MSC Nastran; Patran Tutorial - Buckling; Flat Plates Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

in this video I will be performing a
buckling analysis on this flat plate
full details of this exercise are on
page four zero seven of the PDF linked
in the video description below I'll go
ahead and start a new patron session the
units for this example are in inches
pounds in psi start a new file save it
to a folder here call it problem 18
click OK here and first I'll create a
surface defining the entire plate using
the XYZ method here the play has a width
of 16 a height of 4 and a depth of 0 I'd
apply now I'll create a separate group
by going to group create I'll call this
quarter section because in this example
we're modeling just a quarter section of
it make sure you have make current and
then this there won't be anything in
this group so click apply so now what I
have are two different groups so how
that one default group at that surface
and now a quarter section doesn't have
anything
I'll make sure quarter section is made
set to current click OK on this group
tab I'll make another surface that goes
up 8 inches in the X 2 inches on the
wines around the Z and here my origin is
at 8 to 0 close it and hit apply so this
is a quarter section will be a plane
within this example so I'll focus here
I'll first create my properties so under
isotropic create one called mat and your
input properties give it a Young's
modulus of ten e6 and 0.33 click OK and
hit apply to create this material now
let's apply this material to the section
so here under 2d properties click shell
call this prop under info properties
let's use this material and skip it a
thickness of 0.1 inches click OK your
application region and select this
surface notice it's a change this color
indicating we've selected it so surface
2 added ok and apply now we can go ahead
and define your boundary conditions
since we're defining a quarter section
we need to apply symmetric conditions
here and here so select nodal
displacement constraint here under new
set name call it sin Y for your input
data let's go ahead and restrain
movement in the x-direction leave
everything else blank
it's prevented rotation about the the
y&z so type in a 0 for the 5th and the
6th and these are commas in between the
values click OK for your application
region we only want to select curves so
select this icon here you notice only
allow me to select the curves
now let me hide this other section it's
conflicting with the picking when you
turn off groups on and off it pops up
those stab you can use counsel that here
select this curve add it okay apply now
make a new one called cement SIMEX your
input data our restrain is the two
direction is constrained everything else
is buying and for rotations the the
fourth and the fifth directions or the
six directions are constrained so
there's two four and six click ok for
application regions select this curve
curve for service to added okay and
apply and now we want to add simple
supports to the outside so we'll call
this on simple support for input data we
just want to prevent translation in the
third direction and this could be just
brackets here click ok application
region to select these of outer curves
so your app curves three and two of
surface to add ok and apply now we'll go
ahead and add our pressure here and let
me go ahead and turn on the other one so
right now we're still working on the
quarter section so for pressure after
click that icon give it a name of
pressure we're working with two
dimensional elements so select 2d for
EMPA data your edge pressure will be 100
psi so click OK application region we
are working with the edges so here I can
just you know notice it's trying to pick
this entire thing but we don't want that
we just want to work with this quarter
section the game close this tab of it
open
select the screw add it select this
curve and add it okay and apply let me
really orient this in the front view
you'll see you all where we're going
with this now it's time to mesh this so
let me go to meshing apply some seeds
around the corners where the edges on
your mesh sheets like uniform the number
we're trying to get here is 24 for the
these top and bottom curves and we're
trying to get six along the vertical
curves when I go and match this with
quad elements simply select the surface
and hit apply now you'll see that your
boundary conditions again look like
they're being applied at the nodes at
just the nodes for a better
representation go to display load bc
element props scroll down turn on show
on them only and hit apply turn on and
off your boundary conditions you'll get
a better idea of how the conditions are
actually applied to your mesh let me go
back to the front view and view the
actual tire section so here we've
defined one for this of the section with
appropriate boundary conditions so now
we can perform our analysis so go to
analysis and select entire model for
solution type select the buckling here
it should be 105 click OK and select
apply
once that comes in good access results
click X DB hit apply and imports results
go to the results tab here you'll notice
on my buckling factors 6.1 33 and here I
can view the eigenvectors translational
but before that I'll actually modify my
pressure to reflect this new buckling
factor so the 613 click OK and apply and
the way I did that it was a here on the
model tree I just right click then
modify the a data and Phi's them in
you'll see a 613 throughout the edge
here let me reanalyze this let me
replace the old files let me we import
the xeb file I'm going to go to results
notice my buckling factors now one let
me turn off the boundary conditions let
me show the fringe and the deformation
resolve for translational eigenvectors
now this is what I get when we compare
this exercise that is in fact what we do
get 613 pounds per inch make sure to
save this and this concludes this video