PDA

View Full Version : I didn't know drilling holes was so difficult.



Tommo
11-01-2012, 10:18 AM
I've never given it much thought, but apparently that's my problem! What are any tips/tricks to drilling a long hole and keeping the bit from wandering? I tried drilling a 1/4" hole in a piece of steel chucked into the lathe, the hole was about 2" long. Looked great at one end, one end only.
I understand some bits wander moreso than others, also using a pilot bit and increasing the size incrementally works well but I'm only looking to drill a .25" hole.

Fasttrack
11-01-2012, 10:50 AM
0.25" hole 2" deep is pretty tricky business. The two most important things I can think of are the following:

1) Use a high quality, properly ground bit. If it isn't ground just "dead nuts" symmetrical, it will drift. You'll want to check, with a drill gauge, even quality bits.

2) Peck drill - drill a little at a time backing the drill all the way out often, clearing the swarf. Also, use a good lubricant to make sure that chips flow and don't weld to the cutting edges/flutes

EDIT: In a lathe, you should also make sure that the tailstock is, in fact, on the center line of the lathe/work. If it is low, high, crooked, or offset then the drill will drift. Also, I suggest starting with a spot drill (not a center drill - they're two different things!) to make sure the bit doesn't wander initially.

mars-red
11-01-2012, 10:57 AM
I always start with a center or spotting drill, chucked up real close in the tailstock. From there I drill in incremental sizes (for most of the stuff I do, 0.25" is not very small so I would take 3 or 4 steps to get to that diameter), and for particularly long holes like this one you're talking about, for each drill size, I start with the drill chucked in as far as possible, and drill / re-chuck out further until I have the full depth. I recently had to make a WW drawbar for my watchmakers lathe, it is several inches long with a 0.25" thru-hole. I used this technique for it and it worked quite well. If you're curious, I have a couple of pics of it here: https://picasaweb.google.com/115933926156798442633/WWDrawbar#
I was using junk hardware store steel so forgive the poor finish. :-/

You could also play around with reversing the work in conjunction with some of the above steps. If you have an independent 4 jaw chuck or good collets you may even be able to drill undersize from each end, then use a small boring bar from each end to get the final diameter.

EDIT: Fasttrack and I posted at the same time - I agree with everything he says, I completely forgot to mention tailstock alignment. Critical, for sure.

Ian B
11-01-2012, 11:04 AM
+1 to Fasttrack's suggestions.

Also, make sure the drill starts true - tailstock barrel in line with the headstock, pilot indent drilled concentric with the axis of rotation.

Ian

Black_Moons
11-01-2012, 11:56 AM
I use my center drill, making sure the flutes are horzontal as I think my tailstick is out more horzontal then vertical

I feed the center drill in slightly, lock the tailstock, wait for chips to stop appearing, unlock tailstock and feed in a little more, lock tailstock, repeat.

Once that is done I switch to a real drill bit, It does not have much choice but to follow start of the hole, and as the center drill was basicly used as a boring bar when I lock the tailstock, its guarenteed on center.

If you start DEAD on center, your drillbit wanders MUCH less. (of course it also helps to have the tailstock dead center too). Do not expect that just pushing a drill bit into the end of stock will drill anywhere close to where you expect, the drill will wander and skate before it catchs, if even just a few thou, thats all it takes.

wierdscience
11-01-2012, 01:01 PM
I don't use the tail stock at all,too many things can be worn/out of tolerance.

Instead I mount a block in the tool post,chuck a center drill in the lathe chuck,center and drill a hole in it to accept the bit I will use to drill the workpiece and use the carriage instead of the tail stock.This method does the best job of averaging for spindle run out and the rack and pinion of the carriage makes the job go faster I find.

Take your time,let the bit do the work.Combined with what Fasttrack said about having a well ground quality drill I have managed 1/4" holes greater than 8" deep that deviated less than .003" off center.

firbikrhd1
11-01-2012, 01:10 PM
D Bits are an option. Here is some info from the PM site:
http://www.practicalmachinist.com/vb/general/d-bits-154906/

More info: http://www.metalwebnews.com/howto/d-bit.html

And an article from Popular Science: http://books.google.com/books?id=1SoDAAAAMBAJ&pg=PA172&lpg=PA172&dq=d+bit&source=bl&ots=pzAUjREU17&sig=Skl2U5ajQqiMt9IqLPgglFxwtYI&hl=en&sa=X&ei=056SUICVA6a50AHYvIHABw&ved=0CCIQ6AEwATgU#v=onepage&q=d%20bit&f=false

Boucher
11-01-2012, 01:14 PM
To make a custom spotting drill holder for your lathe, Start with a drill chuck shank with the appropriate taper to fit your tailstock. Make an orientation index mark so you can reinstall it in the same direction each time. Install a center cutting mill cutter in the headstock and apply a light-facing cut. Next install a spotting drill in the headstock. Turn the speed up and peck a spotting hole. Next use a quality stub drill to drill a 3/4" depth hole the size of your spotting drill. Clean the socket and install a spotting drill using red loctite. Now make another holder for a center cutting end mill.

