Could anybody explain me role which plays perturbation parameter in general step settings for buckling I know that we have linear elastic buckling analysis (LBA ) and non linear buckling analysis but this parameter for me is not clear . How it impact on analysis , how model behave etc…
when I turn on this parameter is it fully non linear buckling analysis for given load ?
thanks in advance for explanation
This parameter is just to include preload (from a previous static/dynamic step) in a linear buckling analysis:
If the perturbation parameter is not activated on the *STEP card, the initial stiffness matrix corresponds to the stiffness matrix of the unloaded structure. If the perturbation parameter is activated, the initial stiffness matrix includes the deformation and stress stiffness matrix corresponding to the deformation and stress at the end of the last static or dynamic step performed previous to the buckling step, if any, and the material parameters are based on the temperature at the end of that step. In this way, the effect of previous loadings can be included in the buckling analysis.
thanks for info but I still do not know if it is full nonlinear buckling, I’m asking since I have different results from creo simulate and from PPM/CCX. difference is significant
No, as I’ve mentioned, it’s still a linear buckling analysis, only with preload included. Nonlinear buckling analysis requires static or dynamic step with Nlgeom enabled.
ok thanks . but results with turned on perturbation parameter differ from turned off . which one is correct I mean LBA
best regards
Do you have another step before the buckling one ? Then they should indeed differ. Otherwise, you don’t have to use this parameter.
I have done simple LBA in creo software and results was BLF 0,45 first shape and I have done exactly the same calculations in Prepomax/ calculix and got BLF for LBA 0,98 more less . I think that the difference is to much. (the same 3d model the same loads materials boundary conditions and so on) .I have heard that calculix had some issues with this type of analysis in the past. Is calculix reliable software for which I can rely on ?
Can you share the file ? Usually, it’s a matter of differences between the models but occasional issues may also occur in CalculiX: First buckling mode skipped when applied load is much bigger than buckling load · Issue #74 · Dhondtguido/CalculiX · GitHub
It might be better to apply unit load in this type of analysis.
I can not share model (company policy) but I have done static analysis in first step and stresses and displacements were identical when compare to Creo simulate so I assume that model is more less the same but BLF is some kind of surprise
best regards
As I’ve mentioned, try with different loads (especially unit load) to get different buckling factors. You can also try adjusting the accuracy parameter: Changes in *BUCKLE definition · Issue #57 · Dhondtguido/CalculiX · GitHub and using other matrix solvers.
Is the mode shape different too ?
I can not also take into account unit load (load significantly smaller than critical lad to skip calculix issue ) since it is not simple column with axial load . It is crane boom with complex geometry and load . So using single unit load I think impossible ( if you had similar example please let me know)
best regards
I would break it into individual load cases anyway. Then you could check which load has the most significant effect and make comparisons with unit values. Plus try what I mentioned above (especially changing the solver).
I have made buckling analysis again with proportional decreasing of acting loads (each force was decreased to 10%of value) with settings only one shape to calculate.Also accuracy parameter was increased to 0,00001 and BLF is 4,1 when I compare to creo simulate where BLF is 0,45 (for 100%load value) it is more less ok ( 0,41 vs 0,45). I confirm issue with buckling analysis in calculix . What to do in non linear buckling ? Has someone any idea how to skip this problem in non linear buckling analysis .
best regards
The issue with the first buckling modes being skipped occurs only in linear buckling analyses. As I’ve mentioned before, nonlinear buckling ones are just static or dynamic steps with Nlgeom on. There you shouldn’t have issues like this but you may e.g. encounter non-convergence if shells and rigid body constraints are used together.
Besides convergence, one of the most important issues in nonliner buckling analysis is it’s dependence on imperfections. You can’t be sure to be on the safe side.
Anything like geometrical imperfections, load excentricities or lateral loads (wind) or residual stresses from welding may trigger buckling modes.
So if you never did that, don’t dare to do that unassisted.
1 Like
Do not be so afraid I have over 20 year experience in design steel constructions…
my experiences in FE nonlinear buckling analysis are gaining insight to the true behavior. Profiled sections can be predicted better, thin shell structure like a tank is more hard due to sensitivity of imperfections.