MSC Nastran; Patran Tutorial - Bending Stresses of a Loaded Beam Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

[Music]
in this example I'll be finding the
normal stresses for this loaded beam you
can find a link to this PDF in the video
description below I'll go ahead and
start a new patron session and I'll
start a new patron database call it
example 618 I'll hit OK on the form on
the right first created line under
geometry go to curves select line by XYZ
method from the origin create a line
that is one meter in the y-direction hit
apply can reorient this as shown next
I'll go to the properties tab to define
my beam cross-section and materials
under tools select beam library here for
your new section name we'll call it
cross section scroll to the right and
select the rectangular section
according to the PDF depth of the beam
is point four meters and the width is
point two so back in that tools beam
library window the with this pointer and
adapter hi it is pouring four meters hit
okay reply at the bottom to create your
section if you go back to tools beam
library you select this cross section
hit calculate display here you get a
diagram of where your cross section
looks like I'll create it or I'll take a
picture of this for future reference
now that I've defined my cross-section I
can define my material click on
isotropic under material name call in
matte for input properties
give it a Young's modulus at 209 and a
Poisson ratio 0.3 hit OK and hit apply
let me reorient this so the Z Direction
is pointing upward and the Y Direction
is pointing this way
so like 1d properties and call this beam
member under input properties for
section name select the cross-section I
made a moment ago and for your material
select the material I'm also made a
moment ago for your barrio orientation
for now type in a value of 0 0 1 this is
a vector going in the Z Direction hit OK
for application region select this curve
at it and hit OK hit apply next go on to
the boundary conditions tab select
displacement constraint and call it
fixed one side of our beam will be fully
fixed or constrained so type in 0 0 0
for translations and rotations hit OK
for application region under pointer
vertex make sure you have this click
select the leftmost point add it ok and
apply next go to nodal force call it
moment and for info data or before then
input data for application region select
the opposite point add it okay for your
Impa data we'll use the values given in
the problem here we have a value of 7.2
kilonewtons acting leftward or you're in
the positive Z Direction here I'll make
the valley go in the positive x so 7.2
III for your next value it is negative 9
points
and that will be acting in the Z
direction so type in 0 for y for Z
Direction type of negative nine point
two III make sure you have this right
I should be points so at a point two
alternatively you can use comments
between the values hit okay and since we
already have something in our
application region we don't have to do
that now hit apply now you can see the
12,000 new in force acting at the tip of
the beam and that is exactly what they
do here this is the moment actually so I
think I just defined a forest not a
moment so if you go back to model tree
and look for the force I just created
right-click and modify move this vector
to the moment section hit ok and hit
apply the two arrows here indicate that
this is the moment and not a force go to
the meshing tab go to curved measures
here so like this curve and hit apply 10
elements have been created you can view
the numbers by going to the Home tab
hitting label control turning on and
turn on the element numbers you can also
turn on the known numbers to view your
cross-section you can go to display load
BC element props scroll and select 3d
full span and hit apply and this will
only work after you've matched your
curve you can go back by selecting 1d
line and hitting apply and now when
reviewing your beam stresses you'll be
given four options you'll be giving your
stress as that point F
Point C Point E and point D and so let
me go ahead and first analyzes so under
analysis go to analyze entire model once
you click that hit apply and I'll hide
all my boundary conditions and prereqs
DB results and hit apply go to your
results tab select this sub case scroll
down and hit bar stresses bending and
hit X component under your position at
Point C you can select the four other
points and those clear response of the
bending stresses as shown in this
diagram so if I view the stresses at
Point C hit clothes hit apply get a
value of negative four point nine five
here now you may be asking yourself
where is Point C let me go back to
display load BC element props and show
you the beam first let me clean this
here I have a projection of my beam
cross-section if I go to utilities
display Emma seen a strong beam tools
here I can view my point C D E and F in
order for this to work first I must go
back to properties and modify of the
beam member property I made a moment ago
switch it to properties and uncheck
associate beam section hit OK scroll
down and hit apply back in that beam
verification tools which again you can
access through utilities display and the
scene a strand beam tools make sure
display is Point C D E and F under
display options uncheck include polygons
for your scale factor make it point 4
and hit OK
under select beam elements select any
element if i zoom in you can see that
it's plotted or drawn points f c/e and d
here and let me do one last thing under
display select axis and select any other
beam let me go back to my results and
here I can see that Point C is in this
location so I'm gonna have you that
result I'm viewing the bending stress at
this top left point if I compare it to
my result Point C here I do get a value
of negative four point nine five as
shown here and in the legend here
switched to point F hit close and apply
that would be this point right here on
the top right I have a value of two
point two five and it matches the value
here point B an Excel view point
and II should get negative two point two
five and four point nine five point D
and E I get two point two five or
negative two point two five next I
should get four point nine five and I
have obtained this value let me clean
this up and go over what this access and
what these points signify back in the
properties section
right click on beam member and modify
here under bar orientation this defines
the y axis of the beam element here I
defined it as 0 and the X is your own
the wines & 1 & the Z if I were to
change this to say 1 in the X and 0 in
the Z I'll hit OK and apply EDIUS for
all or before that let me modify these
input properties so to make this
modification toggle this back to
dimensions once the values are dropped
back in the boxes switch it back to
dimensions or properties uncheck
associate beam hit OK make sure you have
curve 1 here and hit apply now you'll
notice a few things
the cross-section has in re oriented so
when I go back to the beam verification
tools I'll first head all to erase the
ply and now select element 3 or any
other element again you'll notice that
my access has switched before the y-axis
here of the beam which is the green
arrow was pointing in the Z direction
since I changed the orientation vector
so it points in the X direction
the YB maxes now points in the
x-direction and you can see that when
you zoom in and if I view the point c d
e and f I saw like another element
notice that before C was up here F was
up here a and D were down here since the
cross section has been reoriented Point
C F G and D have also changed when you
go onto your results our results will
also change and that's the very big
importance of the orientation vector you
can click cancel and every box make sure
to save and that's how you find the beam
stresses for beam elements