- [Instructor] The extrude feature
is one of the main workhorses
in the arsenal of SolidWorks tools.
Let me show you how to make it work.
First thing I need to do is create a sketch
within an enclosed boundary.
So let's go up to Sketch.
Let's go ahead and choose the top plane
and let's go ahead and just create a basic circle.
So grab a circle, come down here
and click right there in the center on the origin,
drag out circle.
Of course we want to make that fully defined
'cause it's blue right now.
So I want to go ahead and add a smart dimension.
Click over here, add a dimension.
Let me type in three inches.
And there it is.
Now that's all we need to create an extrude, right?
Start with a sketch with an enclosed boundary.
Now head over here to Features,
come up here to Extruded Boss or Base
and notice my model spins around.
So I'm looking at an asymmetric view.
Now I have this little arrow here.
I can drag this arrow up and notice if I drag it,
it gets a little in-context ruler.
So I got to good idea of how far I'm dragging it
or you can come over here and just type in a value.
So I'm going to type in 3.0
and there you can see in the window.
So I'm just going to scroll in and out using that mouse, wheel,
so I can see what I'm creating here.
Now, this is the most basic extrude.
I'm just doing a blind extrude, but inside this box here,
this dropdown, I've got a whole bunch of other options.
So I have up to vertex up to surface,
off from surface, up to body or mid-plane.
Well, the problem is,
is I don't have any other vertexes surfaces
or bodies to extrude up to.
So when I'm first starting out,
I pretty much only have the option of blind or mid-plane.
So mid-plane down here will give it.
So it's going in both directions, right,
up and down three inches.
So it's inch and a half up and inch and a half down.
I have the ability to add draft though
which is kind of cool.
So I can draft to this feature by adding an angle here
and I can draft it outwards if I wanted to.
So a couple options there.
And if you want to go back to just blind,
it's going to go in one direction.
And same thing over here is
where do I want to start this from?
So most of the time you're going to be probably starting
from the sketch plane, where to draw that sketch
and then we're going to take that sketch and extrude it out.
But you have a few other options in here as well, right?
So I can start from a different surface or plane or face.
I can start from a vertex or I can just offset it.
So if I offset it, I can just type in a value here
or just click on these up and down arrows.
And I can just offset from where I drew it.
So you have a few different options there.
Again to use the other ones besides offset,
you have to have either another vertex
or a face or plane or surface to start from.
So we don't have any of those things yet, but we will soon.
So let's go back to just where the sketch plane was.
And let's go ahead and turn off the draft.
Right now, we just have a simple little cylinder.
Click on OK, and there we have it.
Now, what if we wanted to create something else, right?
Another feature, another extrude.
So of course we can come back to the fundamental planes,
the front plane, the top plane, the right plane.
Those are all great.
Or I can choose a face.
So you have to choose a flat face though.
Since you can't choose this outside surface here,
that's not going to work.
It's got to always got to be flat.
So in this case,
I'm going to use another one of the original planes.
So I have the front plane here.
I'm going to go ahead and create another sketch.
This time I'm going to choose
what we call a center point rectangle,
and we're going to be learning about all these tools
as we go through the course.
But for right now,
we're learning just about that extrude feature.
I'm going to hit this spacebar
which is going to bring up the view cube here
and I want to just click directly on that front face.
Now notice if I go right over here, the center,
they get this little blue line
that pops up saying that hey, if I start drawing here,
I'm going to have that starting right in the center
which is exactly what I'd like to have,
draw out a rectangle,
and I want to snap that rectangle to this origin.
I want to always tie into the origin if I get a chance.
So instead of using a regular line,
I'm going to use a center line.
And a center line and a construction line
are pretty much universal.
You can switch between the two.
They're pretty much exactly the same thing.
So choose center line, which really is a construction line.
Grab that origin and snap it right here to that point.
And now I have this define as far as where it is
and let's go ahead and add a few dimensions, right?
So from this bottom to here, I could type in a value.
Or if you wanted to even more fancy,
you could grab another center line,
snap from this point here up to the top
and we can add a relationship.
How about this line here?
Hold down Control, grab that line right there,
and let's say, these guys are equal.
That way, no matter how big I build that original cylinder,
this rectangle will always be in the center.
If you want to add a dimension,
I can add a dimension that is a hard dimension here
like two inches, which is pretty cool,
but you also have the ability to add something,
I could dimension from an edge out to another edge.
So the edge of the cylinder,
I could say these are always going to be half of an inch apart.
So if the cylinder were to get bigger,
the rectangle would also get bigger.
So, which is pretty cool way to design things.
So I'm going to do one that way
and I'm going to do another one, just two inches, all right?
Now Features.
Head over here to Extrude Boss/Base.
So this one's starting
from the center of that cylinder, right?
And it's extruding out.
So that's obviously one way we could do it.
And if I liked it, I just click on the green check mark
and there you have it.
None of those things have been merged together.
You have two solids,
they've been merged into one solid body
but if you want to go back and modify that a little further,
you can click on it over here and say edit feature.
So if you didn't want to merge 'em,
you could come down here and say unmerge
or uncheck that box,
click OK, now you have two bodies.
So notice over here, you got the original body here
and you have the secondary body here
'cause they're not merged.
Go back here and edit one more time.
This time, instead of starting
from our original sketch plane,
let's go ahead and offset that.
So I'm going to offset it out
and I'm going to start outside of the cylinder there,
and let's go in the other direction.
So I can switch the direction,
and instead of going blind, let's go like up to surface.
So I want to go up to that surface there.
And so it's only going to extrude up to that same surface.
Or if you want to be even more fancy,
you could go offset from surface.
So I want to say, hey, I'm going to offset this by 0.1.
And now you've created a secondary body
that is a little bit off of that surface.
So a couple different ways you can do that.
So again, the extrude command
is definitely one of the biggest workhorses
in the arsenal of tools we have inside SolidWorks.
We're going to pretty much use it more
than any other feature out there majority of the time.
In this movie,
we've covered most of the basics for using the feature,
and we're going to be using it a lot more
as we go throughout the course.