Copyright Goodheart-Willcox Co., Inc. Chapter 9 CNC Mill Programming 201 same relationship to spindle speed. This is a hand programming impossi- bility. Tapping used to be done with a floating tapping head to allow some flex while the machine slowed down and reversed. Now, the controller and servo motors can do the math automatically, once the machinist calculates feed and speed with relationship to the threads per inch (TPI) of the tap. It is easiest to start with the spindle rpm and then calculate the feed rate. Assume a 1/4-20 tap (20 represents threads per inch) and 700 rpm for spindle speed. This is the formula for calculating feed rate: rpm ____ TPI = Feed rate 700 rpm ________ 20 TPI = 35 feed rate G0 G90 G54 X1. Y1. M03 S700 (X1. Y1. is location of first hole) G43 H1 Z1. M8 G0 Z.25 G99 G84 Z−.5 R.5 F35. X2. Y2. (Second hole) X3. Y3. (Third hole) G80 Explanation of cycle: ■ G99: Returns to reference return position (.5″ in this case) between holes. ■ G84: Turns on tapping. ■ Z: Final depth of hole. ■ R: Reference plane. Notice a larger .5″ height, which allows tap to get to speed before entering hole. ■ F: The feed rate while tapping. Critical feature. Notice 700 rpm above. From the Shop How Fast Can You Tap? In the G84 example, we used 700 rpm as the spindle speed for the tap. Why? Well, it was an example of what speed we might use if tap- ping steel. You will fi nd that there are many variables at play in tapping speeds for example, type of material, type of tap, coating on tap, depth of tap, or even the class of thread. There is not one answer that fi ts all taps. It will take some experience and some expert input to help you get the best spindle speed. Your best resource is the tooling manufacturer’s recommended speed chart for your specifi c tool, or a tooling engineer from that manufacturer. Start with a slower, conservative speed and then increase speed, with some trial and error. The optimum speed will be fast and provide long tooling life. But remember: if you change the speed, you have to recalculate the feed. 9.8.6 G85 Cycle (Fine Boring Cycle) The G85 cycle is used when boring or reaming holes. The tool will be positioned over an existing hole and feed down to the final Z depth. rpm ____ TPI = Feed rate m _ Tech Tip When using the G84 cycle, spindle and feed rate overrides will be disabled by the control to maintain the spindle-feed relationship.