- [Narrator] Next we're going to model the head tube.
This is another of the smaller tubes
and it sits at the front of the bike
and contains the headset
which is basically a collection of bearings
that holds the front fork
and allows you to turn and steer the front wheel.
There's many different types of headsets and tubes
but most operate on a fairly similar principle
and most fit inside fairly similar head tubes.
For this model, we're going to assume that we're using
a headset that uses cups that are press fitted
into a standard head tube.
This head tube is fairly similar
to the bottom bracket shell.
In that you could probably buy the part off the shelf
or you could make it fairly easily from tubing.
So let's start a NEPA and start a sketch on the front plane.
Then similar to the bottom bracket shell,
we're going to get a sensor line and draw two center lines
from the origin, one vertical and one horizontal.
Then we can start to sketch the profile
for the tube using the line tool.
So start from the end of that horizontal center line,
going up a little bit and then it steps in.
And then on the outside, it's pretty similar.
It goes down a little bit and then it steps in as well.
And then it finishes there.
So this is half of our tube profile
and we can mirror this about to get the other half.
Drag a box around those lines to select them
and then hold down Control and also select
that horizontal center line.
So we don't want to select this vertical one,
just the horizontal one.
Then go to the Sketch tab and press Mirror Entities.
And we should mirror those lines about
because we just had that one center line selected.
So this is our tube profile
and we can now start to add dimensions.
Get the Smart Dimension Tool
and we'll set the total height as 170.
Then this inner thin section is 45.
Remember if you select the line and then a center line,
you can move the dimension over to get the full diameter.
So that diameter is 45.
And then these end sections are 15 millimeters.
The diameter of these end sections is 43.9.
So this is where the 44 millimeter cups will be pressed into
Then for the outside here,
these end sections are 50
and the middle here is 48.
So that's just to keep the weight down a little bit.
Then these ends are five millimeters high.
So that should fully define your sketch
and we can now use this profile to create or revolve.
So go to Features, revolve Boss Base
and then for the axis of revolution,
let's choose that vertical center line
and we should be making a tube like this.
Press Okay and that feature is made.
Then to finish off,
We're just going to smooth these transitions on the end.
So get the Fillet tool, set a 10 millimeter fillet
probably be there by default
and then zoom in and let's select this face on both ends.
And then inside, we also want to select this face
on both ends.
So we should have four edges in total.
You might need to spin your model around
so you can see this one on this side.
And if you select the wrong one by mistake like this,
you can just click it again to de-select.
So we should have those four edges there.
Press Okay to add those fillets.
Then you can save this part
and let's call it something like head tube 44 by 170.
Now we can open the assembly we made in the previous video
and add this part in.
So open that assembly.
I'm going to switch window to that assembly
and we're going to add that head tube part in.
If you were making this frame in real life,
you'd probably use some kind of jake to fix these parts
in place for welding.
Or maybe you'd start with the frame tubes
connected to the bottom bracket shell first
so that you have a fixed anchor point.
But in this virtual model,
doesn't really make much difference.
So let's insert that head tube now.
Go to the Assembly tab and click on Insert Components
and you should see your head tube there.
If you don't see it, it just means the part isn't open
in Solidworks.
So you can click Browse
and then just find the file on your computer.
So select that part
and this time don't click this green tech.
Let's just click somewhere in the graphics area
so we can place that part but it's not fixed anywhere
and we can still move it around.
Now let's use our layout sketch to fix this in place.
So select the outside of the tube, hold down Control
and then select this head tube line in the layout sketch
and then release Control
and we should be able to choose a concentric mate
which is this one.
Left click to add that
and now the tube is aligned along that head tube line.
To fix it in place, let's zoom in a bit.
You can drag it down a little bit and select this top face.
Make sure you get the face and not the edge.
Hold down Control
and then also select the end of that line
and then release Control
and let's add a coincident mate.
So now if we go to a side view,
you can see the head tube is fixed in place there.
Now we've got those two initial parts.
We can save this assembly and we'll continue on
with building the rest of the frame.