iLogic Tutorial – 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 �” 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…
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