PDA

View Full Version : Spotting Drill Lesson Needed



firbikrhd1
01-23-2016, 10:50 PM
In another recent thread there was talk about using a spotting drill to start drilled hole and obtain more accurate placement. There was also some discussion about the use of a spotting drill vs a center drill. I have always used a center drill, carefully, to prevent breakage of the smaller drill point, however I can see the advantages of the use of s spotting drill, plus, it's just the proper way to do things. So, I looked up spotting drills and learned that they come with different angles on the point. MSC has them in 50, 82, 90, 118, 120 and 142 degrees.
So, why the different angles and when is the preferred use of each?

Obviously the 60 degree could be used for centering and the 82 degree could be used for countersinking and if I understand correctly 90 degree for countersinking metric screws, but these are spotting drills, not countersinks. I suppose 118 degree spotting drills are used because they match the drill point angle of some drill bits although some bits are 135/138 degrees and none of the spotting drills mentioned have that angle.

So, what's the deal and what is a good spotting drill to use before you drill?

gellfex
01-23-2016, 11:12 PM
And while a seminar is requested, how about the use of piloting vs spotting. With larger drills I often pilot with a drill slightly smaller than the web of the bigger drill. I have no idea if this is common.

RussZHC
01-24-2016, 12:04 AM
http://www.guhring.com/Documents/Catalog/Drills/NCSpotDrills.pdf solves the 142* part for me.
I was under the impression you wanted the angle a bit flatter (bigger?) than the final drill angle but find it curious that some knowledgeable folks over on PM quoting various sources that you would hope would actually know, engineers and manufacturers and such (hate when the wrong thing is recommended by someone who is supposed to know, that is why I ask them...) some of whom take opposite views regarding the larger or smaller included angle of the spot drill relative to the finish drill.

As an aside, IIRC several go to sources (oft quoted books) recommend that you not use a center drill for anything other than establishing those for turning on a lathe...does one assume it is because of the danger of breaking off the much smaller tip? If that is the reason, would not just taking some care be in order?

PStechPaul
01-24-2016, 12:55 AM
The idea, AIUI, is that the 90 degree included angle allows the 118 to 135 degree bits to ride on and cut with the well-formed cutting edges and not the chisel point at the center on the web. In the machine shop class I took last year, the instructor recommended using a center drill, probably because they were more readily available in the shop.

Paul Alciatore
01-24-2016, 01:24 AM
Oh boy! This is one of THOSE subjects. Who's making the popcorn? I like it buttered please.


LET THE GAMES BEGIN!

KiddZimaHater
01-24-2016, 01:41 AM
I don't know why there are so many different angles for spot drills.
I guess there's an application for each one.
I only use a 118 Spot drill, since all of the drills I use are standard 118 drills.
And, I only use center drills for making centers in the lathe, or for spotting for small diameter drills (I hate snapping off the little tips)

Also, in reply to gelfex, I always make a pilot hole, the size of the drill web, if I'm using any drill over 3/4".
Pilot holes make drilling ALOT easier, and more accurate.

Jaakko Fagerlund
01-24-2016, 04:42 AM
Oh boy! This is one of THOSE subjects. Who's making the popcorn? I like it buttered please.


LET THE GAMES BEGIN!
You forgot the beer :)


Pilot holes make drilling ALOT easier, and more accurate.
Um, no. The smaller bit can easily wander off as it flexes more and the bigger drill will follow that hole you made. There is something wrong with the drill sharpening if larger drills require a starting hole (not counting for the issue of having undersized machine here). Usual hand sharpening gives freely going action on a 40 mm drill and what I've used factory ground bits, the biggest is 76 mm and also can be hand fed to steel easily. With proper grinding the chisel is next to nothing and cuts almost perfectly.

As for the different angles for spotting drills, the 82 and 90 degree ones are so called quick cheating tools, as you can just drill a starter hole and get a nice chamfering at the edge if you drill it deep it enough for the following drill. Used very often in CNC applications when doing production runs.

The 120 degree is the one to use for the basic 118 degree sharpened drills, as it allos the drill to center itself in the divot, even if it is teeny tiny bit off from the center. The 142 degree one is meant for drills sharpened to 135 degree, though I've rarely seen them.

If you make a center hole and start drilling, it's the drills lips that contact first, taking easily a bigger bite, and thus not guaranteeing a proper location as the drill can flex wherever it wants to.

LKeithR
01-24-2016, 05:05 AM
...Um, no. The smaller bit can easily wander off as it flexes more and the bigger drill will follow that hole you made. There is something wrong with the drill sharpening if larger drills require a starting hole (not counting for the issue of having undersized machine here). Usual hand sharpening gives freely going action on a 40 mm drill and what I've used factory ground bits, the biggest is 76 mm and also can be hand fed to steel easily. With proper grinding the chisel is next to nothing and cuts almost perfectly...

