- [Instructor] So for the first project,
we're gonna be designing a valve housing.
Let's get from the very beginning.
Go to New.
Make sure we have our units set up correctly.
Make sure we're creating a model.
We have our folder set correctly.
Again, if you don't remember to set your folder correctly,
you can always go back and do a save as,
to save it to the correct location.
And then give it a name.
Select OK and there's the start of our file.
So what I like to tell people,
when you're designing, depending on what you're designing,
in like in this case we're designing a valve housing,
we wanna make sure we get the main body.
Everything's gonna attach to that main body,
so we wanna use that as a reference for everything else.
So we'll go into our Sketch in Task Environment,
select my x, y plane.
My horizontal reference is going to be x.
And the origin, we'll just use the work part origins.
Select OK.
I wanna draw a circle.
Once again, when I select that initial sketch origin,
it's gonna create that constraint to that sketch origin.
I'm gonna draw my diameter.
Now the size of my diameter I could either just simply click
and modify the dimension,
or I can just simply edit the dimension right now.
Hit enter.
And now you can see my sketch is fully constrained.
Just finish, exit out.
I'm just gonna right mouse click and do a fit.
Now the next thing I wanna do is draw in my next sketch.
It's a separate sketch.
It's not going to be a part of the sketch,
it's going to be a wholly separate sketch.
So I wanna make sure I have them separated.
I'm gonna go into my Sketch in Task Environment again.
Select my x, y plane.
Same horizontal reference.
Select OK and begin drawing.
So I'll just use my profile.
Come in, cross, down, and I want an arc.
So I'll just snap that in.
To constrain this,
I'll just drag this line down to that point.
I wanna take this arc to that line.
Say tangent.
Now as I got through and constrain,
I wanna make sure that I'm getting appropriate geometry.
So if for some reason, you have a setting set,
maybe you accidentally forget to turn on your arc center,
like if you try to pick an arc center,
you may not get that arc center.
You'll notice I actually got the arc,
but not the arc center.
But if you actually want the arc center,
you have to go over here and be very specific
to get that arc center.
You'll see here, that point is highlighted,
versus the arc.
So I'll come back in, specify my vertical axis,
and say Point on Curve.
Place this line on the horizontal.
We'll say colinear.
We'll give this the appropriate radius value, 12.7.
And then the last constraint that I need
is to go from my horizontal to my point.
Now you'll notice I cannot pick my horizontal.
It's not allowing me to pick my horizontal.
So, I'm gonna just cancel.
Sometimes you just gotta go in there, refresh.
If you still can't pick your line,
you wanna make sure you have your method set.
Remember, previously you have it to radial,
and if it's still set to radial,
you won't be able to pick that line.
So in this case I'm gonna make sure
that you have it set to the correct method of measurement.
So I'll go back in, pick my line, pick my center point
and put in my value.
Close.
Sketch is fully constrained and Finish.
We have one more sketch to make.
And that sketch, I'm just gonna rotate the part,
is going to sit on the z, x plane.
Again this is a wholly separate sketch.
I'm gonna end up with three different sketches in here.
Pick my z, x plane.
Now what do I want as my horizontal reference.
So if I come in here, in this case,
if I pick my z, that's going to be my horizontal.
When I hit OK, it's going to orient my sketch.
Draw my circle, put that in.
And this time, I actually drew the circle in
rather than just entering in the dimension.
So I'll just cancel out.
Double click on the existing dimension
and enter in the value, 57.2.
Sketch is constrained.
Select Finish.
Now I have the sketches that are required
for my valve housing.
At this point I'm going to save this file.
File, Save, Save.
Now as a note, just as a reminder,
you cannot save the part when you're inside
the Sketch Task Environment.
Just not possible.
So you have to make sure you exit out of the sketcher
and you have to make sure you hit save once you're done
to save the part to the appropriate directory.