HSS spade drill on engine lathe - how much HP is enough?

Hey all, I have a pretty good set of MT drills for my MT4 15x48 5hp Colchester. I'm considering jumping into the world of spade drills, because I do a lot of hogging solid stock since I can't order heavy wall tube when I need it.

Is there a general rule of thumb for HP needed to drive a spade drill? For example, the auction lot I'm watching has a bunch of big stuff, but I assume that my 5hp will never be enough to drive anything bigger than a 2" spade. Is that number actually smaller, like 1-1/2"?

The usual rule of thumb (OK, "specific power") for metal removal applies to spade drills just as other basic cutters. 1 cubic inch of steel per minute per horsepower. 3 ci/min/HP in aluminum.

I suspect you will run out of thrust before you run out of horsepower. I use a lot of spade drills under 1.5" on a 7.5HP 16x40, occasionally trying a couple up to 2.25", and suspect I am close to the thrust limit on the bigger ones. Fortunately, I only try to drive the bigger ones in aluminum. I use straight shank spade drill toolholders clamped in boring bar toolblocks, rather than MT tangs in the tailstock, so at least I'm not going to torque the quill out of my tailstock.

My advice is to drill a hole just large enough for a stout boring bar, then take aggressive DOC roughing passes with the boring bar.

I don't think that the type of drill, twist or spade makes much difference. the cutting edge is similarly shearing metal. It's all cubic inches per minute.

they seem to think you know your machines efficiency. I might guess 80% motor, 90% mechanical. total of about 70% ?

but if your lathe says 5hp, is that at the chuck or is that the electrical power consumed?

Tooling Pro

dsergison said:

I don't think that the type of drill, twist or spade makes much difference. the cutting edge is similarly shearing metal. It's all cubic inches per minute.

they seem to think you know your machines efficiency. I might guess 80% motor, 90% mechanical. total of about 70% ?

but if your lathe says 5hp, is that at the chuck or is that the electrical power consumed?

Tooling Pro

Click to expand...

All I meant was that it's a 5hp nameplate motor. I'm sure you're right, less is getting to the chuck.

sfriedberg said:

The usual rule of thumb (OK, "specific power") for metal removal applies to spade drills just as other basic cutters. 1 cubic inch of steel per minute per horsepower. 3 ci/min/HP in aluminum.

I suspect you will run out of thrust before you run out of horsepower. I use a lot of spade drills under 1.5" on a 7.5HP 16x40, occasionally trying a couple up to 2.25", and suspect I am close to the thrust limit on the bigger ones. Fortunately, I only try to drive the bigger ones in aluminum. I use straight shank spade drill toolholders clamped in boring bar toolblocks, rather than MT tangs in the tailstock, so at least I'm not going to torque the quill out of my tailstock.

My advice is to drill a hole just large enough for a stout boring bar, then take aggressive DOC roughing passes with the boring bar.

Click to expand...

The "small hole then bore" plan is how I work right now. Except I usually push a pretty big twist drill through, at least an inch, which give me enough room for my beefiest boring bar, then start chewing from there. Maybe the way I'm already working is the best way for my equipment - I just wanted to ask, to make sure I wasn't missing out on something that would be a lot better!

With MT4 and 5HP you can do better than 1” starter and associated boring bar I’d guess, but like has been said I don’t think spade vs twist matters much unless you can run carbide spade with your lathe.

If I had that lathe and was going for quickest large bore I’d start with about 3/8” pilot, using carbide if the lathes max speed exceeded HSS limits for 3/8”. Likely toolpost mounted would be more efficient than TS but up to you. This will greatly reduce thrust required for the large drill but won’t eliminate it for seating the taper. Then I’d go to 1.25” and see how that fairs. If it’s stress free go to 1.5”. In MT4 I wouldn’t push much more than that but run it full SFPM and push as hard as you can. If that works and the motor isn’t stressing when pushed then consider going up in size again and toolpost mounted. But at that point I’d be worried about toolpost strength and twisting. Once you’ve found your drill limit, buy/build a boring bar holder that just fits. You’ll see a drastic difference from a 3/4” or 7/8” bar to a 1.25” bar. If you are boring a lot larger and that bar is limiting you build another larger diameter one.

How deep do you need to bore? making a bar that is supported at both ends can make things stouter and allow deeper cutting.
Bill D.

JCByrd24 said:

Once you’ve found your drill limit, buy/build a boring bar holder that just fits. You’ll see a drastic difference from a 3/4” or 7/8” bar to a 1.25” bar.

Click to expand...

This is absolutely true, and makes a huge difference when trying a deep DOC rough bore.

More important (to me at least) is "How much right shoulder is available ?"
Cranking the tailstock all day against a 2" blade make me cringe.

sfriedberg said:

The usual rule of thumb (OK, "specific power") for metal removal applies to spade drills just as other basic cutters. 1 cubic inch of steel per minute per horsepower. 3 ci/min/HP in aluminum.