Meanwhile, in the world where most of us operate, drilling a pilot hole for a larger drill is perfectly normal procedure--absolutely nothing wrong with it. A 40mm drill is about 1-9/16"--my biggest is about 1-3/4" and I can tell you that pushing it into a piece of solid steel without a pilot hole is not easy. Anyone who does this a lot should know that a drill is not an accurate cutting tool; it just makes a hole. For a quick and dirty repair requiring a spacer or bushing or sleeve a drilled hole is often all I need--if I need something more accurate I'll drill under-size and bore to finish.

If you've got a big machine with lots of power pushing a big drill without a pilot is relatively easy--with a smaller machine not so much. Your example of a 76mm drill tells me you've got a pretty good sized lathe--I'll be that not 1 in 1000 people on this site have a drill that size...

Carm
01-24-2016, 09:16 AM
"So, what's the deal and what is a good spotting drill to use before you drill? "

Heh. As I said in the other thread, there is argument over these things. Always something to learn, which is why I brought it up. There is no definitive answer...many opinions come from shops that earn their keep making holes the way they do because that's what works for them.
My own background in hole making involved getting the most accurate placement & size with the least amount of steps. For dead accurate repetitive work nothing beats a jig plate w/bushings.
(You CNC guys lighten up- all manual pre DRO here)

Let's rule out using combo/centre drills, yes of course they work.
The arguments over angles concern how well the following drill intersects the previous divot. A broad angle divot with a narrower angle follow will intersect the centre first. Vice versa, the outer lips. Carbide drills don't like that.
The "ideal" would be matching angles. Weren't many to choose from in days gone by.

Regardless your view on that, best practice (for me) is short stout spotter, split point screw machine drill, then a jobber if depth is needed.

Like Keith says, a drill is a crude but efficient tool. True centre sharpening is best for accuracy expectations.

vpt
01-24-2016, 10:01 AM
Why not a small endmill to start a hole?

Rosco-P
01-24-2016, 10:13 AM
Why not a small endmill to start a hole?

How are you going to hit a punch mark or layout lines with tooling that has a nearly flat bottom? For the OP, he'd be depending on his DRO which seems to have questionable dependability.

Jaakko Fagerlund
01-24-2016, 10:33 AM
A 40mm drill is about 1-9/16"--my biggest is about 1-3/4" and I can tell you that pushing it into a piece of solid steel without a pilot hole is not easy.
If the tool is properly sharpened (i.e. not having that chisel end on it), it will cut very easily, with less heat produced and thus for longer. When you drill holes day in and day out on various machines you really learn what sort of sharpening works and what doesn't work. The best and easiest by far is a 4 facet sharpening (provides a self centering end) and the chisel point edges ground to cut with the edge of a grinding wheel.

My example of a 76 mm drll cutting easily is just an example that a proper sharpening on a tool makes it a lot easier on you, the tool and the machine, no matter what size they are. Heck, if you jump to U-drills (carbide inserts), they cut with even less power.

dalee100
01-24-2016, 11:12 AM
Hi,

A small end mill will tend to wander when plunged and produce an oval hole.

As far as spot drills vs. center drills. To me it doesn't matter, I use what ever is handy at the moment.

Spotting drills did not become popular until CNC became common. They became popular because they are much stronger than center drills and allow increases in feed rates, (think on the order of 10ipm vs 2ipm rates). Which in turn, decreases cycle times because seconds matter on long part runs. Oddly enough, that also makes them widely available in tool catalogs. So HSM'ers can get easy access to them.

Back in the day, center drills where what was commonly available to everyone. And they worked fine as a dual purpose tool. They not only made center spots for lathe centers, but could also do spotting work for drills and do combo drill and countersinks on thin materials. A very versatile tool all together. Center drills still excel at those things today.

Which angle to get? Depends on what you might need to do. For general spotting drills, I like 90deg. Not only does that give a good general use spot, I also tend to spot drill deep enough to leave a chamfer of the size I want after drilling the hole. This works well whether I'm programming turning centers or machining centers, it saves a lot of cycle time. A center drill would be a more fragile tool if I did that. Other angles can provide other advantages, like counter sinking for screws. It all depends on what you think you want the tool to do.

I think that for the average HSM, it really doesn't matter all that much. Use what you've already got or buy a spot drill if it will make you happy. A HSM'er often has more time than money, so a more versatile tool like the center drill might be a cheaper choice. But if using a spot drill makes you happy, go for it. 3 billion Chinese won't care.

Dalee

Paul Alciatore
01-24-2016, 11:23 AM
A word of caution here about terminology. In drill sharpening circles a four facet tip usually refers to adding additional clearance to a two facet tip. This would still have the standard wedge at the web. I think what you are talking about is a split point grind which provides cutting action to the center and a center point that helps to stop wandering.

Pass the popcorn, please.




