MSC Nastran; Patran Tutorial - Linear Static Analysis of a 3D Solid Video

[Music]
in this video I will perform a linear
static analysis on a 3d solid using
cylindrical coordinates full details of
this exercise are on page three sixty
four of the link PDF in the video
description below
first thing I'll go ahead and do is
create a directory on my desktop called
problem 7
I will then start patrin the units for
this exercise or pounds inches and PSI
I'll create a new patch on database and
save it to the directory and made a
moment ago I will click OK on the form
on the right under geometry I will
define my cylindrical coordinate system
using three points so on your type
select cylindrical my origin will be at
0 0 0 my points on axis 3 will be 0 and
the X 1 and the y NZ on the z and my
point on the 1/3 plane is 1 in the X 0
on the Y and 0 and the Z I click apply
and I've seen my cylindrical coordinate
system here next I will create four
surfaces to define the model so under
surfaces select XYZ method here I will
define the vector that will define the
width height and depth of the surface so
the first surface will go 0.75 inches in
the X 0.5 inches in the Y and 0 inches
and the Z the vector will begin at 0 in
the X 5 and the Y is 0 in the Z and then
I click apply
my next surface will go three point two
five point five and zero and the point
at which it will start is this point and
click apply
my next vector is 2 and the X 0.5 and
the y 0 and the Z and I'm using commas
between the values I'll turn on auto
execute so that when I click this point
it automatically click creates a surface
the next vector is 2 negative 5 and 0
and the point from which this vector
starts is this let me go back to the
Home tab and click X or the front view I
will then go to the meshing tab and
define my mesh seeds I will create a
uniform mesh seed consisting the fort or
one element for these two curves two
elements for these curves
and four elements for these curves I
will then select one way by us so that I
can define an l1 0.32 and an l2 of 0.6
for from the diagram you see depending
on which way that arrow is pointing l1
will be at the beginning and l2 will be
at the end so if i zoom in notice the
arrow is pointing this way for both
these curves so when I select them both
l1 is here and l2 is here for these
vertical curves my l1 is 0.25 my l2 is
0.63 from my curve list I select these
two curves now I can go to my measures
and select the curve measure of a
surface measure I can select all four
surfaces Evan clicking apply it's always
a good idea after done you're done
meshing to run any quillin's
next thing I want to do is make these
two dimensional elements three
dimensional elements so under FEM
actions click sweep under F EA
parameters I will leave this here for
now your mesh control when I rotate
these elements about the the y axis here
I wish to create ten partitions so type
int n here using the this coordinate
frame and about the y axis so here under
axis select according to system
direction to and select this so this
will rotate about this Y axis over to
select coordinate one it will rotate
about this z axis but I want to rotate
about this coordinate system my sweep
angle is 90 degrees once I do sweep
these elements I want to delete these
two dimensional elements so check this
or base entity list select quad select
all and click apply
now you'll notice that the two
dimensional elements are not here
anymore
the initial elements were swept 90
degrees about this y-axis and you can
see there are ten one two and so on
before going on I want to modify the
nodes so the action is modify object is
node and method is that in select your
check analysis and reference coordinate
frame analysis coordinate frame will use
the cylindrical coordinates while my
reference coordinate frame use
coordinate zero so the analysis will use
cylindrical coordinates while my
reference coordinate frame will use
coordinate zero so the nodes will be
defined using this global coordinate
system here I simply select all the
nodes click apply the modification has
been performed let me clean this now I
can define my material under properties
I click isotropic cause material matte
under input properties my Youngs modulus
is 10 e 6 psi and my Poisson ratio is
0.33 click OK and click apply to define
the material just as the know if I go to
home and turn on the model tree and go
back to properties I can see so far I've
defined the material and the model
now I must apply this material to the
solid so here under 3d properties click
solid call this solid underscore prop
under input properties I wish to apply
this material click OK
to all of these elements so here I will
click solid element and select all click
Add click OK and apply so now I'm just
assigning the material to the entire
finite elements we have here after this
I will go to a load B C's tab and define
my various constraints so click
displacement constraint I will create
one called radio symmetry for input data
I will restrain this from translating
radially so here 0 comma blank comma
close my analysis coordinate frame here
make sure to select chord 1 and for the
application region select FEM here and
select the 3 nodes here click Add ok and
apply now let me type these markers I
will create a new constraint called
axial symmetry from PI data I wish to
restrain it obviously restrain it in the
axial direction so leave the one place
blank comma leave the to place blank and
