Interpolating Holes vs Twist Drills

They say nothing removes material faster than a twist drill. Just one problem, it only removes a cylinder of it, so it can’t really profile or pocket (the exception being pluge roughing, but I’ll save that for another time). Although, profiles and pockets often begin with the need to get the endmill down to proper cutting depth. Given that you know how long a tool change takes on your CNC mill, how many such plunges do you think are required before you’d be better off to use a twist drill to do the initial plunge and then let the endmill interpolate off of that?

It turns out to require fewer holes than I would have thought, and it’s pretty easily to calculate with a little help from G-Wizard to get the feedrates.

For a 1/2″ HSS 2 flute in 6061, GWiz gives a plunge feedrate of 4.96 IPM. A 1/2″ HSS Twist Drill can be fed at 15.28 IPM. That difference in speed, with the Twist Drill being a lot faster, has to make up for the toolchange time. In fact, let’s say we want to change twice–from endmill to twist drill and back. Further, lets say our toolchange time is 5 seconds.

Based on all that, if we use the twist drill to drill just 2 holes we are 6 seconds ahead. If we have multiple parts laid out on the table, its pretty easy to see how this multiplies in a hurry to our advantage.

Of course we’d need a CAM program that’s capable of drilling all the holes with the twist drill and then going back and pocketing off those holes without cutting too much air. I don’t think my CAM program, OneCNC, is nearly smart enough to figure it out on its own. But perhaps I could convince it to do the right thing with some suitable fiddling. If nothing else you could create a CAD drawing that showed the holes drilled as solid features not to be milled into. It would make an initial helix pass down around the outside of that slug, and you could bump up the feedrate there to regain the lost speed. Make the slugs hole size minus the tool diameter in side, so ideally you want to use a twist drill a bit larger than your cutter diameter. Maybe 3/4″ for my 1/2″ endmill example.

Of course if you have a 1″ indexable drill sitting in the changer, you can bump the feed up to 38 IPM and really make some holes! Incidentally, I have read accounts of folks leaving a 1″ in the toolchanger on lathes just to make boring go faster on bores that are more than 1″. Same idea.

The interesting thing is not only is the twist drill often faster, its a cheaper tool to put the wear and tear on. Click here to download the quick and dirty worksheet I used for my calculations.

There are tons of tradeoff decisions like this to be made when setting up a CNC job. For example, the usual inclination when profiling or pocketing is to select a cutter that is just equal to the minimum radius to be machined. But you’re penalizing the whole cut with that smaller tool. Most of it could be handled by a bigger tool. Given a knowledge of which tools are in your changer, and the possibility of using 2 tools instead of one (rough with a larger radius, finish with a smaller), and a knowledge of your tool change speed, how much savings can you get using 2 tools instead of 1 and is it worth it?

Remember, the larger tool not only removes more material just by virtue of its size, it is also tremendously more rigid as G-Wizard’s rigidity and cut optimizer modules will show you. What if the roughing pass with the larger tool can cut full depth while finish takes 2 steps to get to full depth? Now the 2 tool approach really has an advantage.

CAM programs have a facility called “Rest Machining” that seems the logical way to approach this sort of thing. Rest Machining keeps track of what a particular operation failed to machine so that subsequent operations know where the air is and can avoid cutting it.