I suspect you will run out of thrust before you run out of horsepower. I use a lot of spade drills under 1.5" on a 7.5HP 16x40, occasionally trying a couple up to 2.25", and suspect I am close to the thrust limit on the bigger ones. Fortunately, I only try to drive the bigger ones in aluminum. I use straight shank spade drill toolholders clamped in boring bar toolblocks, rather than MT tangs in the tailstock, so at least I'm not going to torque the quill out of my tailstock.

My advice is to drill a hole just large enough for a stout boring bar, then take aggressive DOC roughing passes with the boring bar.

Click to expand...

.
obviously you can adjust rpm and feed rate if limited hp. or use a pilot spade drill say 1.5" dia before going to a 2.5" drill. yes for 1018 steel figuring 1hp to remove 1 cubic inch per min is roughly correct
.
but besides hp there is cutting force. i once tried hand tapping 1.5" dia a part held in a lathe with head stock locked to prevent rotation. using a 24" crescent wrench i applied enough force the lock pin maybe 0.2" dia in the side of a soft zinc alloy gear just broke free and damaged the hole in side of the gear.
.
at low rpm you can in theory lower hp required but cutting forces can be tremendous like over 1000 lbs easily. sort of like using a 10 ton hydraulic jack. it may not move very fast but still apply many tons of force breaking stuff.
.
if you can not feed the drill cranking the hand wheels with normal force i wouldnt try applying higher than normal feed force. obviously if you damage headstock gearing it will be difficult to repair. some lathes have feed screw shear pins or tailstock clamp may just slip if overloaded. but other lathes stuff just breaks and not easy to repair if overloaded

your lowest force non-boring option would be to use a trepanning cutter. link to making one. YouTube

if your not boring very deep just use a long annular cutter. -from both sides if needed.

JasonPAtkins said:

The "small hole then bore" plan is how I work right now. Except I usually push a pretty big twist drill through, at least an inch, which give me enough room for my beefiest boring bar, then start chewing from there. Maybe the way I'm already working is the best way for my equipment - I just wanted to ask, to make sure I wasn't missing out on something that would be a lot better!

Click to expand...

While I used to follow the rule of "biggest drill, then bore to size"

Realize that your drilling with HSS, and when switching to a boring bar, you can employ inserted carbide
thereby increasing the SFM greatly.

I too have a nice 1" min. inserted boring bar, and will drill only large enough to get that bar in there, sometimes the first cut of the bar might be .250 on a side (radius) and will have to decrease the feed somewhat to keep the chatter down.

But once I get that bar thru the first cut, look out.

When power feeding I always liked to try & break chips with spade drills which generally needed feeds of .0075” or more per flute → per revolution. I much preferred a tool block on the cross slide to an aloris style toolholder on the compound if I had multiples to drill. Cranking drills (much) with the tailstock sucks rocks.

For drill end thrust I put this up a while back.



Good luck,
Matt

As Digger Doug said, your shoulder suffers if you drive from the tailstock all day. Many years ago I would chain the saddle to the tailstock and use that for power feed. Now I use a QCTP with either a Morse socket or a chuck. The nice thing is you can set up the lathe for a very slow feed that would probably drive you nuts if you were feeding with the tailstock. The other nice thing about power feed is that you can do something else while the old boy is drilling away. You just have to make sure to clear the chips where appropriate from time to time. Spade drills work good in this "unattended" condition because they clear the chips nicely.

crossthread said:

Many years ago I would chain the saddle to the tailstock and use that for power feed.

Click to expand...

OH! I plumb forgot about that...

Matt

Thanks for your expertise, everyone. I hear the consensus that whether spade or twist probably doesn't really matter, but to "get to boring as quickly as you can."

That's helpful, thanks. I guess the two advantages I still see for spade drills (for my application) are that I can get a couple of thru-coolant spade holders and be able to drill a lot of different sizes with coolant, rather than replacing my whole set of MT twist drills to do the same thing. The other thing I like about spade (for my location) is how much lighter a replacement spade insert is than a replacement MT drill of the same size.

However, I don't think either of those are important enough to justify the cost, since I already have the twist drills and boring bars.

I think my "go to" boring bar is a 1" x 12" Kennametal VBMT. It's steel, but is pretty stable. I think I may have a 1-1/4" in my box somewhere, but the Kennametal has been pretty tough, so I haven't gone looking for it. I also have a 3/8" heavy metal Ultradex and a medium (maybe 5/8"?) thru-coolant carbide Ultradex, which I LOVE.

