MSC Nastran; Patran Tutorial - Linear Static Analysis of a Composite Plate Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

[Music]
in this video I will perform a linear
static analysis on this cross ply
composite plate full details of this
exercise are on page 326 of the link PDF
in the video description below I will go
ahead and create a folder here call it
problem zero two and I'll start Patran
maximize this create a new model save it
in the same folder click OK on the form
on the right here in geometry I'll
create surfaces using the XYZ method so
from the origin I'll define a vector so
that the width of this surface is 1.5
inches then the height is 1 inch and the
units for this exercise are in pounds
inches and PSI now create I'll leave
auto execute on so all I have to do is
click this point this point and this
point to create my three other surfaces
I'll go ahead and define my materials by
going to the properties tab and clicking
2d orthotropic here I'll define my
lamina so the name I'll give this
material is lamina on your input
properties my young's modulus is 7.8 e 6
PSI my next young's modulus is 2.6 e 6
psi poisson ratio is 0.25 my shear
modulus is 1.25 be 6 my first thermal
expansion coefficient is 3.5 e to the
negative 6 second is 11 point 4 e
negative 6 a reference temperature of
this lamina
is 270 degrees Fahrenheit so now click
OK and hit apply now I've created my
lamina you can see this if you pull up
the model tree I've defined the toothy
2d orthotropic lamina so far so back in
properties I'll define my composite
laminate by clicking this icon this form
pops up I will call this laminate here
are all insert three rows the material
is lamina so I have three layers using
the lamina just to find the thickness of
the first layer is point zero five eight
inches hit enter my next thickness is
point four five eight three inches to
enter and my last thickness is point
zero five eight inches and hit enter my
orientation of the top layer is zero
next layer is nighty and the next layer
is zero here I'll select this cell and
I'll click delete select a row so I get
rid of the fourth layer click apply now
you see that my lamina has been defined
here if I click show laminate properties
I can view the abd matrices and the
various other properties here I minimize
this now I'll go ahead and apply this
laminate to the four surfaces so here
under 2d properties 2d she'll call this
composite plate under options I select
laminate here under input properties
select the laminate for the material my
material orientation will be a vector
and I'll define it as a vector going in
the X direction so 1 0 0 click OK select
application region is is applied to all
the surfaces so services 1 through 4
click Add click OK and apply now the
vector is going in this direction so
when I display parametric directions I
can tell that my normal is this way and
since the X direction or the 0 Direction
is this way the plier orientation is
positive and distraction so let me turn
this off go back to this now I will go
and define my boundary conditions so go
to this tab click displacement
constraint I'll call the first one CL y
for centerline about the Y so click
input data for translation simply
prevent translation in the X direction
click OK select application region here
click curve icon so we just pick curves
goes one goes another click ok and apply
I'll make another constraint called
centerline or CL and your score X so
restrain this line cylinder and put data
restrain the y direction click OK select
application region select this curve add
it select this curve that it click OK
and apply now wish to constrain this in
the Z direction so name a new one called
Z constrain under info data the t 1
blank
the t2 blank but zero but for the
z-direction put a zero click ok select
application region select surfaces here
click pick all it was a bad idea
click surface here there's a difference
this icon includes the point curves
surfaces and solids the surface is
exclusive to surfaces so when I click
back pick off selects all surfaces add
it ok and apply I'll go ahead and add my
in-plane lows so click distributed load
the name is NX target element type is 2d
under EMPA data people f1 will be blank
or 0 f2 will be negative 2 hundredths so
it points away and reserved for the last
one click OK
select application region select this
whole shift and select the sides notice
they turn orange
click OK and apply next I will apply my
nodal temperature so click temperature
here and I know the temperature we are
to prescribe a 70 degrees Fahrenheit so
under EMPA data type in 74 the
temperature for the application region
select make sure this is selected
surfaces then pick off so I have
surfaces 1 through 4 here and apply so
now I can turn off the markers using a
model tree now I can go ahead and mesh
this under meshing click uniform I want
the bottom surfaces here three curves
meshed with ten elements each and the
same set for these the sides I want five
elements per curve just like this
followed by this one and that's it
here under measures select surface
select pick all so you have surfaces one
thing for here and click apply
make sure to equivalence after you're
done meshing and I notice that it
removed duplicate nodes here along the
boundaries of the surfaces I can then go
to analysis analyze the entire model
here click apply to analyze this model
I'll let me first go ahead and pour my
results click X DB click apply let me
hide the model tree go to results I will
click quick plot or actually I'll click
fringe so here gonna be my stress sensor
in the X for the first layer I get let
me fix this slightly so it's easier to
read
so I get negative 6000 psi in the
extraction we compare this to the value
we are to supposedly get a theory tells
us we get approximately negative 6000
here and we go to layer two we get a
stress of - 645 psi and then you'll see
it here it's actually on on the other
side the values we're looking at right
now or the layer the local stresses so
this would be the stress and the one
direction for layer two this value for
layer three and so on
so if I would like to get the global
stresses I would need to transform the
results to the global coordinate system
so here I've gone to plot options and
select the global coordinate axis in
which the trends for my results so now
if I go to layer one see the results are
the same as before last time if I go to
layer two now I don't get the the - 645
I had before I actually get 1691 now so
now I can view the results so we view
this value this value this value and
these are global values now for this
3001 so here we would go to the Y
component view the layer one results and
click apply get a 3,000 psi
[Music]
the lair to get a 645 psi the layer 3
I'll get what I got him home and I go
3,000 psi and then for the shear
stresses here simply come here say I
want to be the X Y component you'll see
that the values are small enough where
we can say they're essentially zero I
know the friend says otherwise see the
small decimal values and filler two so
this is essentially zero now
now in the second half of the video I
would just model one fourth of the
section and make use of symmetry so let
me go back here erase that and now I'll
just model this top right section so the
first thing I have to do is go to my
meshing tab and delete the mesh here in
the finite element Attila's pick all and
apply clean it up and now let's mess
just the top right section and apply
now I must modify my boundary condition
so in the Home tab click the model tree
we will just modify the displacement
constraints for C CL underscore Y you
would right click on this and modify it
and the modification involves fixing the
rotation about the fifth direction which
would be rotation about the Y the next
thing would be to modify a seal X here
you would add an extra constraint that
would be a rotation about the X now let
me turn all the markers just to make
sure everything's in place now our
boundary conditions are applied to the
geometry but since there's no mesh for
these other three surfaces nothing
really will happen in the analysis the
focus of the analysis will be on the
Vinaya element since that's where the
boundary conditions occur so now when i
analyzes be honest to replace previous
files
we'll go ahead and clean this up and
then pour my xdb now first thing I have
to do is under fringe make sure this is
make sure I've selected stress in the
x-component and I've transformed this
into my global coordinate system so we
get the valley we've got before get the
same value as before for the second
layer for the third layer we get the
same result
so here I've just bought a 1/4 of the
section as opposed to the entire
reception and have me use of symmetry
constraints reduce the model size here
make sure to save your model and this
concludes this example