- [Instructor] When dimensioning holes
on a SOLIDWORKS drawing, we've got a couple
of great tools we can work with.
The first one is the Hole Callout
and it's right up here, click on that
and then come down to any hole you'd like to define
and click on the outside of it
and notice right here we get the size of the drill,
we've got the distance that we're going to be
counter boring it and we've got all this
other information here that goes in here.
So I've got a through-hole that's 180,
I've got another hole that is 300 wide.
This only going to 0.350.
And sometimes this is a little bit confusing.
I'm like, I'm not exactly sure what's happening here right?
So,
when you get to something that you're not entirely sure of
it's a good idea to kind of slice that hole
in half and see what going on there.
So a quick way to do that is to add another drawing view.
So right over here, click on this view here
go up to drawings, go to projected view.
Let's go ahead and project one up here
and I'm going to switch over on this view though
to instead of a wire frame, hidden lines, remove style
I'll switch over here to the full wire frame
and notice what happens as soon as I do that
I can see into my part, like an x-ray view.
I can see I've got this hole up here
and I've got this hole actually, this going
down and connecting with all these other holes here.
And if you didn't look at this in the wireframe view,
you would never notice that.
I mean, you might just think there's a tapped hole here
but you didn't know
that it intersected all these other holes.
And now we do.
So how do we illustrate that on the drawing?
And I'm going to show you how.
So well, let's go back over here to the hidden lines removed
and a good way to do that might be to do a section view.
So if I grab the section view tool I can come over here
and section this part right at the center of
where that hole is and then click on the green check mark
and bring that little section view right over here
to the side.
So now you can see what happens is that we're
actually taking this view here
and we're looking inside and seeing what's going on.
So that looks pretty good.
And now what I can do is I can come over here
and also let's take a look at our projection
make sure that we've got the correct projection on here.
So,
properties threading over projection.
So that doesn't make sense.
Thing looks correct there.
So now what i can do is I can come over here
and start adding some dimensions, right?
So I can say, Hey this dimension here is 0.3
And the depth from here to the top
is going to be that 0.35
So that's same thing we saw down here.
So it makes more sense now what I'm looking at.
And then my through hole is this dimension right over here
which that 180.
And we might want to define a few other things
like the angle here.
That's 120 degrees which is a strange size for a drill.
Most of time you'd see 118 degrees.
So you might want to go back and look at your SOLIDWORKS part
and see why you're seeing 120 degrees here
which is a strange size.
And if it is the size you're trying to use is fine.
But if it's not, you might want to correct that over here.
Let's see what size that is it can be 90 degrees.
So, we're getting some of this data here.
We want to arrange it on our drawing so it looks logical
and you can see things very clearly, same thing over here.
Let's move that over here so it's a little bit cleaner.
And then the 300, we can even pull off to the side.
All right, so now we don't have anything overlapping.
We've defined what this hole is,
how it looks with this data here.
And if you have something that you want to call out twice
like this case here we're showing it as a call out
and over here we're actually showing the dimensions.
I can actually click on this one here and say
I'd like to make this as a add parenthesis
which means that's a reference.
We're just referencing it here
but I'm actually defining the holes right over here.
So that's a good way to define
any kind of holes that are complex on your drawing
either using the whole call out
or actually dimensioning them by using a section view
and taking a look inside of the part.