To start a hole straight and centered flatten the surface with the end mill then use the spotting drill holder to get a good starting socket. It is important to increase the speed appropriate to the small diameter of the end of the drill and to peck with a consistent feed rate. Use the best cutting fluid you have (probably a tapping fluid like Castrol Moly-D)

Mike Amick
11-01-2012, 01:21 PM
Instead I mount a block in the tool post,chuck a center drill in the lathe chuck,center and drill a hole in it to accept the bit I will use to drill the workpiece and use the carriage instead of the tail stock.


That's a pretty neat idea. How do you hold the drill in the block then ?
Some type of set screw or what ?

Fasttrack
11-01-2012, 01:29 PM
I use my center drill, making sure the flutes are horzontal as I think my tailstick is out more horzontal then vertical

I feed the center drill in slightly, lock the tailstock, wait for chips to stop appearing, unlock tailstock and feed in a little more, lock tailstock, repeat.


That's a great trick for worn out or otherwise problematic tailstocks. Combined with what Wierdscience posted, you have a really good shot at drilling a deep hole without drifting. When I was working with my little Smithy lathe, I noticed the tailstock wasn't true with the center line so I'd use a broken center bit ground like a mini, fluted boring bar to get a shallow socket started. Then I had a 5C collet block holding a drill chuck clamped to the table/carriage. Using a spotting drill and the eyeball method, I could get the drill chuck centered properly. Switch to my drill bit and I'm off to the races. I had pretty good success drilling 1" holes 6" deep. Not quite the same as a 1/4" hole 3" deep, but my main motivation was using the power feed ;) Not as elegant as Wierdscience's solution (and thus more prone to problems!).

lugnut
11-01-2012, 01:35 PM
You might take a look at the 2012 Nov./Dec. issue of Home shop Machinist, where Santro Di Filippo is talking about the very subject.
Just a thought
Mel

wierdscience
11-01-2012, 03:20 PM
That's a pretty neat idea. How do you hold the drill in the block then ?
Some type of set screw or what ?

Yup,setscrew.On my list of roundtoits is a purpose made toolholder fitted with a small ER collet chuck,but sadly it's way down on the list.

Jaakko Fagerlund
11-01-2012, 04:51 PM
Whatever you do, DON'T use a center drill to start your hole! It is not meant for starting holes, it is meant for making centers and drilling in to a center drilled spot can/will break your drills lips.

Rich Carlstedt
11-01-2012, 07:04 PM
Go to the 'Sticky- favorite threads" on the main page.
Look for deep hole drilling 101 for hints

Rich

brian Rupnow
11-01-2012, 09:26 PM
Okay---Somebody educate me!!!! I have ALWAYS used a center drill for starting holes in stock which gets drilled in my lathe. Perhaps I have always been doing it wrong. Can somebody post a bit of information about, or a link to these "spotting" drills please.---Brian

Boucher
11-01-2012, 10:08 PM
http://www.use-enco.com/CGI/INSRIT?PMAKA=325-2143
Your ENCO catalog has some information at the beginning of this section

rohart
11-01-2012, 10:34 PM
I bought a couple of carbide spotting drills. They couldn't cope with anything other that nice clean faced mild steel. They broke within a week.

I replaced them with HSS, and these have been going for over a year, into cold rolled, hot rolled, black oxide coated, rough sawn, you name it.

As for the original task, I just hit the work with a spotter, an 1/8th, a 1/4 and go from there. I can get five inches out of a 5/32 long series drill I have, and expect reasonable results.

My tip is to go slowly in the first inch or so when you go up to the next size of drill. You want to make as much use as you can of the rigidity of the drill. If the hole with the smaller drill had drifted off a tad then this gives the next size drill a chance of cutting assymetrically, and bringing the hole back on centre.

Be ruthless about drills that wander off. Chuck them in the 'to be reground' bin. This includes new drills that cause trouble.

