- [Instructor] Now I wanna talk about the revolve tool.
Revolve is just that.
You're taking a sketch, a shape, a section, whatever you
wanna call it, and revolving it around an axis.
So to find revolve, gonna hit the little arrow down under
the Extrude and select Revolve.
So the section, what am I revolving?
I'm gonna pick this sketch.
Now, remember, when I pick my sketch,
I wanna have my selection intent set correctly.
So in this case, I'm just gonna say feature curves
so it's gonna pick the whole sketch.
Next thing I wanna do is specify my vector.
I'm gonna pick my, as you can see, Z axis.
When I pick a vector, it's also going to, in this case,
infer that that is the true axis of rotation.
I can specify a different point to be my axis rotation
as well so it can be an offset point from the vector
so you may have a tooling direction that you have to use
and just simply your point as a reference
for the rotation vector.
Now the way this works, is off of my sketch I have my 0, 360
start and end for my revolve.
So as you can see, if I go in the opposite direction
from the start, it's a negative value.
If I go in the same direction for my start and end,
you'll see it's a positive value.
So I'm going from 16 to 48 in this case.
So in this case, if i just bring back,
you'll see a negative value.
You'll also have various settings here so I can specify
until selected, maybe I want that to come down to this plane
so now it'll come down and go to this plane
and this case, because I am using a plane,
you'll see multiple intersections found.
Intersection closest to the user's selection used.
Okay, so it's telling you that there's a potential for this
to find a intersection here, there's a potential to find
an intersection there, you can come over here
and specify, like I said, value until selected.
If I go back to value, it's gonna allow me to enter
in a value, until selected, just leave it where it's at.
And it's using the nearest intersection
for that value on that plane.
As I scroll down, you'll notice I have several other
options as well.
I have Boolean options.
Booleans are what you can do
with multiple volumes in shared space.
We also have offset options.
If I click on offset, you'll notice I can go into two sided
and what this allows me to do is give a thickness
to that shape so you'll notice once again,
at the start if I go in, it's a negative value.
At the end if I go out, it's a positive value.
If I look under settings,
you'll see I have a body type set to solid.
If I change this to sheet, you'll notice that the offsets
go away and it's not valid for trimming up to a plane.
So I would have to change this and just say value
in order to properly use the sheet.
You'll see the first option, two sided, is not set correctly
so it does not like a two sided because when I'm doing an
offset, I am by nature creating a solid.
When I'm switching it to sheet, basically, a sheet
is a zero thickness entity.
It cannot be a solid.
So you're gonna end up with conflicts like this
in the system so you'd have to go back in,
change things, and say none, go to sheet.
Now you'll see everything works just fine, change my value,
make sure that it's trimming up to the right location.
However you wanna go about doing this.
But, if its set to sheet body,
you cannot have an offset value.
Cause, again, the offset by nature has to create a solid.
So if I select okay now,
I'll just have a zero thickness shape.
If I change this back to solid,
I'll have an actual volume for my revolve.