- [Instructor] Now that we've added
the first two small parts, the bottom bracket shell
and the head tube to the frame assembly,
we can actually start to build up
the rest of the frame with larger tubes.
We could start with any of those tubes really
but we're going to start with the seat tube
because this finishes out the bottom bracket shell.
So it only needs notching,
that's rounding off to suit this shell at one single end.
Open the frame assembly
and it should look something like this.
We've got the two existing parts and the layout sketch.
We're going to create that seat tube part
directly in the assembly.
But before we do, first we need to set up a plane
to start that new part up.
To do this go to the assembly tab,
and then click on reference geometry and choose plane.
Here on the left for the first reference let's zoom in
and select the actual line of the seat tube there.
Then for the second reference,
let's select the top point of that line.
So now we should be adding a new plane
that's perpendicular to that line on the end of that line
and you can press okay to add that.
So we've got the new plane here in the parts tree.
We can rename that by doing a slow double click
and call that something like seat post plane.
Now to insert the seat tube part,
let's go to the assembly tab,
click on the dropdown under insert components
and choose new part.
And if you move your mouse into the graphics area
you should see this small green tick next to the cursor.
Now depending on your settings
you might've been prompted to enter file name at this point.
If so, then just call your new parts
something like seat tube.
But back in the assembly, this little green tick means
that we need to select a plane for the new part.
So let's select that new plane
that we just added, the seat post plane.
Click on it on the left here in the parts tree.
So now we're sketching in a new part
on that new plane that we added
and we can draw our tube profile.
Get the circle tool and let's zoom in
and draw two concentric circles
at the end point of that line.
Something like this, the outer diameter of these is 28.6
which is one and one eighth of an inch.
And if you lose where you are
you can always just press F to zoom to fit,
to zoom back out again.
So for the second circle, we want it to be smaller
than the first one, so you can drag it
so it's smaller than the first one,
and then get the smart dimension tool
and let's click on both circles
and let's make a wall thickness of naught .9 millimeters.
So at this stage both of your circles
should be fully defined
so they should be black in color
because they're both fixed to the origin here
and both of the sizes are set.
Now that we've got the profile
we can create the tube using an extrude.
So go to the features tab, press extruded boss base
and we want to extrude downwards
towards the bottom bracket shell.
So click this button here on the left to flip the direction
and we want to extrude down something like this.
Then for the end condition we could use a blind extrude
and then notch the tube afterwards
but there's actually an easier way to do it.
So notching the tube as we mentioned is,
if I go to a side view,
is cutting away a circular edge of the tube
so it fits perfectly against that bottom bracket shell
at the bottom there.
So instead of using this blind extrude
we can actually go over here to the left,
click on the dropdown and choose up to surface.
Then make sure you're in this surface box,
if not, left click in it,
and then just left-click on the outside
of the bottom bracket shell
and we should get a nice curved preview,
something like that.
Then we can press okay to create that feature
and we can exit editing this part
by clicking up here in the top right.
So now we have that new tube in the assembly.
You should see the new part in your parts tree
and if you see this little circumflex,
the little upwards pointing arrow,
it means this part is a virtual part.
So it only exists in this assembly,
it doesn't exist as a stand alone external part,
depending on your settings,
it might have been creating like this.
If you do see that little up puts arrow,
the circumflex, just right click on the part
and press rename part.
Let's call it seat tube.
You can also then right click on it again
and press save part in external file.
I'd recommend that you just click same as assembly here
and then okay.
This means that we've now made that virtual part
into a normal external part.
We can open this just by clicking on it
and pressing open part
and if we move it around you can see at the end there
we've got that nice notched end
where it meets the bottom bracket shell.
So at this point just make sure all of your parts are saved
and we'll continue on in the next video.