MSC Nastran; Patran Tutorial - Linear Statics; Plane Strain with 2D Solids Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

in this video I will be performing a
linear static analysis on this plane
strain example full details of this
exercise on page 334 of the PDF linked
in the video description below
offers begin by starting a new patron
session and I'll create a new file and
I'll call it problem for the units for
this exercise are inches pounds in psi
I'll first begin by creating or clicking
ok here and then creating a new
coordinate system by going to
coordinates entry point my type is
cylindrical leave the defaults and click
apply you'll see my new coordinate
system here at the origin I'll create a
curve using the XYZ method or actually
I'll be using the 2d arc angle method
the radius from the origin will be 3
inches I and angle will be 15 degrees my
rotation axis will be the z-axis
recording at 0 with the third axis which
is Z and the center point will be this
crosshair which is 0 0 0 I click apply
my first curve is created my next curve
has a radius of 6 or 9 actually that
angle insert angles are 0 and 15 of the
other values are the same so I hit apply
next I'll create a surface using the
curve method this allows me to select
one curve followed by the next one and
I'll fill in and create a surface I'll
go ahead and translate this actually to
create my other 5 surfaces so here under
transform click surfaces so here you
have transform surface click rotate
here we'll rotate about the z axis here
my rotation angle would be 30 degrees my
repeat count will be 5 and from my
surface list I'll simply select this
surface here you have auto execute
checked this will automatically generate
the surfaces once you select an entity
so here as soon as I click surface one
I'll create the five surfaces if you
accidentally make a mistake you can
click the undo button here now undo the
action here I have surface 1 in here so
I click apply again and I'll go ahead
and create my five surfaces here I can
now move on to create my materials under
the properties tab I'll click and select
isotropic here under material name I'll
call it just material under my info
properties my elastic modulus is 1000
psi and my Poisson ratio is pointer 499
click OK and click apply now we have to
assign the material to these surfaces so
under 2d properties click shell under
property set name type in shell under
input properties select this icon here
and select this material or before doing
that should cancel this and switch my
options or I've actually selected the
wrong 2d properties I just select 2d
solid here make sure it says 2d or
create 2d 2d solid leave the name of
shell your options should be plain
strain under input properties make sure
you select this material select ok under
your application region select surfaces
1 through 4 1 2 3 4 you can simply drag
and click click add ok and apply here
let me rotate this
here I've called this she'll actually be
called something else I'll call my next
one property two for plane strain select
revised formulation for your input
properties
you should have materials selected here
if not selected like you did before
click OK for your application region
select these leftmost surfaces hold the
shift key to select multiple entries
click Add ok and apply so now I can move
on to my boundary conditions tab here
all define a boundary condition here
here for every surface
so click displacement constraint all
simply call this set name constraint
under input data I wish to prevent
translation in the two direction of this
coordinate system which is the hoop
direction so here select this coordinate
systems coordinate system 1 before it
was 0 which in which was foil up this
global system but this time we're
selecting the cylindrical coordinate
system click OK for your application
region you can select curves here what
you can do is simply click hold shift
and go around and select the multiple
curves or what you can do is notice the
side you can click polygons pick here
make sure your cursors in here you can
use this polygon pick and you'll see
it's on in the depressed state so this
allows me to start a click it basically
allows me to move around and create an
enclosure in which then cities will be
covered so then click this last point
and I'll select these surfaces or these
curves here it's selected surface one
curve three surface one curve one
surface two curve three and so on click
Add ok and
apply see it's defined there next I once
I add my pressure so here under element
uniform click pressure it's up in the
new set name is pressure for target
element type type in 2d for your input
data type in 100 click ok and select
application region zoom into the model
here you'll go ahead and just select
these outer edges here so surface six
add your curve to and hold the shift key
so you can click and select other edges
click Add you'll notice they stay pink
indicating they've been selected click
OK and apply and you shoot see arrows
for each edge here now we can go ahead
and move on to my meshing first I'll go
ahead and view this in the XY
orientation or the front view here you
can do two things to hide the boundary
conditions here you can click reset
graphics here or turn on your model tree
and check them on and off another way is
to just select this plot lbc markers but
to turn them off you would have to click
this again and to see the this this icon
here plots the boundary conditions that
are in the current load case I'll hide
the mana tree and now I'll go the
meshing tab to actually mesh those for
my mesh seeds I'll click one-way bias
and I'll use the l1 and l2 method so
here as soon as I'm in the mesh seat I
get a little arrows indicating which
ways the direction for each curve so I
know that looking at this diagram the
arrow points from the l1 to the l2 so I
know that L ones here and L twos here so
for my l1 I want a value of point six
zero seven eight seven inches
my L tube will be 0.243 one three inches
and for auto execute I'll uncheck that
I'll select this first curve and apply
and you'll see the much seat is there so
now I can what I can do like I did
before is use the polygon pick select
these curves here or these edges see
that all entered here and they're all
highlighted orange or pink click apply
now the mesh seat it is there next thing
