25 mm. It is not noticable with eye (maybe a younger eye will see it:) So, I don’t see any problem with that.
Confirmed. We have obtained converging solutions even when no displacement is added (with perfect analytical geometry). And thanks @xyont for pointing out your topic on solver comparison.
We would like to proceed with changing from SHELL to SOLID, starting with a double layer. But before that probably halving of the mesh size as recommended above will be good to see the correlation between the mesh and mode shape resolutions.
Imperfection amplitude is usually taken as a percent of the shell thickness (something like 10-15% for instance).
Btw. sometimes imperfections are introduced as a superposition of a few initial modes with different scales, but doing that in CalculiX is not so straightforward.
So far, based on the above discussion it was decided to solve the plain cylinder (without holes) and shown that the modal analysis was in agreement with Donnell’s equation.
Subsequently, two S4 meshes with different refinements were used in the nonlinear analyses, where the cylinder is subjected to a displacement controlled axial compression of 100 mm (roughly 1% of its length). You can find the input files below.
Interestingly, the relatively coarse mesh (lc=128) converged up to 56% of the total displacement, while the finer mesh (lc=64) only converged up to 26% of the total displacement.
Actually, you are using S4R (reduced integration) elements that are not recommended for buckling analyses in CalculiX. Try with S4 (fully integrated).
As long as you are not overconstraining shell elements or using nonlinear (e.g. rigid body) constraints with them, it should be fine. But you can try solids too just in case.
With plasticity, you would have GMNA or GMNIA analysis (depending on whether you also include imperfections). Then the model may yield before it buckles and convergence will probably be worse.
i’m using quadratic shell element with reduced integration (S8R) and composite option activated to define number of four layer in use..
imperfection is considered by deformed mesh saved from multiple combination of unrestrained eigenfrequiency analysis. Indeed, plasticity also being considered in my previous analysis. rotational restraint in local coordinates system seems a common problem issue in CalculiX,/ Even it has been defined properly, still at specific condition led to some problem but overal case is working properly.
Sorry about my mistake, indeed the element-type used in the previous post results were S4R. Correcting this to S4 yielded better convergence but still not full convergence. (This is explained below, and we choose to deal with plasticity later @Calc_em)
And thanks to @xyont for sharing the element type and layer information in his reply. We appreciate this information, though I am not sure if increasing the number of layers would have a positive implication for convergence?
Changing the element type from S4R to S4, we show the responses from two cases:
A coarse mesh (lc=128) of a plain cylinder
A finer mesh (lc=64) of a plain cylinder with added deformation of buckling mode #4 shown below (max deformation does not exceed half the cylinder thickness)
Both cases fail to converge beyond 86-88% of the applied displacement, with a reaction force-displacement curve below
The deformation in direction-1 is shown for both cases. On the right the finer mesh has obvious deformation pattern in agreement with the overloaded mode. But more interesting agreement between the two cases show an eminent regional circumferential swelling parallel to the lower and upper edges. This pattern is independent from the mode #4 deformation.
Moreover, looking at the stress plots (von Mises) confirms the similarity between the two solutions (coarse and fine mesh) despite the fact that no extra modal deformation was superimposed on the coarse mesh, in contrast with the fine one.
Maybe you should try with larger imperfection amplitude and even different pattern of imperfections. Shells are particularly sensitive to that.
Perhaps a different (more flexible) way of constraining the edges would be better.
Keep in mind that a regular NR solver like this may not be able to converge past the bifurcation point. Arc-length solver would be best, but CalculiX doesn’t have it yet.
Linear buckling can be very inaccurate and misleading in some cases, especially for imperfection-sensitive shells and when nonlinear behavior prior to buckling is important.
I think you should check if your mesh density and element type is adequate for the problem at hand. Maybe you need to refine and/or use second order elements.
Check stress error results for guidance. I’d prefer to have available non averaged results, so you can check mesh convergence at a glance. Maybe in a near future…
“Buckling and collapse are identical states for isotropic circular cylinders subjected to axial
compression”. [NASA/SP-8007-2020/REV 2]
-“Critical axial stress is determined by dividing 𝑁𝑥 by the shell thickness t”. That means it is a mean membrane Stress. Check *NODE FILE OUTPUT 2D (It removes the bending Stress.) if you want to compare with the analitical solution or compute it by dividing 𝑁cr by the shell thickness t.
¿?. Tell your student to double check that value and build a good quad regular mesh. It has alrready been recomended/suggested in several ways.
If you use Gmsh then you should be able to get a regular quad mesh with the Quasi-structured quad algorithm. Irregular meshing is sometimes used to introduce mesh imperfections, but shouldn’t be necessary in this case. Even with geometric imperfections (dimples) from linear buckling, the mesh can be nicely structured.
Some users prefer to have more control over imperfections and apply them by directly morphing the mesh with scripts, but your approach with linear buckling should still work if you use a good mesh and constraints/BCs.
hi, could you repost mesh file of this model at the same mesh density for both w/o cut outs? it seems the problem is not always in mesh regularity since quadratic element can deal with these conditions. Interesting to conduct study of imperfection sensitivity to get lower/upper bound values compared to steel design code regulations.
Thank you for your interest. The mesh file for this model is gmsh_hls7.inp, and one without cutouts is noholes_S8R_256.inp. Both files are shared below.
first look about the problems, it seems the model is almost perfect in geometry and loads made it stiff enough to generate buckling form, required imperfection to capture these conditions. Model of medium mesh with quadratic shell element (reduced) and composite option activated still divergences even reach higher than finer mesh of linear shell element.
modeling imperfection as 10mm maximum still not convergences, it seems due to elastic material in use i.e no plasticity defined make the model still in stiff enough led to no relaxing or stress redistribution did not occur.
byw , what probable steel yield strength being used, is that high strength type? the behavior can be considerably differed with old reference reported in sixty era.
*edited, updated
example using S450 steel grades with plastic definition is convergences.
