- [Instructor] In this video,
we're going to create the rear dropouts.
These are only small parts
but they're extremely important
because they actually hold the rear wheel.
In most frames, including ours,
the rear dropouts actually fit slightly
inside the chain state and the seat state
and they're welded in place.
So they hold the ends of those two tubes together
and they brace the rear corner of that triangle there.
There's many different kinds of dropouts,
depending on exactly what kind of axle you have
and what kind of brakes and gears you're running
but most older bikes use an open C-shaped jaw
that the axle clamps into.
Through-axle designs are becoming more popular
but these basically have a hole
that a removable axle goes through.
And in our case, we'll stick with the older style.
It's quite simple but it's tried and tested.
But you can really make what you want
and you can adjust these to suit your own needs.
First, we're going to model them up
and then in the next video,
we'll add them to the assembly
and make any changes that are needed.
Start a new part in SOLIDWORKS.
And then start a sketch on the front plane.
And we'll draw up the shape.
Get the circle tool
and draw a circle at the origin
that's 28 millimeters diameter.
In the actual frame, this will be centered
on the rear axle.
Next, we need to make the ribs that come off this.
So let's get the center line tool
and draw two center lines going to the origin like this.
So this one should be horizontal
and this one should go up to the left.
For the angle here,
this is actually the angle
between the chain state and the seat state.
So let's go back to the assembly.
I'm going to go to a side view
and then get the measure tool.
And then I'm going to zoom in
and measure that angle.
So it's the angle between those two tubes.
It's coming out as 57.7.
So I'm going to call that 58.
I'm going to go back to that new part
and then get the Smart Dimension tool
and I'm going to set this angle as 58 degrees.
Now we can sketch the arms of the dropout
using the rectangle tool.
So I'm going to select the rectangle tool.
Choose the center rectangle, this second option
and then start a rectangle at the end of this line
and drag it out.
Something like that.
And then set the size as 16 high.
This left-hand edge should be 40 from the center point
of the circle.
And then for this right-hand edge,
you can just grab one of the points
and drag it to the outside of the circle.
So your sketch should be fully defined at this point.
For this upper arm, we'll also use the rectangle tool.
So select the tool but we'll use this option.
This is called a three-point center rectangle.
So select that one.
Start the endpoint at this line.
And then drag the line down
so it's parallel with the center line
and draw something roughly like that.
For the size, this one's going to be 12 wide.
This endpoint should be 48
from the middle of the circle.
And then select the center line,
hold down Control and also select the outer line.
And then add a parallel relation, which is this one.
Then finally, all we have to do
is grab this point and drag it
to the outside of the circle.
And now your sketch should be fully defined.
It should say fully defined down here.
If not, just find any of the blue lines
and try and drag them around,
and you should be able to see
which relations you need to add.
Now we need to extrude the shape.
So let's go to Features, Extruded Boss/Base,
and let's do a midplane extrude, which is this one
and five millimeters.
And you probably see
that we don't have the usual yellow preview.
That's because we've got intersecting lines in this sketch.
So we've got lines that overlap each other.
This means that we've got multiple closed profiles
in the sketch.
So SOLIDWORKS doesn't really know
which areas we want to extrude.
So we need to specify this.
Click here on the left in Selected Contours.
And then just choose all of the areas in the sketch.
So click on the circle.
And then click on the outside
of these two rectangles.
If you choose the actual shape itself
instead of the area,
then it will select the entire shape.
So the preview should look like this.
It should have no gaps anywhere in that.
So make sure you have midplane five millimeters
and press OK to add that feature.
And if you look at it from the side,
you should see it like this.
There should be no holes anywhere.
If you do have any,
then just edit your feature
and then fill in those areas
and then press OK again.
At this point, we can save the part.
And let's call it Rear Dropout.
So we now have the main shape.
Next, we're going to add a raised section
with a bit more thickness
just for the face.
So this is a sketch on the back face.
So rotate your model around.
Select this rear face and start a sketch.
And then get the circle tool
and just draw a circle at the origin.
This is 20 millimeters diameter.
And let's do a blind extrude, 2.5.
So it should look like this,
just a small raised area.
Then we can rename those two features
as Body and Face.
So this is the basic shape.
These lugs go into the frame and are welded in there.
And then the axle fits within this circle.
So let's make a cutout for that.
Start a sketch on this face
and then go normal to
and let's get the slot tool.
We want to draw a straight slot,
which is this first one.
Start from the origin.
And go down like this.
Make sure you're not going vertical.
Draw something roughly like that.
Make sure you start from the origin.
You might just need to drag that point into the origin.
Let's set the angle from the horizontal here
as 75 degrees.
And then the width across here as 10.2.
But this could be adjusted for different axle sizes.
And then the length,
it can be any length,
as long as it cuts all the way through the shape.
So you could just grab this center point
and drag it to the outside of the circle there
and that should fully define your check.
And then we can go to Features, Extruded Cut
and we can make it through all.
And we can rename that feature as Axle Cut.
So hopefully you can see the function a bit better now.
The rear axle goes in here
and then these parts go inside the frame.
To finish off the design, let's just add some fillets.
So get the fillet tool.
I'm going to add a seven-millimeter fillet inside here.
And press OK.
And then just two more 20-millimeter fillets.
One here and then one here.
So now this part is finished,
you can save it and we'll add it to the assembly
in the next video.