# Center drilling in steps or 1 pass?



## Jmanb13 (Apr 24, 2017)

I just wanted to know if there is a best practice for drilling on a lathe.

I know to start with a center drill to get the hole started. After that should I just chuck up the bit size I want and go to town or should I start with a smaller bit and then size up in steps?

Also, my assumption is that drill bits are more of a "close" but not perfect size hole? If I wanted a perfect hole I would use a reaming tool correct?


----------



## Silverbullet (Apr 24, 2017)

A lot depends on the material , the tolerances , the power of the lathe. Ive always used the step on holes larger then 1/2" , even then its up to the material . If it cuts easy , let chips break often live chips cut grab and hurt. Ive cut big holes in materials with big machines capable to turn 2" drills and bigger , but it was to be bored bigger so if it wasnt straight it didnt mater. In my shop I always step up beyond the 1/2 " hole. If reaming I always step drill the hole. Your drill bits will work easier and last longer too. Less resharpening  even.


----------



## DAT510 (Apr 24, 2017)

For me... I step drill.  Starting with a center drill.  I had been taught by an old machinist, that each of the drills should be slightly larger than the width of the chisel point of the next large drill you will be using in the step.    So, for example: if my final bit is a 1/2" drill.  I look at the width of the chisel point and pick the next smaller bit so that it's diameter is slightly large than the width of the chisel point on the 1/2" drill.    For a 1/2" hole, I'd personally do it in at least two steps depending on material (Center Drill, Intermediate Drill, 1/2" Drill).  

If the accuracy of the ID needs to be close, I drill it close and then ream to final size.

If Concentricity is important, I drill, then bore, and possibly ream (if the ID is reasonable for me to ream)

Hope this helps.


----------



## David S (Apr 24, 2017)

Not too much to add to the advice already given.  I may depend on your machine power.  I don't own many reamers so usually drill close then bore to final dimension.

If you haven't seen the thread on the discussion of centre drills vs spotting drills for ...well starting.  For 30 years I have been using a centre drill to spot for starting drill bits.  And often noticed that one flute would catch and drill a bit off.  Based on the information in this thread I ordered some spotting drills, and have immediately noticed an improvement.  Now a lot of my work is drilling holes well under Ø 0.25".

http://www.hobby-machinist.com/thre...-with-center-drills-vs-spotting-drills.57023/

David


----------



## wildo (Apr 24, 2017)

David S said:


> http://www.hobby-machinist.com/thre...-with-center-drills-vs-spotting-drills.57023/
> 
> David



Was also going to link to this thread. Lots of good info there.


----------



## T Bredehoft (Apr 24, 2017)

I, too, am impressed with a spotting drill. Its cut is broad enough to let the center of the drill bit start the cut rather than the flutes which occasionally will catch and start the hole off center.


----------



## Doubleeboy (Apr 24, 2017)

Found out about spotting drills about 15 years ago.  Since then the only use I have for center drills is for setting up to turn between centers.  Couple licks with a diamond hone and a spotting drill is good as new.  I have a few different sizes but the cobalt 1/4" does most the work.


----------



## David S (Apr 24, 2017)

Jmanb13, I didn't mean to redirect your thread by mentioning a spotting drill.  If you have any other questions to get back on track, please ask.

David


----------



## mikey (Apr 24, 2017)

Jmanb13 said:


> I just wanted to know if there is a best practice for drilling on a lathe.
> 
> I know to start with a center drill to get the hole started. After that should I just chuck up the bit size I want and go to town or should I start with a smaller bit and then size up in steps?
> 
> Also, my assumption is that drill bits are more of a "close" but not perfect size hole? If I wanted a perfect hole I would use a reaming tool correct?



The guys have given you excellent advice - start with a spotting drill if you can and if you need to drill a large hole then using a pilot drill that is sized to span the web of the main drill helps. It helps because the center of a drill does not cut; it locates the drill but it requires more pressure to move it through the cut and the pilot obviates this need. 

The problem with using pilot drills is that they tend to be small drills that must also be pushed through the cut and the pressure tends to bend them and make those small drills wander. This will lead the main drill that follows to follow the same wandering path. For this reason, if you need an accurately placed hole it is often better to spot and follow with the main drill. You will also find the main drill will also produce a more accurately sized hole because it is larger, stiffer and is also not bouncing around inside the hole.

All drills deflect, even large ones. To minimize deflection, use enough pressure for them to continuously cut but no more than that. A properly sharpened drill will output equal sized curled chips from both flutes and you should see these chips continuously moving. If they stop moving, raise the drill and clear the chips. When you go back in, use more pressure initially to get the drill past the work hardened surface and then watch for the chip flow. With large drills, slow the speed way down and increase feed pressure to keep chip production going. This maximizes the cutting action and minimizes heat production. Done well, a 1/2" drill will only feel slightly warm immediately after the cut. 

