to bore or to drill?

Andy221 · Apr 18, 2015

I've had a few jobs at work where the part needed roughly a 5" diameter hole and 5" deep. The material started out as a solid round, one was 1045 (couldn't get the right size seamless fast enough). In both cases my boss told me to to drill up to 2-5/16" then bore. Went from 1/4" to 1" then 2-5/16 then bore.

It seem like it would have been faster to drill to 1" then bore. Drilling a 2-5/16 takes for ever. Or, maybe drill in smaller increments. I was wondering what you guys think would be faster.

Thanks,
Andy

Here's what the parts looked like finished. Thought it might help to see what I was doing.

stonehaven · Apr 18, 2015

Drill then bore is the way I would do it.

BridgeportinD2 · Apr 18, 2015

I'm guessing you were using the engine lathe in the photos, probably no turret.

I would have skipped over the 1/4" and went with a 1/2" or whatever smallest dia. would allow clearance for the web. Blow through with that, then straight to the 2-5/16". I don't think your arm would be any more tired in the end doing it that way vs. running an extra drill through.

Either way, cranking on a tailstock is going to be slow.

If you have the h.p., the holding ability, and a decent sized carbide bar and can roll .5"+ off in a pass then go ahead and bore from a drill size just big enough to get a start for the bar. 350-400 sfm, .012"-.018" feed would make pretty quick work roughing that out.

Again, ya need the horsepower to do it fast.

El Mustachio · Apr 19, 2015

Mount an indexable drill in your QC toolpost, go from Zero to 1.500"+ in one pass half the depth, flip the part, core out the opp. side to meet in the middle, then bore the rest of the way. BTW, make sure the face each side before coring out with the indexable drill. If your lathe has a threading stop on the carriage, use it to set the C/L position for the indexable drill. Oh, & make sure to plumb the drill with coolant.

Standard Helical Flute Drilling Holders | Travers.com

ortho · Apr 19, 2015

stonehaven said:
Drill then bore is the way I would do it.

Water jet or oxyfuel cutting for stock removal?

---Joe

MattIrvine · Apr 19, 2015

We make replacement wheels for William crushers at work, 500 OD 200 ID, 250 bearing seats, they're laid out to centre, spotted then, 12mm pilot, then drilled 80 straight through in a radial drill, then bored.

DMF_TomB · Apr 19, 2015

drill or bore

Andy221 said:
I've had a few jobs at work where the part needed roughly a 5" diameter hole and 5" deep. The material started out as a solid round, one was 1045 (couldn't get the right size seamless fast enough). In both cases my boss told me to to drill up to 2-5/16" then bore. Went from 1/4" to 1" then 2-5/16 then bore.

It seem like it would have been faster to drill to 1" then bore. Drilling a 2-5/16 takes for ever. Or, maybe drill in smaller increments. I was wondering what you guys think would be faster.

Thanks,
Andy

Here's what the parts looked like finished. Thought it might help to see what I was doing.

.
1) i would do as the boss says to do
.
2) you have to hold the part and if it slips in the chuck you might scrap the part
.
3) hp needed might be more than your machine has and as hp used increases cutting force goes higher.
.
4) chips coming off. a drill you can peck drill to break chips, you can vary feed when boring but if feed is maintained and you get long chips forming a mess you have to stop to clear the mess of stringy chips
.
5) tooling cost, depending on drill type it might be cheaper to use a drill than expensive carbide inserts.

Forrest Addy · Apr 19, 2015

Drilling is generally more efficient for stock removal than boring with an HSS tool but if you're willing to max cuts using carbide insert bars you can generally beat converntional twist drilling drilling especially for loger bores. Feeding a 2 5/16 drill is no easy matter even if you have a 2 speed tailstock. Your wrists swell up like grabpefruit. after a day of hand feeding honking big drills in an engin lathe.

