Tapped Holes in all Directions

How many times have you needed to complete an extra setup for that one hole at an angle to the surface you have machined, or perhaps a radial hole on a circular component that requires drilling and tapping?

One way to overcome this extra setup is to use a fixed angle tool or even an adjustable tool for the most flexibility and whilst these tools are readily available from most tooling suppliers, the difficulty can be with the canned cycles in the machine. These drilling and tapping cycles make the assumption that the drilling or tapping action is going to be performed in the Z-axis direction – fine for the majority of cases but in the examples above that is unlikely to be the case. 

So as a programmer how do you overcome these problems

You could sit down and write specific sub-programs and use a floating tap holder to allow for the change in spindle speeds through the tapping cycle, however if you are using a Haas machine, you have the General Purpose Tapping Cycle G184 for CW tapping, designed by Haas’ control engineer’s and incorporated it into all Haas mills since 1999. The syntax for the cycle is below and with its sister cycle, G174 for CCW threads, these standard features can have a marked effect on programming time and reducing setups. For additional information please consult your Haas manual or contact our Service Dept. for further assistance.

G184 General-Purpose Rigid Tapping

• F   Feed Rate in Inches Per Minute.
• L   Number of Repeats.
• X*  Optional X position at bottom of hole.
• Y*  Optional Y position at bottom of hole.
• Z*  Optional Z position at bottom of hole.

This G-Code is used to perform rigid tapping for non-vertical holes. It may be used with a right-angle head to perform rigid tapping along an X or Y vector on a three axis mill, or to perform rigid tapping

along an arbitrary vector with a five-axis mill.  

The machinist must ensure that the head is positioned correctly before the G184 command is given. If the head is not aligned with the direction of motion, the tool will break.  Also, he must ensure that the ratio between the feed rate and spindle speed is precisely the thread pitch being cut, otherwise the threads will be stripped or the tool will break.

This canned cycle is modal in that it will perform tapping each time a new motion is commanded. However this will only result in a tapping motion, rather than a re-positioning motion.  Therefore the

only use would be for performing successively deeper taps in the same hole. You do not have to start the spindle before this canned cycle.  The control will automatically use the speed specified by the last S command, also, unlike G84, there is no R plane.