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

in this video I will perform a linear
static analysis on a rigid frame full
details of this exercise are on page 320
the link PDF in the video description
below and before I go on with this
example we'll create a folder on my
desktop called problem zero one I will
start Patran
okay my new database and save it to the
folder on the desktop I will click OK on
the form on the right now before I begin
an example I want to create my cross
section for the beams so under tools go
to beam library here I will create a new
section called cross section I will
scroll through the menu here and select
a rectangular section my width is 0.5
and my height is 0.5 if I want to view
the area moments of inertia and so on I
can calculate a display here minimize
the window I can view my area moments of
inertia and various other section
properties after you're done hit OK or
apply and make sure here we get the
feedback SS beam section cross section
created now I can go ahead and define my
geometry go to the geometry tab and
create a career using the line by XYZ
method so here what I'll do is define a
vector that makes a curve in this
direction I'll make two curves that go
horizontally in this direction and then
I'll make a curve that goes vertically
down in this direction so from the
origin my first curve will be defined by
a vector going 0 inches in the X 7
inches in the Y and 0 inches in the Z
here I've used spaces between the values
another way of typing it in 0 comma 7
comma 0 hit apply here's my first curve
now my next line will go to inches in
the X comma 0 inches in the Y comma 0
inches in the Z comma close bracket the
original point for this vector will be
this top point so click this one time
notice the curve is created now click
this point and my second curve is
created for my last curve it will go 0
inches symbol Y or the X 7 or negative
10 inches on the y 0 inches in Z on this
top point click it and your last curve
is created to make my materials go to
the properties tab make an isotropic
material call it matte under input
properties the Youngs modulus is 1 East
7 psi and the units for this example or
pounds inches PSI my Poisson ratio is
0.3
click OK and apply now to apply the
cross-section and the material to the
curves I need to make a 1d property that
uses a beam option so once you click
being here you will need to create two
properties one for these two vertical
curves and one for the two horizontal
curves so here call it vertical curves
under input properties click this outer
W section icon select cross-section
under material click this icon and
select the material you made a moment
ago underbar orientation create a vector
that is in the x-direction sub 1 in the
X 0 and the Y and 0 to Z click OK for
your application region just like these
two curves click add ok and apply now
for horizontal curves
under input properties give a change bar
orientation so it goes on the Y so 0 in
the X 1 on the Y and 0 in the Z click OK
select application region select these
two top curves add them ok and apply now
I can define my boundary conditions here
now the problem statement says the
bottom right is fixed and there's a 100
pound load acting downward at this point
so let me go ahead and define
displacement constraint here I'll call
it fix from an input data all fixed
translations in the 1 2 and 3 directions
and rotations about the 1 comma the Y
comma and the Z direction and recall
that I can either add spaces between the
values or I can add commas click OK
select your application region here I
just want to select points so I will
pick the point filter here and you'll
notice that two entities have been
selected here this is 0.5 this is
actually curve for the first point is
here the second point is here so by
saying curve for point two that is the
same as saying the end or the the end of
curve for which is this point so these
two are actually the same so add them ok
and apply now it's add my force I will
click nodal force here call it f under
info data the load x 0 in the X minus
100 the Y and 0 and Z click OK add it so
for your application region you can
select this point and again here is
selected curve 2 point 2 which is this
curve and the second point here you see
clear of three point one three
Oh point 1 and point 3 which is be its
own point so add this ok and apply a
zoom out using holding down the control
key in the middle mouse button let's see
the loading here I can go ahead and mesh
this using the curve master here I can
select all the curves like this or I can
simply use the pick all shortcut here
and apply click yes for all here and now
let me clean this up and let me show you
the node numbers so here under the Home
tab click the icon under the label
control icon here and click nodes so
here you see the numbers for all the
nodes 1 2 3 all the way to 7 here it's
sort of difficult to read the 8 you'll
notice it's 10 here notes 8 & 9 or
overlapping here nodes 11 and 12 are
overlapping and nodes 14 and 15 are
overlapping here in order to fix this
you will go to the meshing tab and you
will click equivalence here click apply
and it removed duplicate nodes so now
you can clearly read the nodes and you
don't have any more overlapping nodes so
once you're done with that go to the
analysis tab analyze the entire model
but before that we will modify the sub
case select the default sub case under
output requests remove the stress and
that SBC forces
and add gridpoint force balance the grip
poit force balance will allow us to
create a Freebody diagram click apply
and counsel now you can hit apply here
and submit the job to nash Jennifer
analysis let me fit the model using the
fit view icon here let me turn off the
node numbers and let me import my
results so I able to click on xdb here
and apply your results I will use the
cursor tool here and I wish to review of
my translational displacement in the X
direction click apply separate form
appears here I can select individual
nodes and view the values to make this
easier to read I can go to the display
attributes and under label style I can
change the color to light the label
format to fix significant figures to
five
click OK and apply so now when I click
the nodes I get easier to read numbers
so here at the bottom left I get a
deflection horizontal direction of 0.1
0-3 I compare this to what I should get
that is what I do get for the vertical
direction I will go back here and select
Y component and the plier select this
bottom note again and I get one point
six seven inches
and that is what I do get and remember
this is negative and let me clean this
and apply again sometimes it may be
difficult to read but there is a
negative there here we get a rotation of
point zero four to about the z-axis
severe switches to rotational
displacements about the Z and apply
select this node and we get point zero
four two just as we should get here
cancel this clean it up fit it if you
would like save the model and this
concludes this example now as a
continuation of the last example I would
like to create a Freebody diagram so
what I can do is under the results tab
click Freebody here I have free body
load selected I click the display
attributes I would like to show the
forces and moments so click for slash
moments when I click apply I get a free
body diagram of the model so here I have
the 100 pounds applied here I had a fix
condition so the vertical support or the
vertical reaction is 100 pounds and my
moment is 200 pounds inch that's how you
display a free body diagram and the
requirement for this is that your output
requests include grid point force
balance as shown earlier in the video
clean it up
save and this ends this exercise