In this section, we will cover the third mandatory check
that is known as the buckling analysis check. In
the buckling analysis check,
the stresses are dominantly...
The dominant stresses are compressive.
This situation easily occurs in the case of vessel under
external pressure, but it can also occur in vessel under
internal pressure.
Near to the discontinuities, the dominant stresses
could be compressive and there are chances of
local buckling occurring typically at the crown to knuckle
junction of torispherical
head of a pressure vessel can fail under buckling
under internal pressure.
However, most of the cases you will be looking into external
pressure loading for doing this analysis. The buckling analysis
can be performed using three alternative approaches.
The first one is elastic buckling.
The second is Elastic Plastic and the last one is a particular
variation of Elastic Plastic analysis known as collapse analysis.
The elastic buckling analysis as the name suggests uses the
perfectly elastic material model. Elastic Plastic uses the
elastic plastic model and the last one in addition to Elastic
Plastic model considers the geometric inaccuracies
which can exist
in the model. In this section we'll be covering the elastic
buckling analysis.
We will illustrate the approach by using an actual case.
We are considering a cylindrical vessel
subjected to external pressure of 0.10135 MPa. The
dimensions of the vessel are as given here.
The first step is to create a geometric model.
In this case, the geometric model is created using surface
geometry rather than actual three-dimensional geometry.
This will allow us to use the surface elements or
2-dimensional elements which will make the computational
solution time much smaller.
The next step is to create the finite element
mesh.
The mesh should be of sufficient discretization size so that
the proper results are obtained.
The actual details of buckling analysis are not covered in
this session.
However, to just summarize, the first step is what is known
as the preload step in which the model is subjected to the
design pressure load.
In this case, the external pressure is applied on the
model with the proper boundary conditions and the initial deformation
of the model is obtained.
This is used for the subsequent state which is known as
eigenvalue analysis
to determine the buckling load. The next is to create the
buckling step.
Please note that this particular analysis is carried out
under Abacus software,
so the interface screens are corresponding to that software.
You have to mention how many eigenvalues
which corresponds to the different buckling shapes which
you're interested in.
In this case, the three eigenvalues have been mentioned
in the design and you have to apply, what is known as perturbation
load, to the actual boundary condition which is applied earlier.
Under this perturbation load you will get the different
buckling mode shapes and their corresponding eigenvalues.
The first buckling mode corresponds to formation of two
lobes, the second buckling mode is identical to the first mode
except that the orientation of the lobes is different,
and the third mode is having 3 number of lobes.
The value of the buckling pressure is obtained by using the
first mode or the lowest eigenvalue mode.
The buckling load can be calculated using the pre-load, which
is, the design pressure what you've considered and the eigenvalue
times the cultivation load which is used for the eigenvalue
analysis. In our case, the buckling pressure is computed
as 0.9263 MPa.
This is the pressure which the finite element analysis
prescribes... it predicts that the buckling will occur at this particular
pressure. This pressure needs to be compared with the factored
design pressure.
You have to calculate the design factor and using that
you can calculate the factor design pressure, which is
0.253 MPa. Since our buckling pressure is higher than the
factor design pressure the buckling... the particular geometry
is safe against the given external design pressure.
This overall summarizes how the elastic buckling analysis
can be done. In the Elastic Plastic buckling analysis,
you will be using elastic plastic material and some more
adjustments and changes in design factors are involved.