put 0 for the third direction which is
the axial direction make sure at
analysis coordinate frame is 1 click OK
select application region reorient this
select the bottom nodes make sure this
is select the two FEM after we selected
the bottom notes click Add ok and apply
uncheck this create a new constraint
called poop symmetry under input data we
will restrain it 9 the 1 and the 2 we
will and not in the 3 so there's a blank
entry here followed by a comma 0 comma
then blank
now this corner frame is 1 again click
OK select application region now to
choose these notes properly you would do
this
so here I've clicked under orientation
the front view so I simply drag a box
very slightly beyond the side of the
model you'll notice that it's selected
just the nodes on the side and be
careful when you do this because
sometimes you may selects identity
select these nodes here click Add ok and
apply or before that I forgot to select
the other side
[Music]
so here I've selected these so far
now let me reorient this to the top view
so now when I hover and drag a window
just slightly above the edge or the side
it just selected these nodes on this
side click Add kay and apply so I'm done
with that now can defy my pressure so
under the loads B C's tab under pressure
call this pressure since my elements are
3d I can give this ask 3d under info
data assign a pressure of 1000 psi click
OK select application region and let me
orient this so it's easier to select
okay now
so I've made sure I can see the backside
of the model now here are your visible
entities only I turn that on I get this
message read it carefully before
continuing I simply drag a box over
these elements and if you rotate this at
the incorrect view summary rotate this
the other way now when I select these
elements you'll notice that only the
ones that were immediately visible were
selected so let me go ahead and add
these here let me view this from the top
now let me do the same thing add it
you'll see that it's only select the
ones that are immediately visible so if
I were to go here and drag a window over
here it would actually select these
other ones since they were immediately
visible so nothing behind it is chosen
so you can see that nothing in the
middle was chosen whereas if I turn this
off it would actively select elements
inside of the model so make sure this is
off
click OK and select apply
now let me clean this up and turn off
the model tree now I can go to my
analysis tab and analyze my entire model
so I'll simply click apply here after
the analysis is done I can access my X
DB results by clicking this icon
I'm clicking apply here once the results
are in I can view a fringe and I wish to
review my displacements that are
translational my quantities that are X
before that after transform my results
to cylindrical coordinate system so here
under plot options I click Cid
and select this coordinate system and
now I click apply so here the highest
value obtained is point zero zero three
inches radially and point and negative
point zero zero zero four four eight and
I compare this to the results
we have obtained that now next would be
to review the axial displacement results
so here what I would do is go back to
select results here for quantity I would
change this the Z component and hit
apply now you can see my lowest zero and
my highest is negative point zero zero
four or negative point zero four and
that is what we've obtained here not for
the stresses so the radial stress here
we have a maximum value of thirty
thousand a minimum value of negative
30,000 psi the same is nearly true for
the hoop stress so back in patran I
switched the fringe result to stress
tensor quantity to the X component and
since that transformation is already
there I don't have to worry about that
so for the radial stress the highest is
thirty thousand the lowest is negative
thirty eight thousand psi for the hoop
stress it should be the same and for the
actual stress I get a
3000 psi and negative 13 psi and if you
look at the results we're actually down
a little or we're actually off a little
so here they at 2300 and 16,000 where's
we got 3,200 and approximately 1400 now
I'll go ahead and clean this up just to
show you the deformation here I click
deformation select displacement
translational click resultant and click
apply you will see this may not be as
clean as you would like it to be so here
under display attributes where you can
do is not show the under form shape by
checking show under form clicking apply
now you'll notice that the green
original surfaces we created are still
visible so I can go to the Home tab and
click erase geometry this will just hide
the geometry it won't actually erase it
click refresh or recycle affix click
apply here
now if you wish to show how this is
displayed you can go to render style and
switch this to shaded click apply you
can switch between the various other
options too so depending on how you like
it you can definitely do that here for
label style I can switch it to fixed and
maybe put seven significant figures
click apply you notice this number
change now if I want to show the fringe
click French here say I want to stresses
the radial stresses click apply now the
fringe is superimposed on the
deformation plot we made a moment ago
and here I can do the same thing where
the label style can be changed
here I put 11 significant figures but
you can change it to something lower
make sure to save your work and this
concludes this example