- [Narrator] Up until now, we've been looking at
modal transient solutions.
Now, we're going to look at a direct transient solution.
The way we're going to approach that is by taking
a non-linear transient analysis option
and switching out the non-linear components of that
so we'd be left with a linear direct transient solution.
So now, we're going to open up a SolidWorks part
and this is plate one begin.
If you don't have version 18 or later
then use the parasolid part as usual.
Now once the part is open
you choose the simulation tab.
We're gonna set up a new study.
We're gonna use advanced simulation.
And we're going to be using non-linear analysis.
We have two options, either static or dynamic
non-linear anlysis.
We're going to choose dynamic non-linear analysis.
And we're going to call this direct transient, check okay.
Now we want to change the default transient settings
so right mouse click, and select properties.
This gives the transient properties.
Now the first thing I want to do is to set
the duration of the analysis to 0.26.
The accompanying video showed I've done that calculation.
Now, we also want to check here
'cause I don't want to save the data for restart.
Now, I override the automatic time step calculation
because we want to put in our own values.
Again, the accompanying video show how we calculated
that time step size.
I'll enter 0.00039.
Now, switch off the large displacement formulation
to make sure we're running a linear transient analysis.
Now, one of the advanced options
I deselect sharing the intermediate results.
And now we close out the form.
And we just doublecheck the settings
right mouse click on details
check the time step and the duration.
Now, right mouse click on the part, tab the material
and we'll use the usual alloy steel.
Now, this will be a thin shell model
so right mouse click to find the shell by the surface.
Pick the top surface here
do it at a thickness of 0.05 inches, and close.
Now, we're going to have a cantilever plate
so go to fixtures, right mouse click, fixed geometry.
Pick the top edge there
and then check okay.
Now, select external loads.
Right mouse click.
We're going to be applying a force.
Force is going to be applied with the vertex just here.
Now the direction we choose, zoom in
and choose that edge to define the vertical direction.
We'll want to change the value of the force
to 100 pounds force.
We're going to apply a curve here
so we edit the curve, and then we start to input our pulse.
So there's the first millisecond, just a lead-in.
Slightly past that, we put the first value of ulity
then we need 10 milliseconds sliding on there
that takes us to 0.0101.
Add the value of one in again
that's the plateau of the peak region.
Now we need second point drop down to the zero line
so just go a little bit past that.
And our final tail out, so we just choose 0.02
and we just put that to zero.
And we can see a little inside picture
we've got a nice pulse there
with gradients in and out
and also lead-out at zero
so there's no problem there with extrapolation.
So the loading actions are complete
we can close out the form.
Now, we right mouse click on mesh.
Create the mesh, and just reduce the mesh density slightly
check okay.
Just center the model, and then we can see
the shown mesh is being created.
And we want to apply the dampings
so right mouse click, edit, define
and because this is direct, we don't have the option
to use modal damping.
We're going to have to use Rayleigh damping.
Now, Rayleigh damping is quite tricky
and it's very easy to get it wrong
so if you don't have these coefficients.
So, in the accompanying videos
I explained that in some detail.
In summary, what we do is to pick two strong loads
and equivalence these to 2% modal damping.
Now, we use the mask participation tables
to decide which of the strong modes
and in this particular case, it's mode one bending
and mode two torsion.
So the coefficients for our parameters
have been calculated previously
and we're entering them here.
And so we finish, and just check okay.
And with things set up, and we're ready to run the analysis.
Now, we immediately get a warning that the impulse curve
stops before the final time steps.
In other words, it's shorter than the duration.
But that's okay, because we were careful
to have it flatline at zero in the extrapolation
of that impulse curve.
So, we just click okay, and then the analysis will continue.
Now, I fast forwarded through this solution
so we could get to the results quickly, as usual.
Right mouse click on displacement plot
select animation
and I've increased the frame rate by a factor of 5
as previously.
And now, we can see the transient animation.
It's being dominated by the bending mode
and the torsional mode.
We can also see the influence of damping
so it's starting now, hunch displacements
which damp out as we run towards the end of the analysis.
So we shut down the animation
now we want to set up a time history graph.
So we go to define history plot.
We're going to choose the node that we want
which is going to be the corner node, the vertex here.
Our x-axis is time, and our y-axis we want it to be
the translational acceleration.
We have to be careful to put this in units
of inches per second squared.
Everything is complete, just check okay.
And now, we can see the transient acceleration response.
Now, it's labeled as nonlinear
in fact, we've set this to be a linear direct analysis.
All the modes within the time step accuracy
are included in the calculation.
Now, consider the response under the impulse.
And we can see the early high frequency content.
Now this gets damped out to show the low auto modes
towards the end of the analysis.
And now we save the file off
and we're going to save the file
as plate_2a_dt_end.
And we want to copy the result files, so we just click yes.