If the tool is properly sharpened (i.e. not having that chisel end on it), it will cut very easily, with less heat produced and thus for longer. When you drill holes day in and day out on various machines you really learn what sort of sharpening works and what doesn't work. The best and easiest by far is a 4 facet sharpening (provides a self centering end) and the chisel point edges ground to cut with the edge of a grinding wheel.

My example of a 76 mm drll cutting easily is just an example that a proper sharpening on a tool makes it a lot easier on you, the tool and the machine, no matter what size they are. Heck, if you jump to U-drills (carbide inserts), they cut with even less power.

Rustybolt
01-24-2016, 11:26 AM
Spotting drills did not become popular until CNC became common.

Not so. They were used on the screw machine induatry many decades before CNC cme along.


If you're going to be drilling deep holes with a narrow drill the point angle of the spotting drill should be the same angle as the drill. It is easier for the drill to find center that way.

dian
01-24-2016, 11:38 AM
If the tool is properly sharpened (i.e. not having that chisel end on it), it will cut very easily, with less heat produced and thus for longer. When you drill holes day in and day out on various machines you really learn what sort of sharpening works and what doesn't work. The best and easiest by far is a 4 facet sharpening (provides a self centering end) and the chisel point edges ground to cut with the edge of a grinding wheel.

My example of a 76 mm drll cutting easily is just an example that a proper sharpening on a tool makes it a lot easier on you, the tool and the machine, no matter what size they are. Heck, if you jump to U-drills (carbide inserts), they cut with even less power.

jaakko, i completely agree. but can you tell me why its impossible to buy four faceted drills? well, im sure you can somewhere, but my supplier didnt carry any when i last looked.

Forestgnome
01-24-2016, 11:38 AM
Prick punch, punch, pilot drill, drill. That will give you the most accurate hole location in the home shop. I always use a 1/8" for the pilot since it's relatively stiff, and I peck drill with that. If the final hole is 1/8" or smaller, I don't use a pilot. If you need a hole more accurate than that you need a jig borer. The whole discussion of chipped edges is really only relevant to production work. Otherwise you would never want to use a pilot hole, step drill, or enlarge a hole. When my drills chip, I sharpen them. Big deal.

Mcgyver
01-24-2016, 11:39 AM
I agree with Paul, its a split point grind that reduces the downward force substantially. I'll do four facet grinds or hand sharpening, but don't put a split point on, for example. imo the need for pilot hole is a "depends". We sometimes drill holes several inches in diameter, even on a 5' radial drill, you reach a size where it you need a pilot. I'll often do a pilot hole on smaller work just because its easier - depends on equipment, ability to grind, and whether you're racing the clock or messing about on the weekend.

On spot drills. Don't over think it, just buy the 118's.....99% of it is dropping the 60 degree cone centre drill for one close to the drill....whether its a degree or two off the drill point just does not matter All you need is the point close to the angle of the drill and the drill will then start without jumping about. btw, you can use a large centre drill as a spot drill - just use the very end, the 118 degree point :)

dian
01-24-2016, 11:41 AM
Hi,

A small end mill will tend to wander when plunged and produce an oval hole.

As far as spot drills vs. center drills. To me it doesn't matter, I use what ever is handy at the moment.

Spotting drills did not become popular until CNC became common. They became popular because they are much stronger than center drills and allow increases in feed rates, (think on the order of 10ipm vs 2ipm rates). Which in turn, decreases cycle times because seconds matter on long part runs. Oddly enough, that also makes them widely available in tool catalogs. So HSM'ers can get easy access to them.

Back in the day, center drills where what was commonly available to everyone. And they worked fine as a dual purpose tool. They not only made center spots for lathe centers, but could also do spotting work for drills and do combo drill and countersinks on thin materials. A very versatile tool all together. Center drills still excel at those things today.

Which angle to get? Depends on what you might need to do. For general spotting drills, I like 90deg. Not only does that give a good general use spot, I also tend to spot drill deep enough to leave a chamfer of the size I want after drilling the hole. This works well whether I'm programming turning centers or machining centers, it saves a lot of cycle time. A center drill would be a more fragile tool if I did that. Other angles can provide other advantages, like counter sinking for screws. It all depends on what you think you want the tool to do.

I think that for the average HSM, it really doesn't matter all that much. Use what you've already got or buy a spot drill if it will make you happy. A HSM'er often has more time than money, so a more versatile tool like the center drill might be a cheaper choice. But if using a spot drill makes you happy, go for it. 3 billion Chinese won't care.

Dalee

please explain how an endmill can wander. lathe or mill? my endmills produce holes that are accurate enough for dowel pins.

dalee100
01-24-2016, 12:21 PM
Hi,

"Not so. They were used on the screw machine induatry many decades before CNC cme along."

