MSC Nastran; Patran Tutorial - Buckling; shells and Cylindrical Coordinates Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

this example will be performing a
buckling analysis using shells and
cylindrical coordinates full details of
this exercise drawing page 405 in the
PDF link in the video description below
I'll begin by starting patran and the
units for this example are in inches
pounds and PSI I'll call this database
problem 17 hit OK on the form on the
right and I'll first define my geometry
so I'll make a curve using the line by
XYZ method the radius of this cylinder
is 5 so I'll type in 0 for the X 5 for
the y 0 for the Z and I'll start from
the origin next I want to rotate this or
revolve it about the z axis so that
would be the third direction for
coordinate system 0 I'm going to rotate
it 180 degrees and I'll select this
curve so this is one of the caps for the
cylinder next thing I want to do is
create the rest of the cylinder as shown
so under your surfaces i'll select
extrude my translation factor view it
will be 0 on the x and y and negative 20
and z and for my curve list i'll select
this curve next I'll want to define my
last cap here for the cylinder to do
this I go to transform surface for my
direction vector I select 0 in the X&Y
negative 20 and Z and I'll select the
surface and that's defining my slender
so far I'll create my cylindrical
coordinate system by going to
coordinates three point and selecting
under types cylindrical accept the
default values here and hit apply now
what I want to do is look at my normals
for this interaction go to show surface
normal and here under surface list
either pick all or individually pick the
surfaces to make this easier on us hit
the surface icon here so the only thing
you pick are surfaces and since auto
execute is on and performed operation
automatically so this is what we have in
regards to normals for this uncap the
normals into the cylinder let me shade
this for this cylinder section the
normals inward but for this end cap the
normal is actually the outward when we
define our pressure it's important that
we have all of these normals facing
inward so what I'll go ahead and do is
modify this uncap surface so here go to
edit object the surface and under method
go to reverse I'll select this surface I
draw the normal vectors to see it again
you see its outward after I select this
surface and hit apply and I draw the
normal vectors again now the normal is
pointing inward so when I go and define
my pressure
give it the name pressure target element
type is two-dimensional for EMPA data my
top pressure is negative 100 hit OK for
application region select the surface
icon and pick all surface one through
three are added to the application
region hit apply now my pressure is
defined in word for each surface if the
normal for this uncap were to be
pointing the other direction the
pressure here would actually point
outward and we didn't want that so we
corrected it now going back to geometry
we've defined the geometry we can move
on to properties for my material I'll
create an isotropic one I'll call it
matte under input properties rings
modulus is 10 e 6 and my Poisson ratio
is 0.33 hit OK and hit apply now define
my two-dimensional properties so here
under shell property set names prop
under input properties use the material
with just me to give it the thickness of
0.125 inches for your application region
make sure you have surface selected here
pick surfaces 1 through 3 added to the
application region select ok and hit
apply now I can continue on with this by
defining my displacement constraints
under new set name create one called
tangential for EMPA data' prevent
translation in the second direction and
prevent rotations about the third
direction
and we are not using the coordinate
system zero we're using the cylindrical
1 coordinate system one hit okay for
application region we wish to select all
of these edges here so click curve or
edge here so the only thing you can pick
are curves I'll simply drag and select
and I'll add it and you'll see added
these two extra surfaces or edges so I
can select this one click remove select
this one and remove and you see that the
orange highlight it curves out of the
ones that are included in the
application region and it's important
that you make sure that these four edges
are inside of here hit okay and hit
apply next we want to define a radial
constraint so call this x1 radial under
NP data I'm going to prevent translation
in the one two and three directions
I'll leave the rotations blank the
analysis coordinate frame is one for
application region we want to select two
points the center point and the center
point hold the shift key to select
multiple entities click Add ok and apply
and if I go to the model tree expand the
LDCs I can turn off the tangential
condition and I can see my radial
condition here so it's been applied to
these two points next I'm needed to find
one last condition but that will have to
wait until I mess this moving on to the
