iLogic Tutorial – Creating the hinge sketches
Start by grabbing the Line tool and drawing a short line parallel to the stile and about 2″ long. Make sure you are seeing the Vertical constraint glyph before ending the line. If you don’t have the Constraint placement priority set to Horizontal and Vertical, you should do so now by selecting the Application Icon, Options (at the bottom), then on the Sketch tab, make the change in the 2D sketch options at the upper left. Now, starting in the center of the first line (wait for green dot as shown in the image below), create another line tangential to the first. When you see the Horizontal glyph, and the line is an inch or so long, finish up the line. You should have something that looks similar to the image on the right below…
Now you need to grab the Point tool from the Draw tab, and add a point to all three line ends. When you get the green dot, click. After the last point is placed, right click anywhere and choose Done. Now get the Circle tool from the same panel and draw three circles to get a sketch that looks similar to the one below…
Now window select the whole sketch you just created, and change the lines to construction geometry. The points are the only geometry that will be used to create features. The circles are only there to show design intent. Now select the Project Geometry tool from the Draw panel, open the origin folder in the browser, and select the YZ Plane . Highlight the line just projected, and click the Centerline tool located on the Format tab.
Now it is time to start adding dimensions to the geometry using the parameters we created on page one . Get the Dimension tool from the Constrain Panel , and select the uppermost circle. Click the little arrow pointing right on the Edit Dimension…
…dialog that appears, and choose List Parameters from the list. Scroll through the list and find Hinge_Cup_Diam and select it. The upper circle should now display a diameter of fx:1.378. Now add dimensions to the two lower circles, but this time use the Hinge_Dowel_Diam as the parameter.
The new dimensions will display fx:.315. even though the parameter is stated in mm -this is because the standard units for this model are in inches.
Your sketch should now look like the image to the left. Continue to add dimensions by adding a dimension to the line that connects the two smaller circles representing the dowel holes. Add the Hinge_Dowel_Space parameter to that line. Add the Hinge_Dowel_Offset to the other, tangential, line that goes up to the large circle.
Now add a dimension from the centerpoint of the large circle to the line at the end of the stile (top edge that was projected at the beginning if the sketch) Use the Hinge_Offset_L parameter here.
The last dimension to add (for now) is the distance between the large circle and the edge of the stile. To achieve this, start by selecting the edge of the stile (line closest to you) then move your cursor over the point on the circle closest to the line until you get the tangent glyph, then click and add the Hinge_Setback parameter…
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