iDoor with iLogic -
Rules for Automatic Hinge Boring and
Size Limits
Page 4 - Creating
the hinge sketches - continued
After the last dimension was added,
the sketch should have turned blue indicating that it is now
Fully Constrained 
. In the image below, I have changed the
Dimension Display setting to expression so that you can compare
to those you have added. The name of the dimension may be
different, it doesn't matter, it is the parameter or expression
--the part after the = --that matters. If you want to set your
dimensions to display this way, right click anywhere in the
Graphics Window and choose Dimension Display. Choose Expression 
from the list. This setting looks very cluttered when zooming
out, go I generally do not leave it this way. The original
setting was Value if you want to reset.
The next line is just for a visual check later on.
Starting on the centerpoint of the large circle, draw a line to
the right. As always, make sure you see the constraint glyph
before ending the line. The length does not matter. The line
should be blue and solid, and the notification area at the lower
right of the screen should state '1 dimensions needed'. We will
now add that dimension. Grab the
Dimension 
tool from the
Constrain Panel 
and add the Mirror_Offset_L
parameter (the L stands for long). How long this dimension winds
up being is dependent on the current size of the door as it uses
the Opening_Height parameter in its equation.
No matter what height the door is changed to, the end of the
line will remain 3.5" from the bottom of the stile. If you
door opening is 24", which is what it should be if you haven't
changed it, the equation should be fx:16.875 which is 24" minus
two 3 ½" hinge offsets and two 1/16" gap
allowances. Make this line a construction line to help
uncluttered things. We will now mirror some of the geometry over
to the left style. It is normally better to mirror features
rather than sketch geometry, but in this case the latter needs
to be done.
Select the Mirror 
tool from the Pattern Panel
,
and select all three circles as well as the three center points.
Click the red arrow button to change the selection to Mirror
Line, and select the projected YZ line that was changed to a
centerline earlier, and click apply.
Click the Finish
arrow, and save. We will now create another
sketch on the same stile the same way that this one was created.
After starting the sketch you will get the projected edges
again. This time, just delete them. Now grab the Project Geometry 
tool from the Draw Panel 
, and select all six points (3 on
each side) and the centerline. To check whether you have done it
correctly, just turn off the visibility of the previous sketch.
You should have a sketch like the one below...