meshing tab I'm going to define a
requirement that says 12 elements along
a few curves so click mesh seeds uniform
leave Otto execute on so when I pick a
curve automatically makes a seed so I
want 12 elements here I want 12 elements
on this curve but you don't notice there
are two curves so I want to do that yet
here I want 12 elements here again add
two curves so I have to change this to
six I'm going to select this curve I'll
make six and when I select this curve
I'll make another six and the same for
this curve and the scurb I want twenty
elements along this length and twenty
elements along this length so now when I
go and use the surface measure use quad
quad for well after you use a different
measure for each section for the hole
use quad elements and select the this
middle surface here surface two and hit
apply for your end caps switch it to
tria and this time you'll select surface
three apply to mesh and then the surface
surface one and apply to mesh and one
thing we have to always do is head of
equivalence to remove any duplicate
nodes you'll find that it's delete aslim
here and on the side too
I'll go ahead and reorient this so I
look at it from the side and I'll have
to define my last boundary condition so
under nodal displacement constraint I'll
call this one Center axial my input data
I'll prevent movement in the third
Direction four coordinate system one
click okay this time instead of the
geometry will apply this to the FEM
where the nodes make sure notes is
selected here and pick and select the
metal nodes now if you're skeptical
you've chosen the wrong one where you
can do is under meshing you can go to
actions show no location and we know
that the hole is 20 inches in length so
we know we need to pick the nodes at 10
inches so here it is 10 inches so I've
select the right one let me actually
reorient this again
so that would be this this set of notes
is along where we have to apply our
boundary condition go back here apply to
these add okay and apply let me turn on
the other boundary conditions and let me
turn on the pressure now to get a better
idea of how the boundary conditions are
applied you can go to display load BC
element props here check on show on
phenylene hit apply clean it up turn
these off and on you'll see the
constraints here then you can see the
pressure here and again the pressure
should be applied in Word
I mean uncheck or I'll leave that on now
can go ahead and analyze this or before
I do that if you will call in a cell the
location of a node it's currently using
the global system for the reference and
analysis coordinate system I'll go ahead
and use the cylindrical coordinate
system so under action modify object is
node method is edit and under analysis
and reference I'll select as corn a
system called cord one for my noodle
Isola nodes and hit apply here I get the
feedback all the nodes have been
modified and now I'm ready to analyze
this under to the analysis tab go to
analyze entire model under solution type
switch it to buckling and hit ok on your
sub cases select default and make sure
it's been dropped here so it says
default here to your sub case parameters
this is not a back in solution type go
to solution parameters
under eigenvalue extraction we want a
limit of 100 for the eigenvalue range
I'll click OK here okay here okay here
and I'll hit apply it's analyzed this
once that's done can click X DB and put
the results go to the results tab click
on quick plot fringe and here you can
already tell well my buckling factor is
and I'll simply view the results really
quickly and here what I have to do next
is multiply the pressure I apply it by
this factor and that would be the actual
load at which this cylinder buckles so
here they had a value of a theoretically
256 psi when in fact they should get a
270 psi so if I take this value I'll
round it up to 2.7 I go back to my
pressure and I can multiply this by 2.7
or what I'll do instead is I'll modify
the load case
so here for the pressure it currently
has a scale factor of 1 I can change it
to 2.7 and you can click OK or hit
applier and I'll take the new value so
when I go back to analysis and analyze
the entire model Oh take that 2.7
multiply it with the original pressure
of 104 over resulting pressure 270 psi
and when I import my X DB results and
view the results again my buckling
factor is approximately 1 and the
buckling shape is almost the same and if
you want to clean this up you can go to
deformation attributes and uncheck show
undeformed if you want to see the mush
on the deformed shape you can come to
French attributes here switch this
element edges and here you can see that
the geometry still there and I can high
bat by going to home and hitting plot
your race geometry and now you see the
green line of the geometry is now gone
if you want to bring it back you can
click it and it's back again and just to
show you again I'll guess a lot and do
it the other way
there you go that's a buckling example
make sure to save and that concludes
this example