- [Instructor] We're now going to create the seat stay part
in a very similar way to how we created the chain state.
From within the assembly,
let's insert a new part.
So go to Assembly, Insert Components, New Part.
And similar to the previous new parts,
you might be prompted to enter a file name at this point.
If so, then call this part seat stay.
If not, let's choose the new plane for the new part
and that will be the Seat Stay Plane down here.
Now, we need to draw a path for the seat stay tube
and this is similar to the chain stay tube
but it actually goes to an even narrower point
because it has to go all the way in
to the seat tube here
and for this reason,
the seat stays are often even a smaller diameter
then the chain stay.
Maybe only 14 or 16 millimeters.
Now, these lines can be tricky to see at first,
so let's get the line tool
and let's start in 3D.
Let's start from the end point of that axle.
Let's go vertically up.
So make sure you get that vertical relation.
And then let's go in at an angle
to roughly about there
and then go to the end point of that seat stay line like so.
And then you can go to a normal to view.
Remember, you can open this view menu
by pressing the space bar.
Now we can use Smart Dimension
to fully define this sketch.
So this end vertical section
is 50 millimeters.
Like so.
And then the other end point
is already fixed there.
So all we need to do
is move around this point.
Let's select that point, hold down Control.
Also select the corner of the rectangle
and then add a horizontal relation.
Then for the distance here,
this can be smaller than the chain stay tube
'cause it's a smaller diameter tube.
So I'm going to make this 10 milometers.
We can always adjust this later on.
And then for the radii of these corners,
let's get the sketch filet tool
and let's make this 40.
So I'm going to add a radius there
and also a second one here.
And then that should be a fully defined sketch
and we can exit that sketch.
And if we look in 3D,
we can see we've got a straight section here
for the rear dropout.
And then we go up here,
we avoid that tire area
and then we go all the way in
to the seat tube there.
So now we can draw the tube profile.
First, we need to add a new plane.
So go to Features, Reference Geometry, Plane
and then zoom in,
click on that straight section at the end of the path.
Then also click on the end of the path.
And press OK.
And then we want to start a sketch on that new plan.
So you might need to expand the new part
in the parts tree, click on the plane and press Sketch.
Then get the circle tool
and let's draw our tube profile.
Just two concentric circles,
starting from the endpoint of that path.
The outer diameter is 16 millimeters.
If you lose where you are,
then just press F to zoom all the way out.
And then go back to the right place.
And then the wall thickness is 0.8 millimeters
and that should fully define your sketch
'cause we've set the size
and the position is set at the endpoint of that path.
So you can exit that sketch
and we can create our swept tube.
Let's go to Features,
Swept Boss/Base
and then for the profile sketch,
let's choose those two circles
and for the path sketch,
let's choose those bent lines like this
and that looks good in 3D.
We're still going to avoid where the tire is.
So press OK to add that feature.
Now we need to cut the end away here
so it suits the seat post.
So let's go to Insert, Features, Cavity.
For the design components,
let's click on that seat tube,
press OK, and then for the bodies to keep,
let's just keep that rear section.
So for me, it's this one.
Press OK, and now we've got a nice notch
at the front there.
So we're almost finished
but we just need one final little tweak.
If we click on the end of the seat tube here,
and press normal to,
now we're looking down from the top of the seat tube.
If we zoom in, we can see this seat stay
actually crosses over the center line of the bike.
This line is the middle of the bike.
But later one, we're going to mirror these parts
over to the other side for the second half
of the triangle.
So if we cross over like that,
there'll be a problem
because the two parts will clash with each other.
So we need to move the seat stay over
to the left a little bit more.
And we can do this just by editing that path sketch.
So expand the new part in the parts tree,
expand the sweep feature
and then edit the path sketch.
So it should be on this one, click on it,
and press Edit Sketch.
And then just click on the endpoint of the line
and delete the coincident relation.
So you can click on the icon here
or you can click on it here on the left
and press Delete, it's the same thing.
And then let's just move it out
to the side a little bit more.
So roughly about there.
And then go to a 3D view and move around.
Get the endpoint of that line,
hold down Control and also get the endpoint
of the sketch line there.
And then add a horizontal relation.
And then for the size,
let's try five millimeters.
So that should fully define your sketch.
Let's press OK.
And the new tube is updated.
Let's go and have another look.
So I'm going to zoom in, choose the top of the seat post
and press normal to
and then I'm going to zoom in
and now you see that looks good.
It's all over on this side.
So when we mirror this part over to the other side,
we're going to have a very small gap there.
So at this stage,
you can exit editing your part
and you can rename your part if you need to
by right clicking on it, pressing Rename.
I'm going to call it Seat Stay.
And then save your assembly
and save your parts externally if you need to.