iLogic Tutorial – Extruding more hinge bores
We will now do pretty much the same thing for the next set of holes –create two hole features and pattern the features to create the instances needed. The major difference is that there will be three patterns created that represent the rest of the possible hole patterns. The first thing to do is get rid of the dimension visibility to make things easier to see. Right click on the Lg Hinge Layout and select Dimension Visibility to uncheck it. you should now have a screen similar to the one below…
We will do the cup bore first for the sake of continuity. Get the Hole tool from the modify tab, deselect the five previews that are not applicable, you will only be doing the close, large hole. Make sure the right rail is selected as the solid that the operation will be performed on (outlines with dashed magenta lines), change the hole diameter to the Hinge_Cup_Diam parameter, and make sure the Drill Point is set to flat bottom. Click OK to create the feature. This sketch is already shared, so you just need to find the Lg Hinge Layout sketch in the browser, right click it, and change the visibility back to visible. Change the name of the feature to Right_Cup_Bore. You can now create the two dowel holes nearest to you. Notice that when you click the arrow to the right of the Diameter field on the Hole Dialog, there will be recently used parameters listed just below the List Parameters option, choose Hinge_Dowel_Diam from that list. Due to a flaw in the program, you will again need to change the Drill Point type to a flat bottom as the program does not default to last used as expected. Make sure only the two holes you want are previewing, and that the right stile is selected as the solid that the operation will be performed on, then click OK to perform the operation. Change the name of the new hole feature to Right_Dowel_Bores and save the part. Next we will create three patterns of this set of three hole.
The first pattern is created exactly like the pattern created for the last set of holes, with the only difference being the parameter used for the spacing. This one uses the Mirror_Offset_L parameter. Begin by selecting the Rectangular tool from the Pattern tab. Select the two hole features just created in the browser, click the direction arrow and select the closest, long edge of the right stile, Flip the direction if its wrong (it almost always is), leave the count at 2, and choose Mirror_Offset_L from the parameter drop-down in the distance field. As always, make sure the correct solid is selected. Click OK to accept the settings and create the feature. Rename the new feature Med Pattern Right and save the file.
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