- [Instructor] At this point in the course
you probably already know to start a sketch,
we need a face or a plane to start drawing on.
Now, what happens if we are trying to create a hole
or something like that at an angle,
and there's not a face or a plane that's available
for us to draw on.
That's when we have to go back into SolidWorks
and create our own plane.
So if I head over here to Features,
I then come up here to Reference Geometry,
and directly below that is this thing called Plane.
Now notice we've got first reference,
second reference and third reference.
Now, depending on how powerful the object you choose
or the face you choose or the plane you choose is,
the less that you actually need.
So if you're choosing a face itself or a plane,
you only need one reference.
So let me give you an example.
Right over here, I'm going to go ahead and choose
something like this plane right here.
So the top plane.
Now notice I'm choosing that top plane
and it automatically assumes
that I want to make a new plane,
that's an offset distance from that.
So I can type in a value here,
like two inches and notice it's going to push it over there,
or I can flip it around to the other side if you wanted to.
So that's just an offset for my existing plane.
Now I can create multiples if I'd like to, pretty handy.
But let's go back to just one right now.
And notice I don't need the second reference
and I don't need the third,
'cause that plane is extending in all directions already.
And so if I'm selecting my top plane,
all I need to know is
how far away from that plane
do I need to make the new plane.
And there we have it.
Now, what if I chose something like a line?
Well, a line, we don't know exactly the angle
of where it is.
So I actually would probably need a line
and another line, or a line and a point to create a plane.
So that's where we need that second reference.
Let's go ahead and click on Reference Geometry
one more time.
Click on Plane.
This time for my first reference,
let's go ahead and choose
something like this line right here.
So it gives me a preview of what it's going to do,
but it doesn't really know where around the circle here,
or where it's going to rotate around the axis there.
So it doesn't really know where it is.
So if I go ahead and I choose is a second line
like this one here.
Now the plane shows up as blue,
showing that it has enough information
to define where that plane is.
It's going to make a plane between those two lines,
and I don't need the third reference in this example.
Click OK.
Here is my secondary plane.
All right, one more time.
This time, we're going to go up here
and I'm going to choose only a point.
So if I choose a point,
maybe a corner here, click that point there.
I can click another point right here,
which is equivalent of choosing that line or that edge.
But if I want to make another point right here,
now it's going to create a plane through those three points.
So that's how you define that.
And that's when you'd need all three of those references.
But I do want to show you one more plane.
And this one is going to be a plane here,
and I'm going to choose my first reference
as this one right here.
Now obviously we can offset this a value,
but instead of choosing or typing in a value,
I could also choose another plane here, or another face.
So instead of typing in that value,
I want to get rid of that.
I don't want to offset it.
That's not what I'm trying to create here.
So let's just cancel up these out of here.
Let me get rid of this guy,
and get rid of this guy over here.
So this time I'm going to choose a face here,
and I'm going to choose a face here.
And then automatically, because I've chosen two faces,
it creates a plane between the two.
So that's a really handy way,
especially if you don't have a plane
in the middle of your part and you need one,
choose those two outside faces,
and automatically create a plane in the center.
And that'll make things really easy
if you're going to mirror something
from one side of the part to the next.
But anyways,
that is the methods for creating planes
inside of SolidWorks.
Remember that if it is a powerful reference,
like a face or a plane, you only need one.
If you have something like a line or a point, you need two.
And if you're providing a reference
that's only a point you're going to probably need three.