- To start on the connecting rod open
from the chapter two folder
the 02_01 Conerod Start part file.
On the front plane we have an existing sketch
constructed with a (mumbles) angle, a start spline,
and three point arc command, which we have
already used in chapter one.
Note that we have sketch one as the main profile
and it is on the front plane.
This is so that this orientation would be
the front view on a detailed drawing if needed.
Now let's select sketch one and do an extruded bus.
Since we will mirror the extrusion we will do
a blind extrusion in one direction only.
So set the depths to 16 millimeters
and note that in the properties we do have
an option to add draft to our extrude if we wanted.
Now this is useful if we want to add draft
to all the sides of the profile, which we don't
want to do at this stage.
Let's complete the command and look
at the next tool that we'll be using.
Next I want to add draft, but only to select faces.
Now for this we have on the features command bar
a draft command.
Now click on the draft command
in the property manager.
For the type of draft use a neutral plane.
With a neutral plane box selected select
the back face of the model.
If needed, reverse the direction so the arrow
in the graphics view points to the front.
Set the draft angle to five degrees.
With the faces to draft selection box selected
select only the three top side faces so that
the draft will not be added to the two
vertical and bottom side faces.
Now complete the command and you can see
that we have only applied draft
to the three selected faces.
On the front plane let's sketch a circle on the origin
and let's dimension this to 75 millimeters.
Now from this do a blind extrude and we will
set this to 21 millimeters and in one direction only.
Make sure that it's extruding toward the front.
Complete the command.
Now select sketch two, which is a recess profile
for the front face of the model, and let's do
an extruded cut this time.
Now set the from option to surface, face, or plane,
and select the large front face of the model.
Make sure the direction is set so it cuts
into the model.
We'll use a blind in condition at a depth
of 5 millimeters.
Under selected contours delete the sketch two
entry that's already there, and then from
the graphics area let's select the three outer edges
of the slot sketch entities.
Let's complete the command.
Now on the front plane let's start a new sketch
for the profiles of the bearing
and shaft holes of the cone rod.
Select the bottom circular edge and do
an offset entities command at five millimeters
and to the inside of the selected edge.
Sketch a concentric circle to the larger top arc.
Note that the top arc has been sketched
on the front plane.
Now remember you can wake up the center point
of the underlying arc by hovering over
the arc edge with the circle command selected.
Using shift dimension we will dimension
the underlying arc to the new circle
at eight millimeters.
Do an extruded cut with a through all in condition.
Reverse the direction if needed.
With that done let's select the mirror command.
Select the back face of the model as the mirror face.
Then activate the bodies to mirror selection box
and then from the graphics view simply select
the model and we can go ahead
and complete the command.
Let's leave it at that.
Save your work and I'll see you in the next video.