If you need an accurately sized hole or a hole with a good finish then reaming will do that. However, it may not be a straight hole. Reamers follow the hole so if the drill produced a wandering hole then the reamer will produce an accurately sized and finely finished wandering hole. If you need an accurate, straight and properly sized hole with a fine finish then you should drill the hole, bore it straight and then ream it. The problem is that quite often we do not have the right sized reamer, in which case the only option to get an accurate hole is to bore it.

Keep in mind that drills are like all cutting tools - if they chatter, slow down the speed and increase the feed. Since both flutes must cut, both flutes must be sharpened identically. Unless you are good at drill grinding by hand, buy a Drill Doctor or some other machine/jig to aid you.

Making a hole is easy. Making a straight hole is a bit harder. Making a straight accurate hole with a fine finish is much harder. And then you have to make sure its located in the right place! Fun, isn't it?


----------



## Jmanb13 (Apr 24, 2017)

David S said:


> Not too much to add to the advice already given.  I may depend on your machine power.  I don't own many reamers so usually drill close then bore to final dimension.
> 
> If you haven't seen the thread on the discussion of centre drills vs spotting drills for ...well starting.  For 30 years I have been using a centre drill to spot for starting drill bits.  And often noticed that one flute would catch and drill a bit off.  Based on the information in this thread I ordered some spotting drills, and have immediately noticed an improvement.  Now a lot of my work is drilling holes well under Ø 0.25".
> 
> ...





David S said:


> Jmanb13, I didn't mean to redirect your thread by mentioning a spotting drill.  If you have any other questions to get back on track, please ask.
> 
> David



Thanks for the tip! And no worries about redirecting the thread. Finding out there is a totally different way to do something is just as good as learning how to do it the same way. It is funny because I ran across that thread through the "similar threads" at the bottom right after I posted this one  Guess the forum is working well.

I've also noticed while i'm drilling that it seems 1 flute sends out a nice long curl while the other one is hardly doing anything. Just a few small chips here and there.

I'll definitely look into the spotting drills.


----------



## Bob Korves (Apr 28, 2017)

Jmanb13 said:


> I've also noticed while i'm drilling that it seems 1 flute sends out a nice long curl while the other one is hardly doing anything. Just a few small chips here and there.


That means the drill is not ground correctly.


----------



## Wreck™Wreck (Apr 28, 2017)

Use the biggest drill that the machine will drive, spade drills are excellent for large rough holes when your goal is to remove the maximum amount of material in the shortest possible time followed by a finishing operation. 

Spade drills seem to work best without a pilot hole, spot and go leaving generous room for finishing, for example, for a  3 1/4" bore I would rough with a 3" drill straight through. As mentioned this requires a machine capable of doing so.

As a side note, if needing a 3" hole 6" through a blank and the machine already has a 2" drill set up I use that because I'm lazy that way, changing tools may take far longer the the actual drilling of a single part. A 2 1/2" X 6" deep hole through 304 stainless should take 15-30 minutes each or so, changing drills would take longer. Remember that 15 Minutes times 50 parts is 12 1/2 hours or roughly  $1500.00 in machine time or more.


----------



## mikey (Apr 28, 2017)

Okay, wait ... drilling a 3" ID hole ... most of us are lucky to drill a 1" hole on our machines but a 3" hole on a home shop machine is, well, heroic.


----------



## kd4gij (Apr 28, 2017)

At work drilling a 3" hole in one shot, piece of cake. At  home not so much.

Now for bronze, plastic and aluminum I never step drill at home. Made that mistake once.


----------



## Tony Wells (Apr 28, 2017)

I used to spend days pushing a 3 1/4" drill through a piece of some sort of stainless just to rough the part out for the CNC lathes finishing the parts. Some threaded jack tube for a big jet landing gear as I recall. The tubes were nearly 2 feet long. Two things happen. You learn to sharpen big drills, and you get strong arms. Orders for 50-100 at a time used to come in. I was wishing for a spade drill, but never happened in that shop. One lathe the operator ruined the nut in the tailstock on our Colchester pushing it so hard.....but he was using a cheater bar in the wheel. He never learned when or how to sharpen the drill. So much for the "good old days". Those I don't miss, even a little bit.