Screw machines are/were pretty special machines and tend to use specific tooling. And like CNC, ran pretty much automatically for long production runs. Not really common on most shop floors. In a shop full of turret and engine lathes, vertical, and horizontal mills, drill presses and radial drills, center drills would have been far more commonly used.

"please explain how an endmill can wander. lathe or mill? my endmills produce holes that are accurate enough for dowel pins."

Just because you can press something into a hole, doesn't mean the hole is round or accurately placed. Try that when you need to place that dowel pin +/-.0002". Or try spotting on a round surface.

Dalee

rkepler
01-24-2016, 12:54 PM
Prick punch, punch, pilot drill, drill. That will give you the most accurate hole location in the home shop. I always use a 1/8" for the pilot since it's relatively stiff, and I peck drill with that. If the final hole is 1/8" or smaller, I don't use a pilot. If you need a hole more accurate than that you need a jig borer. The whole discussion of chipped edges is really only relevant to production work. Otherwise you would never want to use a pilot hole, step drill, or enlarge a hole. When my drills chip, I sharpen them. Big deal.

I think that's for hand work. If I'm drilling in my mill I tend to spot drill (replacing the prick punch and punch cycle) to keep the drill point from wandering then to drill to size immediately with a split point drill. If it's really casual (like a clearanced bolt hole) I might just drill with the shortest split-point drill I can get in there - I have a complete set of screw machine drills just for that. Once the drill is up to jobber there's a fair chance that even a split point is going to wander some.

If I want a hole in absolutely the right place I spot drill, drill under, bore to locate the hole and then drill or ream (reaming when I really care about the hole size). Usually if I really care about the placement I really care about the size.

I once had to make some plates with .1250" holes all accurately placed relative to the plate and one-another, accurate to about .0002" each lengthwith and maybe the same or better overall. Something like 48 holes per plate. Came out good checking on the surface plate so I did OK, but doing that was jig work and not really easy on a mill even with a good DRO.

If the surface you're drilling into isn't square to the hole and clean you're going to have to spot drill with something. If it's really screwy (like the side of a cylinder) you're usually want to pop a flat for the spot drill with an endmill first. You can punch the hole with the endmill if you have to, but a drill is usually more efficient at material removal then an endmill (on a per-unit time and dollar basis). Advantage of using an endmill is that they're usually really, really short, disadvantage is that they cost a lot more than a drill.

Sorry, got more windy here than I expected.

vpt
01-24-2016, 01:01 PM
How are you going to hit a punch mark or layout lines with tooling that has a nearly flat bottom? For the OP, he'd be depending on his DRO which seems to have questionable dependability.

Ballnose. :)


Hi,

A small end mill will tend to wander when plunged and produce an oval hole.


Dalee


If that is happening something else must be moving. I don't think endmills 'wander' much. :D

dian
01-24-2016, 02:21 PM
Hi,

"Not so. They were used on the screw machine induatry many decades before CNC cme along."

Screw machines are/were pretty special machines and tend to use specific tooling. And like CNC, ran pretty much automatically for long production runs. Not really common on most shop floors. In a shop full of turret and engine lathes, vertical, and horizontal mills, drill presses and radial drills, center drills would have been far more commonly used.

"please explain how an endmill can wander. lathe or mill? my endmills produce holes that are accurate enough for dowel pins."

Just because you can press something into a hole, doesn't mean the hole is round or accurately placed. Try that when you need to place that dowel pin +/-.0002". Or try spotting on a round surface.

Dalee

o.k., 0.0002 beats me. no way i can do that, not with the equipment i have.

J Tiers
01-24-2016, 02:30 PM
jaako is, of course, right.

But the common drills including spotting drills, usually have a thicker web, noot thinned, and not 4 or 6 facet ground. They need the hole or there is a lot of force required.

Faceted grinds sure are nice!


o.k., 0.0002 beats me. no way i can do that, not with the equipment i have.

I think that's jig grinder territory. Just use your SIP!

dalee100
01-24-2016, 05:28 PM
Hi,

It can be done on a wimp-wristed, pantywasted, wet noodle Bridgie. It just takes a lot of extra effort and time mixed with a tiny bit of luck. Back in the day, I repaired a few stamping dies with nothing more. As it was all I had to work with. Not a good way to make a living and I don't recommend it.

End mills make poor drills. They are not only amazingly bendy, (particularly a tiny size like you might use for spotting), but they also like cutting on the flutes as much as the end. Which can lead to headaches and grief quite quickly. It's generally not considered good practice.

If you really wish to elimenate spot drilling, short solid carbide drills are the bomb. I often omit spotting if I can use a solid carbide drill. But at $25+ depending on size, they ain't cheap. Nor readily sharpened at home.

