MSC Nastran; Patran Tutorial - Total Response of an Undamped System Video Lecture | Nastran: Basic Tutorial for Students - Design Softwares

in this example I'll find the response
of an undamped system I am asked to plot
the response of a spring mass system
linear harmonic force for the following
data the mass is 5 kilograms the spring
constant is 2,000 Newton's per meter the
force is defined as a function of 100
multiplied by cosine 30 T in Newtons the
initial displacement is point 1 meters
and my initial velocity is point one
meters per second
and I'll go ahead and start patrin one
file you'll need is the load CSV file
and up you'll find a link to this PDF
and the CSV file in the video
description below
the load the CSV file is a
representation of the various forces at
various times now once I have Patran
open or starting your patrin database
call it example 311 I hit OK here now
I'll first define two nodes I'm at the
origin
another one at a 1 0 0 now if I turn on
my label control and see the node
numbers have nodes 1 and 2 here
next I want to define an element so
under element edit go to bar Connect
node 1 and node 2
so you see node 1 was dropped here in no
two goes node 1 here and once your
cursor is in the next node box selected
in the bar elements automatically
created and one last thing we have to
make a point element for our point mass
so element at
shape should be point select this node
so you see a triangle indicating the
point element so now let's define our
spring constant so I'm near the
properties tab go to windy properties
and click spring give it a name of K for
input properties we are told as a
stiffness of 2,000 Newtons per meter our
degree of freedom will be UX so it can
move left and right make sure you have
UX for both of these hit OK or for
application region select beam here I
select this element lmm 1 added to the
application region select ok and hit
apply next we want to add a mass value
to this point element so under 0 D
properties click mass call it a M upper
options select lump and under input
properties give it a mass of five
kilograms as stated in the problem hit
OK and for your application region
select this element first select point
elements here then select element 2
added to the application region hit OK
and hit apply you see here we've created
this property now let me turn on the
model train you can see what we've done
so far we've created a mass and we've
defined a spring constant max is to
define our load and boundary conditions
so here in the load bc's tab click on
nodal displacement constraint call this
self fixed grandpa data just to make
things simple let's restrain the 1 2 & 3
direction and rotation is about the 1 2
& 3 directions the 1 2 & 3 are the x y&z
directions
click OK and for application region
select point here select this left or
we're actually working with the FEM not
the geometry so select
here hit nodes at node one okay and
apply now we need to create a
time-dependent load case so here the
load BC stab create load case call it
time LC for type select time-dependent
and hit apply for force or before that I
have to import my force data so under l
bc fields select non-spatial here called
it a harmonic force a domain is time go
to input data import export CSV file but
we need to make a quick option change we
want to ignore the first line of the CSV
file so navigate to where the load CSV
file is and hit OK and hit apply or hit
enter to make the field on the left
you'll notice that the harmonic force
field is here if I now go to a nodal
create force type in F and click input
data I can select and provide a value of
1 in the X 0 in the y and z in the box
next to it I need to provide the field I
just created harmonic force hit OK from
application region I select this node
add it ok and apply so currently we're
working in the time LC load case I need
to make a quick modification to it so
far we only have a force in this load
case I need to include the displacement
fix that we created a while ago I simply
click it's added here once it's there I
had applied to update the load case and
now all the conditions are in that one
load case the problem statement tells us
there's an initial condition for
displacement and velocities all do that
now
here under initial conditions I can
select displacement so initial
displacement my input data will be 0.1
and X 0 on the y&z head okay your
application region will be this point no
- so added ok and apply in addition to
this we have an initial velocity so
scroll up and for object change it to
initial velocity here we'll call it
initial velocity and our input data
would be almost the same point 1 0 0
head ok your application region select
this node added ok and apply turn the
markers off and on so so far this is
what we have we've defined
a full constraint here on the left we've
defined our harmonic force on the right
where the point mass is located we have
an initial displacement of point 1
meters and we have an initial velocity
of point one meters per second
all this defined I can move on to my
analysis click analyze entire model
under solution type select transient
response and your formulation should be
the direct method click OK under sub
cases select time LC and make sure the
names here under sub case name for
output requests or first let me modify
the sub case parameters for defined time
steps i want 200 time steps
space the point 0 1 seconds apart as so
in the end i'll have a time history of 2
seconds
make sure it's s 200 and approximately
point 0 1 here hit ok ok here under
output request i don't want to know my
SPC forces I do want to know my
velocities and accelerations just in
case you want to look at these ahead
apply to confirm the modification I'll
click cancel under sub key select I
don't want to run the nearly empty sub
case called default I want to run the
time LC sub case with all the boundary
conditions click cocaine had applied to
analyze this once that's done go to
access results and click X DB hit apply
to import the results here under results
click graph click this icon to reveal
all the results highlight all of them
and here we'll review the displacements
in the X Direction first for node 2
and I let apply so here's the response
and let me clean up the number so
they're easier to read as I hit apply
again I see that the response goes from
zero seconds to two seconds and my
response goes from negative point
16-inches to point 6 or negative point
16 meters to 0.6 teen meters and I
compare this to what we should get this
is essentially what we do yet if you
want to view the velocities or
accelerations you would simply go back
here selects a translational velocities
once you make that switch hit apply
you'll notice that you can really not
tell there would be a point 1 initial
velocity here and 4 accelerations we can
also view that here make sure to save
and that concludes this example