That method works, but is a long way. Depending on if you're using just an extrude or the hole tool, the method changes slightly. With the hole tool, place your hole on the face of the flange, pick your first reference as the center axis you're going to pattern around. Under hole placement tab, pick either radial or diameter, depending on whether you want a radius shown or a diameter shown on your print. For your second reference, pick a datum plane that goes thru the axis. This will become your angular dimension. You should now be able to set your radius/diameter and your angle for the holes position. Accept your hole. You can then create a dimension pattern using the angular dimension on the hole. For extrudes, its slightly simpler. Start your extrude tool and create the sketch on the sufrace of your part. Pick the axis and a datum thru the axis as your references. Create a construction line through the center axis and at a set angle of your datum plane reference. Create a circle at the diameter/radius you want your hole to be at, and right-click->construction. Sketch your hole at the intersection of your construction circle and your construction line. Accept the feature. Now you can dimension pattern according to the angle of your construction line you created in the sketch. The downside to doing it this way is that you'll have to sketch a draft circle in your drawing and a group it to its sketch view, or create a separate sketch in part mode to make your circle visible on the print.