Dalee

old mart
01-24-2016, 05:45 PM
I have three spotting drills, 6,8 and 10mm, 90 degree tips, their advantage is the stiffness and the fine point. I treat them with care as I would not be able to sharpen them. Centre drills can be used but there is a much wider minimum mark made. I use 60 degree centre drills on the lathe for use with a centre and 95 degree centre drills if I'm drilling the workpiece. I found out about spotting drills on this forum and am glad I bought some.

Mcgyver
01-24-2016, 07:03 PM
I have three spotting drills, 6,8 and 10mm, 90 degree tips, their advantage is the stiffness and the fine point. .

try some 118's...you might like them more. The conical start made is close to the drill bits angle so drill bits start without chattering or digging in on top edge...than imo is the advantage of a spot drill

gellfex
01-24-2016, 07:04 PM
Wow, this thread is as cool as I hoped! So far I learned that maybe I should get a set of split point 1-60 screw machine drills if I want to be as accurate as possible without spotting. Or maybe see how well my Drill Dr does them, as they claim to. I often drill soft material as small as #36 or even 43 indexing on the mill with no spotting and my stuff usually fits together.

Jaakko Fagerlund
01-24-2016, 11:56 PM
A word of caution here about terminology. In drill sharpening circles a four facet tip usually refers to adding additional clearance to a two facet tip. This would still have the standard wedge at the web. I think what you are talking about is a split point grind which provides cutting action to the center and a center point that helps to stop wandering.
Yes, that's what a four facet sharpening is (just as I explained), it produces pretty standard web but also makes it self-centering. But split-pointing it after that or 'notching' the web area provides more easily cutting tool.

becksmachine
01-25-2016, 12:57 AM
You forgot the beer :)
Um, no. The smaller bit can easily wander off as it flexes more and the bigger drill will follow that hole you made. There is something wrong with the drill sharpening if larger drills require a starting hole (not counting for the issue of having undersized machine here). Usual hand sharpening gives freely going action on a 40 mm drill and what I've used factory ground bits, the biggest is 76 mm and also can be hand fed to steel easily. With proper grinding the chisel is next to nothing and cuts almost perfectly.


Dang it Jaakko, how do you expect me to maintain my competitive edge in business if you keep giving away all my/our secrets?

:)

Dave

old mart
01-25-2016, 05:28 PM
I may get some 118 spot drills when I can afford it. Another good thing about spot drills is the stiffness allows you to get started on a surface which is not square to the hole axis, most drills would have trouble there.

vpt
01-25-2016, 08:25 PM
Ballnose. :)




If that is happening something else must be moving. I don't think endmills 'wander' much. :D

I am shocked no one jumped on this one. After reading it I realized how general and wrong this sounds. Size matters!

Tundra Twin Track
01-26-2016, 01:01 AM
Meanwhile, in the world where most of us operate, drilling a pilot hole for a larger drill is perfectly normal procedure--absolutely nothing wrong with it. A 40mm drill is about 1-9/16"--my biggest is about 1-3/4" and I can tell you that pushing it into a piece of solid steel without a pilot hole is not easy. Anyone who does this a lot should know that a drill is not an accurate cutting tool; it just makes a hole. For a quick and dirty repair requiring a spacer or bushing or sleeve a drilled hole is often all I need--if I need something more accurate I'll drill under-size and bore to finish.

If you've got a big machine with lots of power pushing a big drill without a pilot is relatively easy--with a smaller machine not so much. Your example of a 76mm drill tells me you've got a pretty good sized lathe--I'll be that not 1 in 1000 people on this site have a drill that size...
Hey LKeith I usually drill pilot hole when drilling large holes,2-1/8" biggest I have that use in lathe mostly but have 4 to 1 reduction on Tailstock.In 1to1 position they are a brute to push but with reduction real easy.

Carm
01-26-2016, 08:33 AM
I am shocked no one jumped on this one. After reading it I realized how general and wrong this sounds. Size matters!

Mebbe context. A ball end mill is another trick in the hat.

Paul Alciatore
01-26-2016, 02:36 PM
Jaakko, grinding the third and fourth facets is not what makes it self centering. It is the angle on the cutting edges that does that. Thus, a 90 degree, a 118 degree, a 135 degree, etc. point drill will all self center regardless of how many facets they have (2, 4, or even 6). The factor here is the tip angle is less than 180 degrees. A drill bit with a conical tip will also be self centering if it has a tip angle that is less than 180 degrees. An end cutting end mill will not be self centering because the tip angle is 180 degrees or slightly more and it will not be self centering: it will tend to walk. You could not use an end mill in a hand held drill.

The split point can be added to other grinds, usually a two facet or a conical grind, and it does three things. First, because it has a true point at the tip, it does a better job of initially locating the hole on a punch mark. Second, it will wander less while starting because it cuts from the first contact instead of just pushing metal aside. And third, it will require less downward force while drilling because it is actually cutting the web area of the hole instead of just pushing the metal aside like a wedge center will. I like split point drills for all of the above reasons. I have a set of split points from 1/16" to 1/2" and would like to get some in the number sizes too.