There are only two ways to get a true hole on the lathe. One is to drill several pieces of work and choose the one that's within limits. The other is to bore. I see no reason why you can't bore out a 6mm hole to 1/4" between centres with a 5.8mm boring bar with a 1/8" HSS insert fixed/glued/welded in the middle.

wierdscience
11-01-2012, 10:50 PM
Center drill vs spotting drills,for starting either will work,if using a center drill just use the tip of it and don't drill a complete center.Having a quality drill is important however,I prefer KEO brand above the rest.Quality steel,accurate grind,will last for years.
http://keocutters.com/search/drilldown/?categories=2040

The drill bit is another source of potential problems.Don't assume that your brand new even from a quality MFG drill bit is perfectly straight.I have seen offenders from all MFG over the years.

I typically chuck the drill in the lathe chuck and give it a spin.If the tip runs out more than a couple thou it gets turned around in the chuck and the shank machined true.

tyrone shewlaces
11-01-2012, 10:55 PM
I don't know about Jaakko's stern notion to never use a center drill for starting holes. I did it for my first few years and it worked OK. However, he is true about saying that they aren't meant for starting holes but rather to make a relieved 60 center. For a long, long time now I've been using 90 spotting drills and it works better for me. Not a big deal, but I just do what I like best.

I understand rohart's problems with the carbide ones and unless you need it to be carbide due to hard material or whatever, then I'd recommend HSS too. Mine last about a year and maybe closer to two, and I do this for a living and probably use one or two of mine (different sizes) at least a couple times a day, sometimes a couple dozen. The last production shop I worked, the owner always used a 90 spotting drill as a chamfer mill on the CNC mills to chamfer edges after milling. It worked great too - tons less deburring and better looking parts. And even there those darn things lasted a pretty long time (HSS).

As for drills drifting off-center, my experience with that is 1) to peck often and use lube as Fasttrack recommended and 2) don't push too hard. I used to run turret lathes and we were drilling 3/16" and 1/8" oil holes down into pins about 8" deep all the time. We didn't use any special drill bit other than they were long ones. But if you tried to get more work done by pushing harder, then by golly they would drift way off center every time. If you don't push too hard and just let the drill do most of the work, then the natural tendancy of the drill to find its own center in a lathe will work like it's supposed to and you'll have a pretty decent hole.

edit to add: I just remembered that when we drilled those deep holes, we would progress from a stub length drill to jobber drill then longer drills until we got to the depth we needed. Maybe after spotting, start with a stub drill to go as far as it will go, then finish with a jobber. The shorter drills are more rigid so resist drifting more than the longer ones. Using this progression of short-to-longer drill bits works very well.

PixMan
11-01-2012, 10:57 PM
+1 to using spot drills. I do this, and when I do I spot to LESS than the diameter of the drill to be used. This way it centers the next drill and the tips of it aren't the first thing to get sucked into the work and chip. I also use parabolic flute split-point style drills, as they need far less chip clearing and cut with less force.

Here's a few I picked up off Ebay for about $15 with a bunch of others. These are Guhring, but I like Titex just as well.
http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/Guhring_parabolics.jpg

These are some of the Titex spotting drills I picked up from Ebay. They have thinner webs than any other make:
http://img.photobucket.com/albums/v466/kenm10759/Dads%20shop/042311193349.jpg

Paul Alciatore
11-02-2012, 01:25 AM
I have been machining for at least 45 years at one level or another. In that time I have only broken ONE center and it was from a set that I inherited from my grandfather so it was probably a good 40 years old at the time when it broke.

I have used both center drills and spotting drills for starting holes and both do work. I have never broken a standard jobbers drill after starting a hole with a center drill. I do go easy on them, specially when starting them in the hole. Most of the drills I have broken were in a hand drilling operation and I suspect you can blame the angle that I held the drill at. Oh, I did break a carbide drill once, but it hit a diamond hard inclusion in the steel. Perhaps it is a diamond. I don't know: I had to scrap that part after three drills were dulled or broken in that hole. Small drills are more likely to break from being dull.

All that being said, it is probably better to use spotting drills to start holes and leave the center drills for drilling holes for centers.

oldtiffie
11-02-2012, 01:40 AM
http://www.youtube.com/watch?v=bh4L65V1SqQ

brian Rupnow
11-02-2012, 09:53 AM
Thanks for showing me the difference between center drills and spotting drills.---Brian

Wirecutter
11-02-2012, 02:06 PM
Whatever you do, DON'T use a center drill to start your hole! It is not meant for starting holes, it is meant for making centers and drilling in to a center drilled spot can/will break your drills lips.