I want to do is apply a uniform SC to
these inner edges so click uniform I
want three elements I'll turn up auto
execute I'll simply select and hold the
shift key to select all these other
edges so like this this and so on and
hit apply now we see your mesh seeds are
there so now I can go to the surface
measure and this one is a quad for mesh
so we just selected a surface one and
hit apply next one is a quad eight so
let's switch this the quad eight select
the surface surface 2 and hit enter this
next one is a tria element 303 actually
and select the surface surface three and
hit apply the next one is a tree a six
mesh and so like a service for here it
apply an X match is a quad leave quad
for select this mat or the surface
surface five and hit apply
the last one is the tria mash select
surface 6 and hit apply let me close
this form by double clicking the tab now
if I turn on my boundary conditions it
looks like it's just applied to these
points here to get a better view you can
go to the display load B C's element
properties icon or label here here
back on show on FEM only click apply'
and turn on your boundary conditions
again now you can see they are actually
assigned to all the nodes here and this
is a good way of ensuring that you apply
your boundary conditions properly to
turn this off uncheck this and click
apply clean this and turn on the
boundary conditions again you'll see
that it's back to normal click refresh
graphics to hiatus now one last thing I
have to do is modify my nodes right now
they're most likely using this
coordinate system as a reference and
analysis coordinate frame what I have to
use is this cylindrical coordinate
system so I have to go ahead and modify
the nodes to do this go to the meshing
tab go to the top for your action you
would modify your nodes you will
actually edit them so I want to edit the
analysis and reference coordinate system
I want to use this cylindrical
coordinate system called chord one and
use the same cornice someone here for
your node list you want to select all
the nodes so you can drag a window over
them or you can use the shortcut here
called select Paul or pickle and click
apply here the feedback tells me that L
645 notes have been modified now I can
move on to the analysis tab to actually
run this so here click analyze entire
model will do a quick modification to my
sub case here I'll modify at the default
sub case that uses the default load case
and I actually want to output an extra
request so far I have my displacement
stresses and forces being outputted I
want to also output my element strains
just in case you want to review those
results too so ensure you have element
strains here and here selected click
apply can cancel out of here
and now you can hit apply and this will
submit the job to MSC nastran for
analysis once that is done you can
import your xdb results by clicking this
icon and hit apply to view results you
can go to the results tab here but
before we do that to make this a little
cleaner on us I'll create a group for
each mesh here so under the Home tab
turn on the model tree you can do this
two ways you can create a group using
this tool or you can actually just up
click anywhere in the model tree or
right-click and you can create a group
here so for my first group I'll call it
one uncheck this for my entity selection
I'll just select the these the these
elements or these entities here you'll
see it selects a bunch of items click
apply next I'll make a new one called
two are used to polygons pick as this
before and then close all these out
entities here apply and do the same for
each other one
and click apply for the last one so now
you see I've defined of six separate
groups so if I uncheck default group and
here I get a problem telling me that uh
this originally was the current group
and wants me to select the add new
current group so I'll just select Group
one as a current group now what I've
done is I should turn that on make sure
you always have one on and now you can
see that I can turn them off and on so
whenever you wear my results this one
make it a lot easier so I'm going to go
back to results and say I want to view
the fringe say the stress tensor - or
let me review the displacements first
let me view the radial displacements so
X component I can hit apply hide all the
groups except for this one hit apply our
council here hit apply here now you can
see my values here so when I compare
this to the actual value I should be
getting you can see what I get
so here I get up 0.317 I should be
getting a point one or point two two
five zero inches for the outer edge then
the point 4 1 2 or point five two five
for the inner edge so here I get up 0.5
inches and the point 1 6 9 inches and
then I can do that for the next group so
I get similar results and I can do that
all around up every time you switch on
or off another group you get this window
you can click Council or just go back to
the results avier so click apply get the
same values for displacements for the
enter in the outer edge same same thing
here
same thing here
same thing here here we've actually
gotten five point three which is a
pretty close to this now to view my
radial stresses I can do this
go back to the results tab make sure
you're here scroll down select stress
sensor quantities X component or radio
stresses click apply and you can note
the values as you go along so 18100 here
back sit down and close out one 125 here
25 here I'm just to compare what I
should be getting here should be hitting
125 for the inner and 25 for the outer
and that's what I got here here you can
see my results are along those lines you
could do this for every other section
that was my radial stresses not to view
my hoop stresses so here what I would do
is go back to my results tab switch to
the Y component which is your hoop
stress click apply
here you can see your values so for the
outer I would get a point 8 here I will
get 91 here you should be getting 100
psi because of the pressure so we should
be getting 0 for the outer edge and 100
for the inner edge and what you can do
is just turn them off and on and go
around the loop essentially to the to
see your results that is like actually
what we do end up getting go back to the
Home tab refresh this turn off your
monitor if you will like make sure to
save and this ends this video