Additional note: I have never seen a split point on a four facet drill. They may exist, but I have never seen it. The point splitting facets function much like the more traditional third and fourth facets of a four facet grind in that they also add additional clearance. So, it is usually not necessary to do a four facet grind before adding the split point. This, perhaps creates an area of confusion in the terminology.

Perhaps I should have said that the split point does four things above, not just three.




Yes, that's what a four facet sharpening is (just as I explained), it produces pretty standard web but also makes it self-centering. But split-pointing it after that or 'notching' the web area provides more easily cutting tool.

Mark Rand
01-26-2016, 07:38 PM
Most people seem to consider that a 'four facet' grind is a planar primary relief on both flutes and a planar secondary relief on both flutes, unlike your 'four facets per flute' grind. If one were to create more facets, than two per flute it were better to use a continuous/conical grind.

This leads to a grand total of four facets. The point is automatically split, since the primary relief planes of the two flutes meet at the centre.

PS. The chisel point in a normal conical grind is there for a reason, it's to limit self feeding of the drill. Thinning/splitting the chisel point reduces the axial force needed, but taken to it's ultimate conclusion can lead to a large drill that will overload the motor or self destruct due to 'biting off more than it can chew'! Not that I've ever done either/both of those things. :o

I could do with some popcorn at this point. :)

Mcgyver
01-26-2016, 08:18 PM
This leads to a grand total of four facets. The point is automatically split, since the primary relief planes of the two flutes meet at the centre.


don't know that I agree with that based on as I know them to be.....here's a split point

http://i20.photobucket.com/albums/b201/michael0100/Drills/drilltip.jpg (http://s20.photobucket.com/user/michael0100/media/Drills/drilltip.jpg.html)


here's a four facet grind. this with my homemade rig, but my christian drill grinder puts the same point on. I never bother with a split point as you need to grind into the angle, ie the "L" that splits the point

http://i20.photobucket.com/albums/b201/michael0100/universal%20swivel/pt2sharpeneddrills.jpg (http://s20.photobucket.com/user/michael0100/media/universal%20swivel/pt2sharpeneddrills.jpg.html)

6061billet
01-27-2016, 12:56 AM
You asked for a lesson, so here you go.

Since center drills, spotting drills and screw machine drill bits come up so often I decided to post a summary for any beginners that stumble across this post in the future. Some may never have seen a center drill before.
In the picture below are some of the most common drill bit types. There are other types like Silver & Deming, Insert drills, etc. but 99% of hole making in a home shop is done with these.

The red line is roughly how deep the drill bits are usually chucked. #1 is the topic of the post but I'll cover it last.
http://i593.photobucket.com/albums/tt20/6061billet1/Drill%20Types/Center_Spot_Screw_Jobber_zps0u43fdkw.jpg (http://s593.photobucket.com/user/6061billet1/media/Drill%20Types/Center_Spot_Screw_Jobber_zps0u43fdkw.jpg.html)

All of these will drill a hole (except for the spotting drill!!!) and with proper technique all can get a hole reasonably positioned. Picking the most effective technique often depends on the type machine you are using and how much time you have.

A novice could mark some hole positions with a Sharpie marker, slap any of these in a worn out drill press, crank the quill down and get holes somewhat close to where they intended to go. Some would wander more than others. A skilled machinist could take that same sloppy drill press, resharpen a jobber drill, scribe, prick, punch, predrill, then finish drill and get a hole accurately placed. There is a big time difference between these two approaches and the hole is still a drilled hole. So it could still be off by a thousandths or so and might not be round or straight. Drills are really roughing tools that can remove metal fast. If you wanted a perfect hole you would need to follow up with a boring head to get the position and possibly ream then lap it.

For most of us a good screw machine drill, some careful layout and lots of practice will cover 99% of our needs. If you are lucky enough to have a small CNC mill however there are some advantages to spotting drills.


#2 is a common center drill: Some people think that it's meant to create a "center spot" for the following drill. The thick stubby body looks like it's meant to stiffen up the drill to prevent wander and that delicate center tip looks perfect for picking up a punch mark or scribed line. In reality this short stubby drill is meant to be used in the tail stock of a lathe to drill the center hole for LIVE CENTER or DEAD CENTER to run in. Hence the name "Center Drill". The broad angle on the center drill matches the angle on the lathe center and that small tip on the drill is to create a deeper clearance hole so the tip of the lathe center doesn't bottom out. You don't want the side forces from the lathe on a fine tip. The drill is extra short because it increases the length of stock you can get in the lathe, it's more rigid, it's less material cost, and you don't really need to drill a very deep hole. The tip on these is very fragile and aside from stiffness they don't have a lot of upsides.