DOH! I've been using a center drill to start holes for years. It's worked pretty well in Al, stainless, brass, copper, and whatever else I have lying around. Guess I'll have to get some spotting drills now.

This reminds me of the post I wrote when I first joined here asking about the use of an edge finder. I truly didn't know how those things worked. Boy was I educated...

Forestgnome
11-02-2012, 04:04 PM
+1 on the parabolic drills. The are quite a bit stiffer for long drills due to the thicker web, plus the benefit of better chip evacuation. Like others said, start it in the center using a center or spotting drill, don't use too much force (it bends the bit into a curve and redirects the tip), clear the swarf often (swarf buildup can occur on oneside and push the tip of center), and aas you peck it helps to approach the bottom lightly so the tip can get a fresh start each time. Currently I'm running a job drilling 2" deep holes .132" diameter, and the hole needs to be concentric to .001" all the way through. I found just pushing on the unclamped tailstock with my hand vs. using the handcrank improved concentricity on the other end, plus it speeds up cleaning out swarf.

Rich Carlstedt
11-02-2012, 05:32 PM
Whatever you do, DON'T use a center drill to start your hole! It is not meant for starting holes, it is meant for making centers and drilling in to a center drilled spot can/will break your drills lips.

Right on Jaakko !

A "center" drill is exactly that, a drill for using ( Lathe) centers.
Many of us fall into habits, that does not make them right, nor does it necessarily address the issue

For starting normal holes, use a starting drill.
But the question from the poster was about drilling long ( deep) holes !
Centerdrills will not allow this achievement with accuracy.
Drilling a deep hole as the requester desired, requires a different approach, and centerdrills or starting drills will not cut it.
You must use a ball endmill and go to 1/2 the flute pitch for depth. Then you will have accuracy, and support for deep hole drilling with a two flute drill bit.
Read the sticky "Favorite Threads" for further understanding of this important approach in machining

Rich

PixMan
11-03-2012, 10:00 AM
<snip>

Drilling a deep hole as the requester desired, requires a different approach, and centerdrills or starting drills will not cut it.
You must use a ball endmill and go to 1/2 the flute pitch for depth. Then you will have accuracy, and support for deep hole drilling with a two flute drill bit.
Read the sticky "Favorite Threads" for further understanding of this important approach in machining

Rich

Must use? The only occasions that I've used a ball end mill to locate a hole has been when I'm tying to start a hole on an angled surface. That's an application for when the technique works quite well.

I have used 90 and 120 spot drills to locate holes of varying depths for a long time, quite successfully. If I am worried about chipping the tips of a drill (such as with solid carbide drills), I spot to a diameter just over the web thickness of the drill to be used. This allows the lip of the drill to bear the chipload first so the tips don't hog in and fracture. Using a simple 90 spot drill to locate, I made a 6.5mm hole through a 14" long motorcycle axle made from 316 stainless steel. I did have to go halfway from each end and it was a lot of pecks with the Titex A1622-6.5 drill at a slow speed, but the holes met in the middle well enough that a 1/4" pin fell right through. It was just a weight reduction hole on a non-rotating part so it wasn't critical, but it came out very nice just the same.

Forestgnome
11-03-2012, 11:20 AM
What hasn't been said is that a center drill's stiffness and flute configuration basically makes it a boring tool if slightly off-center, thereby making the hole perfectly centered. That's why I use them to start holes in a lathe. Otherwise I'ld just pull out a teeny boring bar to start.

Jaakko Fagerlund
11-03-2012, 02:47 PM
What hasn't been said is that a center drill's stiffness and flute configuration basically makes it a boring tool if slightly off-center, thereby making the hole perfectly centered. That's why I use them to start holes in a lathe. Otherwise I'ld just pull out a teeny boring bar to start.
That same thing also makes it possible to make a nice hole in the end of workpiece that has a little nub in the center, as the center drill just goes round and round.

If one uses a spotting drill (120 degrees), the only place a drill can go and start its hole is in the center of that divot, as drills are generally 118 degrees.

JoeCB
11-03-2012, 03:23 PM
One of the trickest drilling operations in the automotive engine business are crankshaft oil holes, typically 1/4 " and 6 inches deep... on a angle thru nodular iron or forged steel. "crankshaft drills" are 1/4 " X 12 inches long. The key feature is a "split point" grind. The point is ground in two facets such that there is zero web thickness at the tip. The objective is to minimize the thrust load on the drill, reducing the tendency to bend. I think that the split point also makes for smaller more manageable chips. The drill is run in a "pecking" mode, of course all automatic in a production operation. Entry into the angled surface is guided by a close fitting drill bushing.
Joe B