- [Instructor] Now we're going to open up
the Solidworks part, so File Open.
And the part number is plate_1_begin.
If you don't have access to version 2018 or later,
then you're gonna have to use the para solid part.
Now the part opens, and it's just a square plate,
created by a simple sketch and then an extrusion.
We open up the simulation, New Study.
The default is a static analysis.
We want to change this to Advanced Simulation,
and then we're going to choose a linear dynamic analysis.
From the types of linear dynamic analysis,
we're going to choose Modal Time History.
Now we're going to rename the simulation study as
10 millisecond impulse.
Click OK, and the new study is set up.
The first task is to apply the plate material property.
We're just going to use the default alloy steel for that.
We want to create our dynamic analysis properties,
so we go to Properties, right mouse click,
and we're going to choose the number of modes
we're going to use, which is going to be six.
And then we go to the advanced dynamic options
and I want to give a start time and then an end time.
And we've calculated this as .26 second duration,
and the time increment is .00039 seconds,
that's our time step.
You might like to review the earlier video
just to see how these numbers were calculated.
Click OK.
And now we're going to prepare the model
for 2D shell meshing.
So define the top surface as being the definition
of the shell surface, and I'm going to give this
a thickness of .05 inches.
Just check OK.
Now, this is going to be a counter-levered plate,
so go to Fixtures, choose Fixed Geometry,
and pick the appropriate top edge there.
So zooming in slightly, let me get a good view of that.
That's the edge that we want.
Check OK.
And now let's zoom out a little bit.
And now we're going to apply the external loads.
Now, this is quite a complicated setup,
so go to External Loads, and we're going to be applying
a force, we're gonna pick the corner
to apply that force there.
So I'm going to choose a direction,
and I'm going to select, if I zoom in,
and to find the corner of the plate there
and just grab that edge there to define completely
what that direction is going to be.
Now, having got the direction, I confirm it is a force.
I'm gonna put 100 pounds force in.
Let's zoom out for the moment and then focus
on the next aspect of the load application
we're going to be applying, which is the time history.
Now we have a choice of a linear time history,
which really means constant, or a user-defined curve,
which we're now going to choose then edit
to create that curve.
Now we're going to be putting in a 10-millisecond impulse,
and you remember from the previous video
I like to put a slight lead in and a slight slope in
and a slight slope out, and then a tail
at the end of the impulse curve.
So the data, the numbers are in the previous video.
The Y axis represents our force values,
which are gonna be zero and one.
They're gonna be scaled by the 100 pounds.
Now we're dropping impulse back to zero at this point,
and then the next point puts the tail in.
And this is just to make sure that the graph
will be extrapolated along the zero axis.
Now we can see the shape of the impulse
completed in the little preview window at the top there.
Now we can click OK, and then check
the building is complete.
Now we right mouse click on Mesh, create the mesh.
I'm going to set it slightly coarser than the default.
Check OK.
And then we see the triangular shell mesh is being created.
Now we're going to define the damping in the models,
so right mouse click, edit define.
We're using modal damping, and for the six modes,
we're going to use .02, 2% critical dampening.
That's defined, and we just check OK.
Now we can control the way that the output is created,
so we go to Edit, Define, and we're going to choose
output for all solution steps.
I'm not going to clip any of the output,
or filter the output.
I also don't need the stress and reactions.
We can use either absolute or relative,
it doesn't make any difference in our particular case.
Choose absolute, and we just check OK.
Now we're ready to run the analysis,
so we can go to run the study.
We do have an option to run just a normal modes analysis,
in other words, run frequency.
So we're gonna choose that first.
And then in results, we can check the frequencies,
and also the mode shapes.
So I'm setting up my default mode shape plot.
I'm going to be setting so I can see the mesh.
I want to superimpose on the deform shape.
I'm gonna put a transparency of .7.
We'll see what that looks like.
Just remember, you sometimes have to flick between
the model and the study to be able to see
that transparent, undeformed shape.
So we're seeing mode one there very clearly,
the first bending mode, and then we can just
go and edit the definition and move to mode two.
Just click up, and now we look at mode two,
check OK, and it's our first torsional mode.
And we just keep on walking through the other modes.
So mode three, which is our second auto bending mode.
Then we move forward into the definition again,
move to mode four.
And this is transverse bending mode.
Come to mode five.
It's our second ordered torsional mode.
And now we can set up the next mode,
which would be mode six.