I've found drilling in as few steps possible saved far more time than a series of interrmediate steps. 2/3 of the drilling thrust comes from forcing the chisel edge into the work. I usually eyeballed the web and picked a pre-drill about 10% larger then the web size. Drill through with the pre-drill followed by the hogging drill. If you're seeking better concentricity, drill a half diameter deep with a drill 1/16 smaller than the hogging drill then bore to the drill size.

This "pre-bore" guides the hogging drill resulting in a straighter drilled hole and, if the hole is deep, a LOT of PITA boring the hole straighter. I've drilled 3/8" holes 20" deep to meet a cross drill back in the day. The material was cast copper nickel and the hole was to pass filtered water to a water lubed outboard bearing of a main injection by-pass pump. Giving the drilled hole a good start in the right direction pays big dividends in straight holes.

Andy221 · Apr 19, 2015

Thanks for the reply's. The lathe has pretty good power, its a 10hp I believe. I was using a 1-1/4 boring bar carbide if i remember correctly .250 was the max material I could take off at .020 and about 350 sfm. Once boring, it went pretty quick. Maybe if I slow the feed down I could have taken .500 off.

Another thing I need to learn or get better at determining is, at what point does slowing the feed and/or sfm down to remove more material become quicker than higher speeds and feeds and less material?

Here's another pic for your viewing pleasure

DMF_TomB · Apr 19, 2015

feed

Andy221 said:
Thanks for the reply's. The lathe has pretty good power, its a 10hp I believe. I was using a 1-1/4 boring bar carbide if i remember correctly .250 was the max material I could take off at .020 and about 350 sfm. Once boring, it went pretty quick. Maybe if I slow the feed down I could have taken .500 off.

One thing I need to learn is, at what point does slowing the feed and/or sfm down to remove more material become quicker than higher speeds and feeds and less material.

Here's another pic for your viewing pleasure

.
carbide inserts are made for certain feed ranges or inch per tooth. when they stop making short chips and you get long stringy chips it can be a problem. carbide inserts when you reach a certain feed rate the corners break down from too much cutting force. also too much cutting force the boring bar will vibrate which also damages insert
.
also 0.250 depth of cut at .020 feed at 350 sfpm at 2" diameter is about
13.4 inch per min feed and removes 21 cubic inches per minute and with 1018 steel thats about 26 hp and 2475 lbs of cutting force
..... my guess is you were not at .020" feed

WHHJR · Apr 19, 2015

Coolant thru Spade drill as large as HP allows then Bore.

Mcgyver · Apr 19, 2015

drilling will always be the fastest way to remove material, but gawd who wants to crank the tailstock quill for days.

Build a carriage power drilling attachments like this smart folks and Dean Smith and Grace do. Bolts to the carriage dovetail with a stop for centre. It take straight shank MT adapters so you don't have machine the MT and could have it up to 5 or 6 MT if you like. I've big chunk of cast iron waiting to be made into one....#673 on the TDL

Andy221 · Apr 19, 2015

DMF_TomB said:
.
carbide inserts are made for certain feed ranges or inch per tooth. when they stop making short chips and you get long stringy chips it can be a problem. carbide inserts when you reach a certain feed rate the corners break down from too much cutting force. also too much cutting force the boring bar will vibrate which also damages insert
.
also 0.250 depth of cut at .020 feed at 350 sfpm at 2" diameter is about
13.4 inch per min feed and removes 21 cubic inches per minute and with 1018 steel thats about 26 hp and 2475 lbs of cutting force
..... my guess is you were not at .020" feed

The material removed was .250 not depth of cut. Doc was .125. I should have said depth of cut instead of material removed originally.

Mike C. · Apr 19, 2015

If you had some threads in there, it looks like a gland nut for a hydraulic cyl. I make them all the time.

From the chips in that pic, you aren't laying on that tailstock quill very hard. Unless the lathe stalls, you can't crank that tailstock too fast with that drill. You want those curls 1" wide and the spiral to be big around as your thumb. Upping the feed rate actually keeps the drill cooler and makes the edge last longer, since it is buried in cold metal instead of rubbing.