#4 and #5 are typical jobber drills: They are long, floppy, cheap and will drill a reasonably deep hole but don't expect them to put the hole anywhere near where you intended if you just yank the quill down. Their length to diameter is often around 16 to 1. They need a center punch, starting spot drilled or a pilot hole to get any reasonable accuracy. A standard grind has a large blunt chisel edge on the tip that likes to wander everywhere. This is one of the reasons that you often see a recommendation to drill a pilot hole then work up in several passes. The small starter drill has a smaller chisel point and is easier to force through the work. Then chisel point of your next larger drill is cutting air as you feed it in. Think of these drills like corncob roughing endmills. Split point, bullet point, faceted grinds all work to eliminate that chisel edge so the drill starts easier, wanders less, and takes less effort to feed. They are all a huge improvement over a standard grind but a punch is still needed to be sure the drill starts on position.

#3 is a screw machine drill. It's half as long as a jobber drill which makes it 4x as stiff, the tip is closer to the chuck with reduces runout and it's a shorter lever arm which puts less side force on your floppy drill press. All good things... Now if you have good tight milling machine and some way to locate the hole without scribed lines then these can start a hole on location without all of the manual steps of scribing and punching. So they are an improvement in your drill press, they are much nicer to use in your manual bridgeport but they still don't save a ton of time. On the other hand if you have a big expensive CNC machining center your profit and loss depends on number of holes per minute that you can achieve. The CNC mill has nearly zero runout and it can slam these drills down faster than you can react and still get some good tolerance holes. They still might wander a little bit but holes are roughing operations and we are talking about a few thousandths or so. Even on a small home CNC mill there is a world of difference between screw machine drills and jobber drills.

#5 Finally, our spotting drill: (or conical depression implement) It looks like the others, it's got flutes, so it must drill holes... wrong... It's also not some floppy counter sink with a reduced shank and multiple flutes.
http://www.guhring.com/Documents/Catalog/Drills/NCSpotDrills.pdf
Spotting drills are specialized tools that work really well for certain purposes. In your old worn out drill press they probably aren't going to work any better than a center drill or screw machine drill but they will cost 4x to 10x as much. Spotting drills are really the next evolution of a screw machine drill. If you have a bunch of hole to drill on a CNC mill and the tolerances aren't too tight then you just knock them all out with a screw machine drill. But, if you need the positional tolerance a bit better, the edges chamfered, or they need to be counter sunk then you bring in a BIG spotting drill. Odds are that all of your screw holes are either metric or SAE. So one 1/2" spotting drill can spot, chamfer, and countersink all of your holes without even changing tools. Spotting drills are insanely stiff. The flutes usually only extend for 1/4 revolution to 3/4 revolution and they have a long solid shank. They are stiffer than an endmill because more material is left in the shank and they often have less stickout (length from the collet ) and more in the collet than the jobber drills. They are also ground to much tighter tolerances than a drill and can have razor sharp edges. Manufacturers often recommend that you never use a spotting drill in a drill chuck. Collets and shrink fit holders are preferred. All of this leads up the next big difference. Typical drills wander and you want the cutting edges to help guide the bit. Since center drills are incredibly rigid and are meant to be used in rigid concentric holders they have a slightly different cutting edge geometry. A spotting drill puts a hole right where the VMC positions it even on an uneven surface because the tip is capable of side cutting like an end mill. Which of the drills above would you like to bring the tip down into the work and then crank one of the axis so the drill is cutting sideways? Most spotting drills can do light engraving work in mild steel, aluminum, and plastic. You can spin up a spotting drill bring it down into the work a bit and then turn on the x axis feed and run it horizontally at 60" per minutes. Try that with a jobber drill and watch it dance. They can also be used as a chamfer tool for all materials. You can run it right along the edge of a boss and debur without changing tools. There is a limitation to spotting drills that many people are not familiar with. You can't take a 3/8" spotting drill and drill a 3/8 hole with it. Because of their unique geometry most spotting drills should not be used to drill any deeper than their point. This is not the case for all manufacturers but for most there is no land or body relief so as soon as you get to the flutes they start rubbing.

And not shown..... an end mill.
If you take a worn out drill press and pop and end mill slam it down into your stock please have a friend nearby to film it. At the very least you might have some youtube material and you will probably get some good footage of the chuck flying across the room. Regular flat end mills are not self stabilizing and drill press tapers can't handle side loads.

Now if you have nice Bridgeport handy we can make it work. Four flute end mills don't have enough chip clearance so pick a two flute. Put that endmill in a holder or collet, check you position on your DRO's, give it a gentle feed and you can get a nice round on location hole. Maybe even use it as a starting hole for that D-bit reamer you made. Now if you have have a small 200lb benchtop mill with a cnc conversion and you bring your end mill down at a normal drill rate you are in for some drama. I know from first hand experience and long since sold that little mill. The only question is what will happen first, either the chatter is going to knock the head out of tram, the endmill will break or the part will be sent flying. Ideally you need a rigid, low run-out, low backlash machine to have the most success plunging with an end mill. It can be done, I do it all the time if I don't feel like a tool change, but it's no where the material removal rate that you can achieve with a drill. Another application for an endmill is as a makeshift reamer. Take a drill bit and drill a slightly undersized hole then follow it with an endmill and you can get a better finish, more round and on position hole.