Click OK, and it's combined bending
both in longitudinal and lateral senses.
Now, this was just a quick review.
We've already done a thorough modal survey
to check, otherwise we should use our time steps,
durational analysis, and what the strong modes are
we anticipate will come out from this analysis.
So now we'll just switch on the mesh,
just review the mesh there, and now it's time
to run the analysis.
So run the study, this is gonna be
our full transient analysis.
But run through the number of time steps that we've defined.
Now, the moment we assume the mode shape,
so we want to change that and want to define
a displacement plot, which will be relevant
for the time history.
So setting up a default, it's the outer planes,
their direction I'm interested in.
I want to have a discrete set of contours
and I also want to be able to see the mesh.
Then we check OK.
Now at the moment, we'll assume the deflection
at plots capped 667, which is the end of the analysis
of .26 seconds.
So we can change that, give it a right mouse click
and go to Edit Definition.
I can pick any of the time steps which I want to check.
And here I've rolled forward to time step 641,
which is about .25 a second.
I can keep on editing that, so I can go up to
the definition again, again select any of the time steps
I like from here.
So let's go to a much earlier time, time 200.
Click OK.
Now I'm also going to scale the deflection
back a little bit, because at the moment,
I've applied a very large force indeed.
So in fact, I've got deflections which
are probably way too high to be realistic.
So if I knock them back from true scale
back to a scaling factor about .2,
that should be more useful to me,
particularly when I now come to animate.
Now right mouse click and select Animate.
They're gonna sweep through the whole history
of the response here.
Now, this point, I get an error dialog box,,
and what it's telling me is that the amount of memory
I have available on my machine is not sufficient
to animate a full 667 frames, so it's suggesting
I cut back on the frame rate.
So if I put a frame selection rate of 10 in,
it will move through very quickly.
I want to try to get the frame selection rate
as high as I possibly can to get a smoother animation.
I've really got to juggle that with the
actual memory requirements on my computer.
So let's synchronize to the start.
There's an early time response,
which damps out quite quickly, and then we end up
with the final frame.
Now, if the frame rate is too fast to
see what's going on, so in this particular case
I've slowed it right down, and what we're seeing
is two modes dominating.
We're seeing the first bending mode dominating,
and also the torsional mode.
You can kind of sense those two modes working together.
We're going to be doing a time history plot
in a second, you'll be able to see that more clearly,
but that's what's going on there.
And in the previous video, that's what we predicted,
is that those are going to be the two strong modes,
and that's what's actually happening
in this particular case.
So we can't really visually see the dampening occurring,
but it is occurring there.
Again, the time history plot of the XY graph
coming up shortly will confirm that.
So when we're ready, we just stop the animation.
So now we're ready to look at the corner node response
through time.
We can look at acceleration or displacement,
and it'll give us a clear indication
of what's actually happening there.
So we go to define response graph.
We want to pick the corner node,
so if we zoom into that, it'll give us a clearer picture.
And if we select, then we see it's node number 43.
Now we choose the component we want to plot.
In this particular case, it's going to be the Y axis,
it's going to be formed by the Z displacement.
And we want the units to be in inches.
And we want the full range of time history to be plotted,
and then we just click OK.
So here the time history plot appears as an inset,
so we can just open that up.
And showing that corner node, there's evidence there
of two modes interacting.
Now, in the theory videos,
we'll expand on that and explain how
we can identify that a little bit more closely.
But for the moment, we just accept that that's
the time history that we've seen there.
And then we want to repeat the exercise
and look at the acceleration of that corner node,
so again, we're defining a response graph.
We pick the same point again,
which is point 43, but this time we change the Y scale
to be the acceleration.
Again, it's going to be the Z acceleration,
not resultant, and again, we need to be careful
to change that to inches per second squared
in this particular case.
And again, it's the full response we're interested in,
so we just check OK.
And now we get the acceleration time history plot
in the corner, again, we can open that up.
The acceleration time history is interesting,
because we see evidence of much higher-frequency content
under an initial loading, and then as we move
through the signal, that high-frequency content
gets damped out and we're left with the
low-frequency content and the make of the torsion mode
and the bending mode as we continue through
to the end of the signal.
Then we'll pick up on that again in the theory videos.
And now we're ready to close down this example,
so we go to File, Save As, and we'll save this name
as plate_1_end Solidworks part.
And we want to save our results file,
the CWR file, as before.