- In this chapter, we're going to be learning the sketch tools
inside of SolidWorks.
We're going to be focusing on the Line tool,
the Center Line tool, the Rectangle tool, Polygon tool,
splines, creating text, plus so much more.
Let's go ahead and get started.
In this chapter, we're going to be learning
about the Sketch tools,
and specifically, we're going to be learning
about the Line and Center Line commands in this video.
Now I'm going to start a sketch right here on the front plane,
and let's go ahead and jump up here
and grab that Line command.
Notice it is a little l, you can hit l on the keyboard
to turn on the Line command, as well.
And in that little twirl down
or that will drop down next to it,
notice we also have a center line
as well as a midpoint line,
so a couple different lines we can create.
But let's go ahead and just choose
that very first line command.
Now we've covered this a little bit already
through the course,
but let me go over a few more things
as far as creating lines.
So there's two methods.
One is the click method,
so you click where you want to start,
and then click again where you want to stop.
Now that leaves the command active, right?
So now that line is still connected to my cursor,
and anywhere I click, it's going to make another line, right?
And you might not want to continue making lines.
So you might have to hit Escape,
actually do have to hit Escape to get out of that command,
and now you're back to where you were.
Now, if you want to get back into the command,
you can hit l on your keyboard again,
or come up here and grab it.
And the second way we can create lines
is just click and drag, right?
So I can click and drag.
And when you let go, it just creates that one line.
So a couple different ways you can create lines,
and just keep that in mind.
Okay, once you've created a line, though,
we have the ability to switch that line.
So click on this line here, come over here,
and you can start adding some relationships.
So I can say I would like that to be a horizontal line
or a vertical line, or I can fix it.
If I want to switch it over to construction,
a construction line is exactly the same thing
in SolidWorks as a center line.
So here's a center line.
Right below, it's a construction line.
Even though they slightly look different,
they're pretty much used identically.
They are just there to help us to do things.
We can rotate around them.
We can use 'em for construction geometry.
We can use them for all kinds of different things,
and can easily switch back and forth between them.
Notice it says for construction,
you can turn it right back to a regular line just as easily.
So that's the Line versus Center Line command.
Same thing up here.
If I chose the regular Center Line command,
draw something out here.
If I want to make it a regular line,
I can actually click on this little
Construction Geometry button
right here on the heads-up toolbar,
and it turned back over to a regular line.
That's also available over here.
OK, now adding relationships, right?
I can add relationships by snapping to the origin,
and it'll automatically add that relationship.
I can add a relationship from one line to the next
by holding down Control, select those two lines,
and say, hey, I'd like these guys to be perpendicular.
But the main thing when you're designing
inside of SolidWorks, making and using lines,
we want to use those construction lines
to help us to define the shape
without adding a whole bunch of extra dimensions.
So let me show you how to do that.
Let's go ahead and window over all this stuff
and and hit Delete on our keyboard.
Let's draw out a couple lines.
So I'm going to draw a line here, a line over here,
a line here, and then close the shape there, okay?
Now, if I want to tie this into the origin, right,
I could add a bunch of dimensions and things like that.
But a better way would be to add a couple
of construction lines.
So come up here to center line, grab that here.
Let's go from one side to the other,
and then I'm going to go from the top to bottom, okay?
Now I could say, hey, this line here,
hold down Control on your keyboards,
select that line right there,
and say, let's make these guys perpendicular.
Right now, we define that shape a little better.
You can add a point.
So here's a point,
and I'm going to kind of go down through this part here,
and I'm going to find where the center point is.
So if I kind of hover over that line,
notice the center line or center point shows up.
I click on that, and I just added a point there.
So if I say that point there,
and I hold down Control on my keyboard,
I could say that point and that line,
let's go ahead and make those guys midpoint.
And notice, now, we have a nice uniform diamond.
Let's go ahead and grab that same point
and hold down Control on our keyboard
and go ahead and make these two points come together.
So coincident brings those two points together,
and now we define it.
So now I can grab one of these points,
and notice it automatically adjusts this way,
or I can grab this point here, and adjust that way.
I can grab this line here,
make the entire thing bigger and smaller.
So that's how you can use the Line
and Center Line commands, as well as some relationships
to define your drawing or your shape
very easily inside of SolidWorks.
And notice there's really no dimensions here, right?
And if I did want to dimension this,
I'd only need to add a couple dimensions
for something like the length of this line here
to define the height and the width right over here of five,
and now that is a fully defined sketch
tied into the origin and looking good.