- We will be starting with the bottom end of our engine,
and in this video we will sketch out
the necessary contours for the extrusions
to block out our design.
First create a new part using the Part Import
from the My Template tab.
Save and name the file to a location of your choice.
I will name my file as 0101FlywheelSketch.
Saving up front is a good practice
and will allow us to simply do a keyboard Control-S
to save as frequently as we deem necessary.
My preferred method of starting a sketch on a plane
is to left-click on the Relevant Plane icon
within the Feature Manager,
and then select the Sketch command
from the Context toolbar.
Feel free to use other methods covered
in the Essentials course if you prefer.
Now let's start a new sketch on the front plane.
I'm starting on the front plane since this is
the orientation I want my front view to be
when doing a drawing of this part.
Since this is our first feature,
the graphic view will automatically rotate
normal to our screen.
Subsequent features will not rotate normal to our screen,
and we will need to use the Normal To command when needed.
We will always use our origin,
the two red arrows found at the center of our graphics view
as an anchor point in some way or another.
This is a good practice and will make
fully defining or constraining our sketches easier.
Select the circle command from the mouse gesture wheel,
and sketch a circle with its center point constrained
onto the origin.
When sketching in SolidWorks we do not concern ourselves
initially with the exact size of our geometry
since we will capture our design intent
after the required profile is complete
with either relations or dimensions.
With the circle in place,
let's sketch a vertical centerline with its start point
on the origin which we will use to establish
both symmetry and the height for our next profile.
With this in place, let's sketch the next profile.
Follow my lead, and again don't be concerned
about exact sizing.
Right mouse click in the graphics view,
and select the Center Point Arc command,
and at the top point of the centerline,
sketch an arc similar to this.
Next, sketch the two lines joining the arc and the circle.
Next, add a tangent relation to the circle
and left vertical line.
Simply select the circle then Control-Select the line,
and from the Context toolbar select the
Tangent Relation option.
Do the same for the right-hand line as well.
To select the two lines I could instead
left-click and drag my mouse from bottom right
to top left making sure I'm touching the circle and line
which is a more efficient way at times.
Note that I don't move my mouse after the selection
so I can make use of the Context toolbar
instead of having to go to the Properties tab
to make these selections.
It is far more efficient.
Now do the arc points as well in the same way.
I'll do the left side first and then the right.
Select the three vertical lines dragging
from right to left again.
Since we have two solid lines with a centerline
in the center of the two,
our Context toolbar will now also have
a symmetrical relation.
Select it to make the three lines symmetrical.
Sketch a centerline horizontal between the two
solid vertical lines.
Right-click on the horizontal lines
so we can use the Select Midpoint command.
Then Control-Select the vertical line
and select the Make Midpoint Relation.
We do this so these lines intersect
exactly at their centers.
We will be using the horizontal line later
as a reference.
Grab the Center Point Arc command again,
and sketch an arc as follows making sure that the
start and end points are 180 degrees perpendicular
to the origin.
With this arc in place, join the arc points
to the circle with a line on each side
to close the profile.
We have completed the necessary profiles,
and in the next video we will add the necessary dimensions.