I might add a small tip on drilling to help stay straight. Once you get about 1 diameter deep with a slightly smaller drill, bore the hole to close fit the next drill size. It will drill much straighter on the next step.  I'm one of the guys who never step it up though, other than that, if I have to drill close to finish size. If the piece is short, and the hole is undersized to the point that the hole needn't be all that true, I just punch a "dirty hole". Drills generally are the most efficient method of material removal for ID work. There are all sorts of things to help keep the hole from drifting, but that's another day, another thread.


----------



## jlsmithseven (Apr 28, 2017)

I just found out this. We had to drill close to a 1 inch drill inside our piece. First I started with a #5 center drill. Then I went to like a 1/2" drill. Then I moved up to the 1 inch drill. I can honestly tell you it was a breeze cutting the rest of the material inside. Once I hit the wall where I stopped with the .500 it was a lot harder to cut. Using the .500 was easy too. I fully believe in stepping up in drill sizes is a good idea and practice..puts less wear on the drill bit too I would think..


----------



## tq60 (Apr 29, 2017)

We were taught in shop class to step drill but not proper stepping.

For sheet stock the step drills do well but back to big drills.
Center drill with the largest one yiu have with tail stock or spindle as retracted as possible to get a good start.

Look at the Web in the center of the bit.

That is the diameter of the drill to use as a pilot.

Your limit is the pressure you can apply and hp of your machine. 

Final size should be via a boring bar 

Sent from my SAMSUNG-SGH-I337Z using Tapatalk


----------



## Wreck™Wreck (Apr 29, 2017)

mikey said:


> Okay, wait ... drilling a 3" ID hole ... most of us are lucky to drill a 1" hole on our machines but a 3" hole on a home shop machine is, well, heroic.


I began with "the biggest drill that the machine will drive" fully understanding that one is limited by the equipment at hand. 

Merely wanted to point out that drilling in steps is not required if drilling to size in one shot is possible, this saves a good deal of time.


----------



## joshua43214 (May 28, 2017)

I am not a huge fan of step drilling, and minimize it as much as possible.
Step drilling chowders the heck out of conventional drills. You can actually buy special drills meant for step drilling.
Start with a spotting drill, then push the biggest drill that your machine can handle into it.
If you don't have spotting drills, use only the very tip of a center drill - do not use the larger diameter meant for registering a center. Use the biggest center drill you have, followed by the largest drill whose web fits into the spot.
Then push the next largest drill your machine can handle through that hole.
The largest drill your machine can handle is close 2x to the maximum depth of cut you can make while turning. If your lathe can cut 0.250" doc, it can handle a 1/2" drill. In theory, it can go right from a 1/2" to a 1" drill, but this is actually limited by the rigidity of the tail stock.

If your pilot hole drifted (it did), then all the following drills will follow that drift + what ever drift they impart from uneven sharpening. in other words, the more drills you run down the hole, the worse the hole gets. To make matters worse, the more you use a drill for step drilling, the worse that drill dill perform as the cutting edges deteriorate unevenly.

The fact is that a drilled hole is not round, on size, or concentric.
You have to consider where you are going with the drilling operation. Are you going to run a tap through a 1" hole? Not likely unless you are a pro. For most of us large hole drilling is to make space for a boring bar, or single point threading.

All that said, there are plenty of lathes that cant drill a 1/2" hole in steel. Same rules apply, biggest drill you can use, followed by the next biggest. Worth considering drilling 1/64" undersize then making a finish pass onsize for taping stuff in the 1/2" size range.


----------



## benmychree (Jul 3, 2017)

DAT510 said:


> For me... I step drill.  Starting with a center drill.  I had been taught by an old machinist, that each of the drills should be slightly larger than the width of the chisel point of the next large drill you will be using in the step.    So, for example: if my final bit is a 1/2" drill.  I look at the width of the chisel point and pick the next smaller bit so that it's diameter is slightly large than the width of the chisel point on the 1/2" drill.    For a 1/2" hole, I'd personally do it in at least two steps depending on material (Center Drill, Intermediate Drill, 1/2" Drill).
> 
> If the accuracy of the ID needs to be close, I drill it close and then ream to final size.
> 
> ...


What you say is the best practice if one has a machine capable of doing it in terms of power and ridgidity; If one drills holes using sizes of drills that do not use the whole cutting edge, it invites wobbling of the drill and out of round holes


----------



## samthedog (Jul 4, 2017)

Don't go cheap on your drill bits. A decent set of drills or buying packets of singles from a reputable manufacturer is a worthy investment, as is decent cutting fluid. Having well ground drills with proper symmetry goes a long way to keeping the hole straight and the bit cutting. Also pay attention to your feed and speed. Most people I see spool up their machine far too fast for large drill bits and usually too slow on smaller drill bits.


----------

