- In this chapter,
we're going to be learning about drawing dimensions.
We'll cover the baseline dimensions, chain dimensions,
ordinate dimensions, plus so much more.
Let's go ahead and dive in.
General dimensions can be added
to your part or your drawing view inside of
SolidWorks, pretty straightforward and easily,
by clicking on the annotation toolbar
and coming over here to smart dimension.
Now directly below smart dimension here are a
whole bunch of other ways we can add dimensions.
But smart dimension generally picks
the best dimension possible, instead of having
to choose individual, like horizontal or vertical
dimensions and so on, the smart dimension
will do most of that for us.
So go ahead and choose that one there.
Now we have to choose which face of our part
is our datum, which one is going to
start all of our dimensions.
So in this case here, I could choose either
this face here, or this one over here.
Now this one over here makes more sense to me,
so I'm going to start there, and I'm going to start
dimensioning to certain things.
So if I choose like, this first hole,
I've got a dimension between the two.
So click the face you want to start from
and then choose the face you want to end to.
If you want to dimension to these holes,
before we go any further, I'm going to escape
out of that tool, I'm going to come over here
to center mark, and let's go ahead and add
a couple center marks in here.
I prefer to not use the default, and get rid
of those extension lines, and then just click
on a couple of these other holes.
Same thing with the, these arcs right here
I can choose and make a center mark down there.
Same thing with these guys here. Let's go
ahead and just add some center marks as we go.
All right. Once we got the center marks in there
we can continue adding more dimensions.
Now I always want to start from this face, right?
Some people will try to go and add a dimension
like from here to here.
Can you do that?
Yes, but it's not a good practice, right?
Because you're now pulling a dimension
from a different side of the part.
You're not using the main datum target.
So you have to have a pretty reason why you
would do this a better way to do it would be
delete that and then dimension directly
from this face over here.
Okay. So what we call this dimensioning scheme
is a baseline dimensioning scheme.
You keep coming from the same baseline
and adding more and more dimensions across your
part, and they start stacking up
like you might see right here.
And again, jump back over in that, in that tool
always go back to that same exact baseline.
Another way though, you could dimension things
is what we call chain dimensioning.
So instead of dimensioning like that
I can delete these guys here.
I could say, well, this one is 1.25.
And then from that hole to the next hole
I can add a dimension there.
And then from that hole to the next hole
I can add a dimension there.
The problem with this style of dimensioning though
is if there's a tolerance here.
So if this is a plus or minus five thousandths
tolerance for this first hole, and then
this is also a five thousandths
that that hole actually can be 10 thousandths,
plus or minus 10 thousandths from this baseline.
And down here, we get another stack of
five thousandths plus or minus five thousandths.
And so this hole can be plus or minus
15 thousandths from this face over here.
Whereas if you added a dimension that was
from this face here over to this hole here
then that one is constrained
to plus or minus five thousandths from this edge.
So that's important to understand the difference
between chain dimensioning and baseline dimensioning.
Now, another thing we could do is a
combination of the two. So let's go ahead
and delete both of these.
And in this case here, I'm going to delete these
and I'm going to say, Hey, these first holes are 0.3
from the edge, and where they start.
it's probably not that critical.
So instead of a three place decimal
I can switch over here to maybe like a two place decimal.
Oh, there it is two places.
So I can loosen that up a little bit more, right?
So it's a little bit easier to hit that dimension.
Then from there, I can say, hey, from there
I want to make a dimension to the next hole.
And then from there I might want to make
a dimension to the next hole from there.
So everything's based upon that first set of holes.
And now we're creating baseline dimensions
from that first set of holes, right?
And it really depends on your design.
What's important. In this case here
maybe it's the hole to hole dimensions that are
more important than from this edge.
So in that case here, you could say, well, you know
that's really not that important here, so I'd rather
prefer to dimension from this hole to that hole.
That's my critical dimension stack right there,
five inches.
And this one here doesn't make any sense.
Let's get rid of that one.
And that one is more important between this hole
and that hole, and that is using the baseline dimensioning
from this hole here.
So again, just look at your design as a whole
and figure out where, and the best way
to add in those dimensions.
All right, let's do a few more right over here.
If I want to make an angle, choose this face here
choose this face over here and
add the dimension that way.
Now, if we want to add some additional dimensions
we might need a couple extra views.
Let's go ahead and add a couple views here.
Projected view.
I'm going to project right up here to the top
and then maybe one over here to the side.
Okay. Now when I'm adding more dimensions here,
I don't want to choose a different datum
surface, right? I want to use that same edge,
which is this one here.
I want to use that same edge right up here at the top.
Right? So when I dimension from here to here,
I always want to choose that same surface, right?
Same thing, if you're looking at the
view on this other side here, we want to make
sure we're choosing the same datum target.
So up here, if I'm dimensioning from here to the
hole, what I'm using is that front face.
So over here, I would want to dimension everything
from the same front face here
to something else on the drawing.
I only have that same hole
so I can't really do anything there,
but you always want to use that same face
in any different views you're using.
We have the option of adding a hole callout
and right up here is the hole callout
and right over here, I can choose a hole.
And if I click on that hole, it automatically
gives me all this information as far as the size
of the drill bit, and how deep I want to drill,
and what type of tapped hole, and the countersink
that I'm adding in there, and the degrees.
All that information, all with one click,
is pretty handy. So that's how you add your
basic dimensions to a drawing inside of Solidworks.
There's a bunch of tools up here
and we're going to be covering a lot
of 'em as we go through the course,
but that's your basic dimension scheme that you
might use when you're starting
out with your first few drawings.