- Now that we have our completed profile,
and the necessary relations are captured,
we will add the necessary dimensions.
Let's say that the design intent
is that the center circle dimension will be our
driving dimension to which the other profile dimensions
within the sketch will be related.
To easily capture this, we will use equations
for our dimensions.
This will allow us to later change the circle dimension
and all other dimensions will update automatically
keeping the scale of the other profiles or contours
in scale to the circle's size.
With the dimension tool selected,
first add a dimension to the circle,
and in the modified dialog that pops ups
set the value to 100 millimeters,
add a dimension to the top arc,
and from the keyboard select the equals key
which activates equation entry mode.
Now we can select the circle's dimension
from the graphics view,
and using the asterisk key multiply by .3.
Enter, and enter again.
As easy as that, we can create equations for our dimensions.
Now, note that the red symbol now presents itself
on our dimension and this tells us there is an equation
attached to this dimension.
We will use percentages to keep our equations simple,
and next add a dimension to the vertical center line,
and in the same way let's multiply that by .7.
Next dimension, the bottom arc, again referencing
the circle's dimension and multiply by 1.2.
Our first sketch is complete,
and we have captured its intended design intent.
Everything is looking good.
Go ahead and complete the sketch from the
confirmation corner which is found on the top right
of our graphics view,
and let's save our work.
Use the icon on the menu bar,
or simply Control-S on your keyboard.
In the next video, we'll extrude the created profiles.