As for the 1/4, 1/2 and then 2 5/16... forget that. If you sharpen the drill with a split point, you can eliminate the pilot drill altogether. A coolmist sprayer pointing down the hole will help, too. Get the hole drilled fast as you can.

Now, on the speed vs depth of cut, I always go with depth of cut. Reason being, you can take a big cut at a lower speed and usually get the chip to break instead of having to fight long snarling curls. Not only are those aggravating, they are extremely dangerous. If you can double depth of cut and double feed rate, you can cut the spindle speed in half and still work twice as fast.

Get the bar up close to the toolpost as possible, while still being able to reach all the way through (I mean leaving 1/4" or less to spare). Set spindle speed to get 200ft/min for mild steel. I'd try to take at least .200 per pass. If the bar squeals, drop the speed to the next available notch and try again. If you can get the squeal eliminated then deal with the chips using feed. Jack up the feed until the chips break short. If the chips just won't break, back the speed down another notch. Last resort, back the depth of cut down and work it out again. Once you get it working, make a mental or literal note of your depth of cut, speed and feed combo so you can go with it next time.

You may have to back speed down as the bore progresses, due to the surface speed increasing as the diameter increases.

Limy Sami · Apr 19, 2015

Mike C. said:
If you had some threads in there, it looks like a gland nut for a hydraulic cyl. I make them all the time.

From the chips in that pic, you aren't laying on that tailstock quill very hard. Unless the lathe stalls, you can't crank that tailstock too fast with that drill. You want those curls 1" wide and the spiral to be big around as your thumb. Upping the feed rate actually keeps the drill cooler and makes the edge last longer, since it is buried in cold metal instead of rubbing.

As for the 1/4, 1/2 and then 2 5/16... forget that. If you sharpen the drill with a split point, you can eliminate the pilot drill altogether. A coolmist sprayer pointing down the hole will help, too. Get the hole drilled fast as you can.

Now, on the speed vs depth of cut, I always go with depth of cut. Reason being, you can take a big cut at a lower speed and usually get the chip to break instead of having to fight long snarling curls. Not only are those aggravating, they are extremely dangerous. If you can double depth of cut and double feed rate, you can cut the spindle speed in half and still work twice as fast.

Get the bar up close to the toolpost as possible, while still being able to reach all the way through (I mean leaving 1/4" or less to spare). Set spindle speed to get 200ft/min for mild steel. I'd try to take at least .200 per pass. If the bar squeals, drop the speed to the next available notch and try again. If you can get the squeal eliminated then deal with the chips using feed. Jack up the feed until the chips break short. If the chips just won't break, back the speed down another notch. Last resort, back the depth of cut down and work it out again. Once you get it working, make a mental or literal note of your depth of cut, speed and feed combo so you can go with it next time.

You may have to back speed down as the bore progresses, due to the surface speed increasing as the diameter increases.

Listen to the man - Mike C knows what he's talking about, and has put it in to words much better than I could.

Keep to the ''old school'' rules, they still apply today, minimum over hangs, sharp tools with correct angles and clearances, making tools work instead of rub - etc etc etc, will get the job done quickly and with minimal problems and messing about.

Andy221 · Apr 19, 2015

Thanks Mike and sami,

the biggest thing holding me back was the drill bit spinning, if I really cranked on it. I used a dog against a 1" piece of square stock in the tool holder to help hold it.

I put a wrench on the nut that holds the tailstock handle on. I slowly put more pressure on the drill and the dog eventually twisted on the drill bit and slipped off the 1" stock. It was loud!

DMF_TomB, are you using unit power or power constant values for your formula?

DMF_TomB · Apr 19, 2015

machinability rating

Andy221 said:
Thanks Mike and sami,

the biggest thing holding me back was the drill bit spinning, if I really cranked on it. I used a dog against a 1" piece of square stock in the tool holder to help hold it.

