Boring Pre-game

[dogma]

I made my first serious attempt at boring last week on a supremely under-powered and insufficiently rigid lathe. It took ~4 hours (yes, hours of listening to a belt slipping) to bore out a ~1.75" ID / 1" depth in 1018 (and I over ran my tolerance, so I get to make it again...).

I started the initial bore with a #5 center drill, went full depth with a 17/64th split point (my 1/4th gets a lot of use), and then a 1/2 split point before changing over to ccmt insert boring bars. After all of this, someone pointed out that it would have been much faster to hog out the bulk of the ID using a mill by plunge cutting or using a rotary table. In my pathological lathe case, this certainly would have been the case as the mill I have access two has substantively more power.

However, I'm curious as to what would be the correct stock "preparation" if a mill and lathe had equal power. (I'm ignoring the obvious solution of starting from precision tube stock). The linear speed (SFM) starts at effectively zero on the axis of rotation and increases as the ID enlarges. Is twist drill faster than a boring on a small ID do to the have two cutting edges instead of one? Thus, an end mill with 4 or more flutes will hog out faster due to the addition surfaces. If that is true, does it make sense to use center cutting end mills in the tail stock over something like a deming drill? Is there an ID size at which a single edge boring has an advantage?

 

[mzayd3]

I think you have it right using a drill as opposed to an end mill in the tail stock. More flutes in an end mill is intended more for faster feed when milling, not while plunging. More flutes, each taking equal depths of cut equals faster longitudinal travel with the same spindle speed. An advantage of boring over drilling is more precise, straight, true holes. A drill can walk and produce a larger sized hole when done.

You did it right, this is a perfect operation for a lathe with drills in the tail stock and a boring bar.

 

[Ed ke6bnl]

I been hearing a lot about using annular drill that drill and pull out a plug for getting started, I have one 9/16 ready to try but will have to change out my chuck in the tail stock to a bigger on to hold the annular cutter.

 

[Wreck™Wreck]

You appear to be boring through, use a 1 5/8" drill and bang it straight through after spotting a center, no pilot drill. This will leave .06" per side for finishing which is more then enough.
1.5" depth of drill at .004" per revolution feed (1.5 / .004 = 375 revolutions of the spindle) at 40 RPMs this will take just over 8 minutes per part, you will not have to peck drill as the diameter is larger then the depth. Since it is a shallow through hole choose the largest boring bar that will clear the hole as chip packing will not be a problem.
Rough bore, with inserted carbide tooling at 1000 to 2000 RPMs at .008-.010 feed and .025 DOC, finish at .005 or so feed at .005-.008 Doc depending on material and tooling.

I realize that you probably do not have a 1 5/8" drill nor the the power to plow it through a piece of 1 1/2" mild steel, however the finish boring OP's remain the same.

Good Luck

 

[JimDawson]

Generally drilling is the most efficient material removal method. Plunge cutting with an end mill is not the best idea, even a center cutting one, unless you have first drilled a large-ish pilot hole. There are exceptions to this like when plunging and cutting less than 30% of the end mill diameter. In this case I would drill through with the largest drill you have, then bore to finish.

 

[Jimsehr]

What Lathe and horsepower?
jimsehr