- [Instructor] In the previous video,
we laid out some more sketches in the assembly
to help us make the parts of the rear triangle.
And in this one, we're going to build upon those
to create one of our chain side parts.
From within the assembly, let's insert a new part
by going to Assembly, Insert Components, New Part.
Now, similar to the previous new parts
you might be prompted to enter a file name at this point
depending on your settings.
And if so, just call the part chain state.
But by default, we should just be in the assembly
with is green tech ready to choose a plane
for that new part.
So let's choose the chain state plane
that we previously added
and then go to a normal two view.
You can press the Space bar to open this View menu
and then click on normal too.
So now we're looking directly up
at that plane that was getting on.
Now we want to sketch a path from the end of the axle here
down to the bottom bracket shell
but we need to avoid this rectangular area.
This is where the tire will be.
So let's select the line tool
and then draw something like this.
It's just three lines segments connected together.
So start from the end of the axle, go vertically down,
so we've got a straight section for the dropout
and then we're angled in a little bit like this
and then angled in again
until we're in line with the origin there.
And then press Esc to stop placing new lines segments.
This will be the path of our chains they part from the top
and we can now fully define this.
So I'm getting the smart dimension tool.
I'm going to make this top section 50
and that should have a vertical relation.
For the bottom part here,
I'm going to select the endpoint
and I'm going to select the origin
and make them horizontally in line.
And then I'm going to set the distance here,
press 12 millimeters.
We can always adjust these later on.
And then for this end of the line,
we're going to drag it up here
and I'm going to select that point.
Also select the corner of that rectangle
and then I'm going to add a horizontal relation.
Now we just need to add a distance in here.
This chain stay tube is a smaller diameter than the others.
It's seven eighths of an inch,
which is about 22 millimeters.
So we need to account for the tube diameter
with this distance.
So let's make that distance 14 millimeters.
It's just a little bit larger to give it plenty of space
and that should fully define your entire path sketch.
Then the final thing we need to do
is just round off the sharp edges.
So I'm going to get the sketch fill it tool
and for these bend radiuses
they should ideally be about twice
the chief diameter or larger
so I'm going to make this 50
and then I'm just going to select those points
where the line segments join.
Then if we zoom in,
we can just see we've got a nice radius here and also here.
So we can exit that tool and we can exit that sketch.
Now, if we look in 3D
this is the path of the tube that we're going to make.
We can use this first sketch
to make a suite for the rear tube.
So firstly, let's add a new plane.
Let's go to Features, Reference Geometry, Plane
and then let's click on the end line segment here
and then also click on the end point of the line.
And that will add a new plane perpendicular to that line.
Let's press OK and then start to sketch on that new plane.
You might have to expand the new part to find that plane.
Now we can sketch the profile similar to the other chips.
So it's just two concentric circles.
So we're going to start at the end point there
and draw two circles out like this.
And the diameter for this is seven eight, seven inch.
So with a smart dimension, you can actually just type in
7/8 in and then press, OK.
You see that's converted to millimeters,
it's about 22 millimeters.
And then for the wall thickness,
this is not 0.8 millimeters.
So that should fully define the sketch
because we've set the size
and it's fixed to the end point of that path sketch.
These red tubes are sometimes tapered,
but for the sake of this model,
we're just going to keep a constant diameter.
Exit that sketch and then from the features tab,
let's choose swept boss base.
For the profile sketch here,
we want that latest sketch that we just drew
the one with the two circles
and then for the path sketch,
let's select that bent path like so
and you should get a preview like this.
If you preview doesn't work,
then just make sure
that your two circles in the profile sketch
are centered on the end of the path line.
The profile sketch needs to be touching
the end of the path for the suite to work.
If we look in 3D, we can see the tube goes along
joins that bottom bracket shell
but it will avoid the area where the tire is there.
And we've got a nice bend radius here and here.
So we can press OK to make that feature.
Then the only thing we need to do is notch the end here,
where the tube joins the bottom bracket shell.
So let's use a cavity feature for this.
You can go to Insert, Features, Cavity
and then for the design components,
let's just click on the bottom bracket shell there,
press OK for the bodies to key,
we just want to keep that rear section.
So it should be this one, press OK
and now we've got a nice notch there on the front
and we don't have that front section.
So I can ex editing the part
and we can see we've got a nice change they achieved there.
It's going to avoid where the wheel is
and it's going to go back here
with a straight section for the rear drop power.
So at this point you can rename your part if you need to,
right click on it and press Rename
I'm going to call it Chain Stay
and then you can save your assembly
and save you part externally if you need to.