- [Instructor] When modeling something like a bike frame,
it can be hard to figure out where we should actually start
because so many of the parts are created
with reference to each other.
When working virtually in CAD,
there's often no specific right or wrong place to begin.
For our model, we're going to start
with quite a small part, the bottom bracket.
And this is the area where the downtube, the seat tube,
and the chainstays all connect together.
And it's the part where your crankset attaches,
so it's basically where your pedals spin around.
Now when people talk about the bottom bracket,
they're sometimes referring to different things.
But often they mean the actual spindle,
the part with the bearings
that allows your cranks to spin around.
The part of the frame that holds the spindle
is usually called the bottom bracket shell,
and that's what we'll be making.
There's many different types of bottom brackets.
Some might screw in, some are press-fit.
But we'll assume that our screws in using threads.
If you're making this frame in real life,
then you might actually buy the entire bottom bracket shell
as an off-the-shelf part.
But you can also create it yourself using tube
and cutting the threads.
In our case, we're going to model this up ourselves,
and you'll find a PDF drawing of this in the exercise files.
So open Solidworks and start a new part.
It's quite a simple model really.
It's just a tube that has
slightly thicker walls towards the end.
We'll draw this using a revolve.
So start a sketch on the front plane,
and let's draw both a vertical and horizontal center line
starting at the origin.
So you can get a center line by clicking on the dropdown
next to the line tool.
And draw the center lines like this.
Now let's draw the revolve profile.
So get the line tool,
start from the top of that vertical center line,
and draw something like this.
This is going to be half of our revolve profile.
So we can mirror this over to the other side.
To do this, select Mirror Entities from the Sketch tab.
And then in the Entities of the mirror box,
let's drag a box around those new lines.
So those new lines should be in that box.
For the Mirror about,
let's select that vertical center line.
And you should get a yellow preview like this.
If you're missing any of these lines,
then just make sure they're in this box on the left.
Then press okay, and we've got
the entire revolve profile there
so we can use Smart Dimension to set the size of this.
We're going to use a very common standard size
which is 73-millimeters wide
and what's known as a British or BSC thread.
But if you've got a different size of bottom bracket
that you want to use,
then feel free to adjust these numbers.
So let's get the Smart Dimension tool.
Firstly, for the overall width of the shell,
let's make this 73 millimeters.
And you should find as you add that first dimension,
the entire sketch resizes automatically.
For the outer diameter here,
it's going to be 1.5 inches.
And often you'll find with old frame components
that many of them are based on old imperial sizes.
So even though I'm working in millimeters.
You can see down here MMGS,
stands for millimeters, grams, seconds.
We can actually add dimensions in inches.
Click on that upper line
and then click on the center line.
But before you click again to add the dimension,
just have a look at the dimension.
If it's up here above the center line,
you see it says 16.
If we move it below the center line,
that actually doubles to 32.
So we can use this to set the full diameter.
So let's move it down to the bottom
and then left click to add that dimension.
And you'll remember that the dimension was 1.5 inches.
So let's type in 1.5,
I-N for inches, and then press okay.
And you see that's automatically converted
into millimeters, 38.1.
So even though I'm not working in inches,
we can still write in inch dimensions.
Next, we'll set the wall thickness here.
So this should be 1.4 millimeters.
And if you find that your lines move around,
you can just drag them back to the correct place.
So next, we'll dimension this thicker section.
This should be half an inch, 12.7 millimeters.
So I'm going to write 0.5 I-N, and then press okay.
And you see that's converted into inches as well.
Then finally we just need to set the thickness
of these end sections.
These will have a thread cut into them
which will be that British thread that we mentioned
which is 1.370 by 24 threads per inch.
So in practical terms,
this just means that we need to leave
a bit of extra thickness at the end here
for the thread to be cut into.
So we'll set this diameter as 34.
So click on the line, then click on the center line,
and let's set that as 34 millimeters.
So now we've got a fully-defined profile for the tube.
All we need to do is revolve it.
From within the sketch,
let's go to Features, Revolve Boss Base.
And then for the Axis of Revolution here,
let's select that horizontal center line.
And you should get a preview like this.
Press okay, and now that feature is created.
So it's a very simple part.
If we now go to a cross-section view,
we can see it's just a tube with these thicker ends
where we're going to cut the thread.
Before we finish, let's just insert an access
that will help us line the shell up in the assembly.
And to do this,
you can go to a Features, Reference Geometry, Access.
And then just click on this outside circular face.
Press okay, and we've added the access along the middle.
And then you can save your part.
Let's call it something like Bottom Bracket Shell 73 BSC
for British Standard Thread, press Save.
In the next video,
we'll create an assembly
and we'll insert this part into it.