- [Instructor] In this movie,
we're going to be covering the basic steps
for creating a model inside of SolidWorks.
To get started,
I'm going to cover the six steps of modeling.
The first one is to select a face or a plane.
When you first get started in SolidWorks,
you don't have anything
besides the three fundamental planes
and so you have to choose one of those to get started with.
Number two is starting a brand new sketch
on one of those fundamental planes
or if you work through the model a little bit,
you have some planes or faces you can choose
then go ahead and choose those.
Once we started a new sketch, we want to draw some geometry
and then we want to take that geometry
and we're going to tie that geometry in to the origin
so it knows where it is in space.
We're going to add relationships
and dimensions to that geometry
and then go ahead and create the feature,
whatever it's going to be.
It's going to be an extrude,
if it's going to be a cut, if it's going to be revolve,
we're always going to be pretty much do
the exact same six steps for each one of those features.
Now there's some more advanced features
that might not use these exactly,
but, in general, we're going to go ahead
and follow these six steps for most of our modeling.
Now let's jump back over to SolidWorks
and see how it all works.
All right, so the first step is to select a face or plane.
Now right over here on the left
you can see I've got the front plane,
I got the top plane,
I got the right plane.
I can choose any one of those to get started
and, in fact, if I come up here to sketch,
if I choose sketch,
the first thing it's going to ask me is, hey,
select a plane on which to create a sketch for the entity.
So it's already telling us what exactly it needs.
So I can do it either way.
So let's go ahead and choose something like the top plane.
Now, step two is going to be start the new sketch.
We just did that.
Step three is draw some geometry.
So let's go ahead up to the sketch toolbar.
Let's choose this two point rectangle
and I'm going to choose this lower left hand corner
up to the upper right hand corner and draw out a rectangle.
All right, there it is.
Now I notice we get these little green boxes
that pop up as I draw.
Now, those are relationships.
So these ones over here are saying, it's a vertical line
and over here, it's saying this is a horizontal line.
And you can add and delete relationships
by clicking on them and hitting delete in your keyboard
and you can also add them using the relationship toolbar
which we're going to cover in a second.
We want to tie this geometry into the origin.
So here's our friend, the origin, and here's our geometry.
So let's go ahead and tie those together.
Now I have this point here and I can just grab that point
and just drag it over so it snaps on top of the origin.
Notice what happens is, when I do that,
it does add this little relationship,
which is a coincident relationship and now this line
and that line over there are black.
The other ones are blue and when a line is blue,
it means it's undefined or under defined.
So it knows something, but it doesn't know everything.
Whereas black knows it's fully defined.
Now, let's go ahead and see if we can get all these lines
to turn up black.
So to define these a little further,
let's go ahead and add a dimension.
So come up here to Smart Dimension
and I'm going to make a dimension
from this side over to that side
and I'm going to place the dimension right here.
Type in six
and then same thing over here.
I'm going to say this dimension here,
this one dimension over here, and type in three.
Now, as soon as I add those two dimensions,
notice this line and that line both turn black
'cause now they're fully defined.
They know exactly how long they are,
they their relationship to the origin, and so on,
so everything is good.
Now there's a couple other colors
for lines that we generally don't want to see.
Those are yellow and those are red
and those means we got issues.
So let's go see how we can create some issues
and then see how we can resolve them.
So right over here, this line here,
clearly it is set up as vertical,
but what if we said, hey, you know,
let's make it horizontal as well.
So if I do that, SolidWorks says, hey, what's going on here?
Notice it says item conflicts or this item is unsolvable.
So we're trying to tell this line
to be both vertical and horizontal at the same time.
Clearly, it can't do that,
so it's either saying you need to delete one of these yellow
or red things so I can solve
or something else you got to fix.
In this case, if I deleted the horizontal,
that would probably fix it.
If I deleted the vertical,
that probably wouldn't fix it because this line,
if it tried to go to horizontal,
would cause a lot of other issues,
but let's go ahead and try it anyways.
So this one here, delete it
and now it's saying, hey, wait, this line is red
because I just can't solve what you've asked me to do.
So let's go ahead and go back.
So undo.
This time, let's go ahead and delete the horizontal.
Hit delete on the keyboard and then boom,
it's back to being all black
and everything is fully defined.
So make sure every time you're creating a sketch,
you create a sketch on a face or plane,
you start that new sketch, draw some geometry out,
tie that geometry into the origin
so it knows where it is,
and then add those relationships and dimensions
so everything is fully defined and black
and then finally,
we're going to go ahead and create that feature.
So come up here to features,
I'm going to choose the extruded boss or base,
drag it up to whatever dimension you want.
You can type that value in right over here.
I'm going to type in three inches and then click on okay
and just that easily with those six steps,
we've created our first solid here.
Now, if you want to go ahead and create maybe a hole in this,
we're going to do exactly the same thing.
We're going to go up here and we're going to choose a sketch.
Choose a sketch.
It's going to ask us, hey,
do you want to sketch either on a plane or a face?
Right, so step number one of the six steps
is select a face or plane.
Let's go ahead and choose this top one here.
Notice we're now in a sketch environment.
Go ahead and drag out or draw out a circle.
There's my circle and I'm going to spin my part around
so I'm looking at the top of it.
So then I'm looking straight on it.
Let's go ahead and tie that into the origin.
So you can do that a couple ways.
One is I could say, hey,
I want a dimension from here over here to the origin, right?
That's one way to do it.
But if you wanted that in the center of this face,
there's a lot better way to do that.
So instead of choosing a regular line,
I'm going to go ahead and choose a center line.
I'm going to snap to the midpoint here and the midpoint here.
Now those two midpoints are defined because it's black
and it knows where the midpoint of that line is
and so if I grab this circle here
and I snap that to the midpoint of that line,
guess what happens?
Defines where it is.
If I add a dimension then of the size
and say maybe two inches, notice everything's fully defined
because, like I said, we tie these into these lines,
which are related back to the origin,
and then the center of this
is related to the center of that line.
So everything's fully defined.
That's what we need.
We have everything fully defined in black.
We tied it into the origin
and now we're ready to create the feature.
So come up here to features, go over here to extruded cut,
and let's go ahead and cut a hole right through there
and there you have it.
So a couple different ways to create extruded features,
extruded cuts.
They're both using those six steps
for pretty much all the features
you'll ever see inside of SolidWorks.