There are some situations where you need to calculate feed rate differently. For one thing, there are several different types of tap holders, which will more or less determine the method. If you have a machine that has a rigid tap function, you do not usually need a floating tap hold holder unless the machine synchronization is not good. Some machines are just better than others in that regard.
In that case, feed the tap at the exact thread pitch, or will put stress on the tap and may break it, especially in hard material and/or deep holes. For example, tapping ¼-20 holes in aluminum you could use 20.0 IPM at 400 RPM, or even 40.0 IPM at 800 RPM. For production, we would program even faster, for 1 of a kind projects we tend to keep it more conservative. You don’t need to make 20 FPM and 400-RPM increments, but I like to keep it even as I don’t like to round off the feed rates.
Some machines are programmed with the pitch for the federate. For example, the feed rate for a 20 threads per inch tap would be F.05 (1 divided by 20 = .05), and for a 32 thread per inch tap it would be F.03125 (1 divided by 32 = .03125).
Some tap holders have tension and compression, some extension, and some only compression. If you don’t have compression, then you want to feed the tap a little slower than the pitch, so the tap is extended for some give at the reversal. If you didn’t have extension, then you might need to feed it a little faster than the pitch. When a tap holder has compression, then it may compress more or less at the start, depending on hold chamfer and how quick the tap “starts”. So you will use some Kentucky windage on both depth and federate at times, to suit the situation, as it can’t be calculated exactly before hand, although with experience your first estimate should be in the ballpark. Even a different RPM may affect when the tap actually starts, and thus the depth.
Also, some stainless steel alloys are much more forgiving than others, 303 is pretty good, where as 304 is noticeably more difficult. We have tapped 100’s of thousands of 6-32 holes through ¼” 303 at 400-800 rpm (depending on the machine) with Trim Sol cutting fluid, with very little tap breakage. But good tap fluid is an extra insurance when you are in doubt. Also, drilling the holes just a little bit larger on difficult jobs may provide plenty of thread strength for the job, but reduce your tapping woes significantly.  |