I put a wrench on the nut that holds the tailstock handle on. I slowly put more pressure on the drill and the dog eventually twisted on the drill bit and slipped off the 1" stock. It was loud!

DMF_TomB, are you using unit power or power constant values for your formula?

.
if 21 cubic inches removed of 1018 steel per minute and using a machinability rating of 0.8 cubic inches per minute per hp thats 26hp. some inserts are more efficient and can remove up to 1.6 cubic inches per hp per minute at higher feed rates so thats 13 hp
depth of cut perhaps not the best term
.
2" dia shaft 0.250 depth of cut is on lathe 0.125 all the way around so 0.25 x 0.020 x 4200 (surface inch per minute or 350 sfpm)= 21 cubic inches per minute
...... my guess is you were not at 13.4 ipm feed as you would have bored hole in about 30 seconds

Andy221 · Apr 19, 2015

There is something else I wanted to say.

Not knowing the proper forum etiquette I did not introduce myself when I first joined.

I've been and electrician since 2002 with a little break in there when I joined the Air Force for 6 years. I got out in 2012 and went back to electrical work. In the mean time I bought a little south bend to do a little gunsmithing, chambering is all really. Through this and some other little projects I really started to enjoy machining.

In January I was able to talk a local machine shop into letting me work part time. By the middle of march I decided machining is what I wanted to do. Electrical work wasn't to bad but, it was more of a means to an end then anything. And in march I decided to work full time at the machine shop.

What I mainly wanted to say is that, I've been having a blast! Its been great learning and getting to do something I enjoy. I also have to add that I'm thankful my boss was willing to take me in and teach me and allow me to learn on his time.

I've been told I'm crazy for giving up electrical work but, I'd rather be happy and enjoy what I'm doing.

The shop I work in is old and little dirty but, I think it is awesome. It was built in the 60's which I think adds to it. We have older machinery and nothing fancy but, we it get done.

On one side is the machine shop and on the other is where all the welders, press, and balancer is. We mainly do repair work or make a new part of something that was broken. I did have to make six bearing housings and a couple other small multi part orders though.

Mike C. · Apr 19, 2015

"the biggest thing holding me back was the drill bit spinning, if I really cranked on it."

Ah! Most good big lathes have MT sockets that also have tang sockets like a radial drill to keep the drill fro spinning. The dog was the proper approach. The last place I worked had a little Leblond that somebody had modified by putting a couple of setscrews in the tailstock quill to grab the MT tang on the drill. Worked extremely well and was one of those things I took note of.

The pilot hole may actually be working against you in this department, as well. The pilot drill is to reduce thrust on the drill by letting the chisel point (web) pass. By not drilling the pilot hole, or at least using a smaller one, you will increase the thrust on the drill, which will push it harder into the tailstock socket, making the MT less likely to slip. I have to use this technique on the little Enco 12" machine at work when drilling over about 1/2". Drilling a pilot hole causes the drill to want to self feed and makes it nearly impossible to keep the drill chuck from spinning. Try it without the pilot and see if it isn't less likely to spin.

You aren't really trying to get a precise hole in this part (another part of the reason for pilot drilling). You just want as large a start hole as possible to proceed with the boring bar. Use a center drill to get a start for the point and then just let her rip.

Andy221 · Apr 19, 2015

DMF_TomB so, I'm not sure I understand you correctly. if I move my tool .125 into the material that is not depth of cut? Just looking for some clarification.

Either way, maybe I have my info mixed up, this job was two months ago. If I was in front of my lathe looking at the dials I would be able to recall.

to bore or to drill?

Cast Iron

Hot Rolled

Hot Rolled

Hot Rolled

Aluminum

Plastic

Diamond

Diamond

Cast Iron

Diamond

Stainless

Diamond

Cast Iron

Diamond

Diamond

Cast Iron

Diamond

Cast Iron

Diamond

Cast Iron

Similar threads