I do understand the "exhausted right shoulder" problem! I have a big boring bar holder and an MT4 holder for my Dorian CXA post. I've tried drilling with the toolpost in the past, but it didn't seem that much easier to me - maybe it was just inexperience setting it up? It seemed like the time to get the drill straight and on center, and get the feed selected, was not faster than the tailstock for one or two parts, drilling from solid up to 1.25" in 2 steps. Maybe I just need to practice more? Or maybe it's only worth it if you have more than a few parts to run? When I did get it set up, the carriage "stopped out" (what do we call that? like when the carriage feed hits the stop, it disengages) easily, too, I had to keep pressing the feed engagement lever back in, the drilling pressure was enough to trip it out. Maybe it would be less prone to do that if it were on the leadscrew like if you were threading, vs being on the feed rod like I was doing? I think if I could fix that problem, with a little practice I'd get faster setting it up, and it would be worth drilling from the saddle.

My lathe does have a shear pin between the headstock and the first, smallest gear in the change gears, so I don't think I need to worry about breaking anything. That shear pin is just 1/8" aluminum (from a welding rod I had around), so I think it'd shear pretty easily. When I bought the lathe, the previous owner (anyone used to work at Florida Power and Light in Miami?) had replaced that shear pin with a hardened roll pin - the ensuing crash is the reason the half nut snapped and I still can't thread on the machine! All of that happened before I got it, but now that the pin is aluminum (I think Colchester spec'd regular mild steel), I'm not worried about overstressing the feed gear system.

JasonPAtkins said:

Hey all, I have a pretty good set of MT drills for my MT4 15x48 5hp Colchester. I'm considering jumping into the world of spade drills, because I do a lot of hogging solid stock since I can't order heavy wall tube when I need it.

Is there a general rule of thumb for HP needed to drive a spade drill? For example, the auction lot I'm watching has a bunch of big stuff, but I assume that my 5hp will never be enough to drive anything bigger than a 2" spade. Is that number actually smaller, like 1-1/2"?

Click to expand...

LOVED the idea that I could custom-grind a specific diameter.

However... fageddabouddit. An Allied Machine Exec was on PM a while back.

He was kind enough to evaluate what my drillpress could expect. About 1 1/4", and I'd HAVE to add high pressure coolant, reliable supply, plenty OF it. Allied has videos as show the how, why, and what, spades can do. Awesome. But neither you nor I NEED it.

Oh, BTW..

Said weak-kneed DP is around 4,400 Avoir and 7 HP worth of early 1950's Alzmettal AB5/S, PIV-Werner-Reimers and geared-head drive, power downfeed. Veritable T-Rex of column drills. EAT the average lathe with push-away tailstock, and many others, even with carriage-drilling.

It can do THREE inches in CI with an ignorant helical twist-drill, all-day, every-day, all-year, year after year.

Just not as fast per hole as an Allied Spade in Warp-speed overdrive.

There are other, slower, but helical-beater types of inserted drills as do not need as much power, push, nor slippy-juice as spades do.

Where you are going to be? Old Skewl helicals can be sharpened by a determined hand. A skill in demand, "basic" economy countries - and one all-hands should learn.

Inserts? Not so much. And then you run out.

Has anyone adapted a Bridgeport (aftermarket servo style) power feed (maybe the knee model) to cranking the tailstock ?

digger doug said:

Has anyone adapted a Bridgeport (aftermarket servo style) power feed (maybe the knee model) to cranking the tailstock ?

Click to expand...

Easier to start from scratch. Been done. Even "right here on PM", powered compounds as well, IIRC.

Hydraulic feed is not uncommon, OEM. Nor hard to shop-fab.

WTH? Close-on a hundred years of that by now? Rockford became Sundstrand off the back of hydraulic carriages, cross, TS, turrets, et al as far back as the 1920's did it not?

Not likely to see that on the average SB nine, though! Nor even a light-medium Colchester.

Though one COULD do, drilling with the carriage is just cheaper and easier to add, given power feed and rapid hand-retract to clear chip is already "there".

Just not "there enough" to push spades at their best effectiveness.

By the time one gets enough "push" the next issue is the torque overwhelming the paltry 5 HP spindle and stalling it.

You up for pushing serious spade, you want 25 to 50 hoss on the motor data-plate and a powered-second carriage on the hoss itself, names like "Warner & Swasey" on that data-plate.

Seriously. Ask Allied. Full-gallop or get TF outta the pool with spade drilling.

My experience is that a spade drill requires a lot more thrust than a twist drill.

I've got a 3" thru coolant twist drill that I've run quite a bit in my 40 hp cnc Okuma for roughing holes and it just buzzes right along at a .025 ipr feedrate.

Also have an Allied spade with a few various blades that I've run in my 4A Warner and Swasey.

Had a job a while back for a few parts with the smallest part of the bore going out to almost 5", so I figured I'd run the spade in the Okuma with a new 3 1/2" blade. Z axis load meter runs a bit less than 50% with the 3" twist in 1144, so since this is 1117 I should be fine with the 3.5" spade at about the same .025 feed.

In reality, anything more than a .008 IPR feed would kick out the axis drive overload. First thought was something wrong with the lathe, but couldn't see anything unusual. Pulled the spade and put the 3" twist in. No other changes except for resetting the Z offset. Twist drill hums right along under 50% as always.