Jaakko Fagerlund
01-27-2016, 03:58 AM
Jaakko, grinding the third and fourth facets is not what makes it self centering.
Of course it does, as the grinds extend to the center line of the drill. See picture above by Mcgyver. the last picture bottom most drill shows a 4 facet grind which is self centering.

Of course you can do a 4 facet sharpening wihout extending the relief to the center and that is not self-centering.

Euph0ny
01-27-2016, 07:22 AM
You asked for a lesson, so here you go.

Thanks for a rather comprehensive first post, and welcome!

Two really tiny nit-picks:

(a) perhaps it would make more sense with respect to the photograph to begin your paragraph about spotting drills with "#1" rather than "#5";

(b) you might like to add something about core drills, which are used to enlarge existing holes (and are arguably a better method than simply stepping-up through sizes of screw-machine or jobber drills, at least for fussy work). Like these:

http://www.icscuttingtools.com/Core.htm

http://advantage-drillbits.com/core-drills-2/core-drills

Jaakko Fagerlund
01-27-2016, 09:00 AM
(b) you might like to add something about core drills, which are used to enlarge existing holes (and are arguably a better method than simply stepping-up through sizes of screw-machine or jobber drills, at least for fussy work). Like these:

http://www.icscuttingtools.com/Core.htm

http://advantage-drillbits.com/core-drills-2/core-drills
And those are also recommended after drilling a hole that is to be reamed. Usually you get them undersized, like for example to ream a 16H7 hole you would get a 15.75 mm core drill. Makes the hole nicely round, straight and to the proper size for a reamer.

firbikrhd1
01-28-2016, 08:11 PM
Just a quick post to say thank you to all who responded to my question. It seems there will always be some disagreement about whether or not a center drill is appropriate for spotting, however the discussion has helped me to choose to purchase a couple of 118 degree spotting drills and give them a try to see if I really find any difference.

Doozer
01-28-2016, 08:24 PM
Beer in green bottles.
Beer in brown bottles.
IT JUST DOESN'T MATTER!!!

-Doozer

Forestgnome
01-28-2016, 09:16 PM
Brown bottles.

Dan Dubeau
01-28-2016, 10:11 PM
clear bottles....

PStechPaul
01-28-2016, 11:05 PM
Cans! All kinds. Ameri-, Mexi-, Puerto Ri-, ... :)

Black_Moons
01-28-2016, 11:58 PM
Just a quick post to say thank you to all who responded to my question. It seems there will always be some disagreement about whether or not a center drill is appropriate for spotting, however the discussion has helped me to choose to purchase a couple of 118 degree spotting drills and give them a try to see if I really find any difference.

I think the great thing about center drills for spotting is its cheap and easy to have a set and they cover a wide range of sizes. they are undeniably short and rigid so they do work good for spotting.

Are they ideal? Likely not, a hole that was actually made below the surface the same size as your flutes will likely get slightly better tracking for your jobber drill then just an undersized peck mark from a center drill.

Will you notice? Only if you are measuring your holes for +-0.002" or better I would say, and im not even sure if you would then, just that center drills as spotters are likely good to at least +-0.002". IMO you'll commonly make more error then that aligning the center drill/spotting drill to the work if your doing it by eye.

Ridgerunner
01-29-2016, 06:34 AM
How do you set a speed and feed with a centering drill? Particularly with cnc.

vpt
01-29-2016, 07:36 AM
Beer out of a stainless keg always tastes the best.

Euph0ny
01-29-2016, 08:05 AM
Beer out of a stainless keg always tastes the best.

Better from the skulls of one's enemies!

gaston
01-29-2016, 09:49 AM
darn I'm out of popcorn again. Is this going to go much longer?? Oh well I'll pop more anyway! hope I don't run out of beer

Doozer
01-29-2016, 01:21 PM
The main difference between spotting and centering bits vs. regular bits is the absence
of margin relief on the flutes. Spotting and centering drills do not have margin relief.
This makes them stay on center, even if there is some small amount of runout.
The other profile differences are largely irrelevant.
That is why I say they are so much the same, it is silly to opine which is better.

--Doozer

Mcgyver
01-29-2016, 01:56 PM
The main difference between spotting and centering bits vs. regular bits is the absence
of margin relief on the flutes. Spotting and centering drills do not have margin relief.
This makes them stay on center, even if there is some small amount of runout.
The other profile differences are largely irrelevant.
That is why I say they are so much the same, it is silly to opine which is better.

--Doozer

balls. they are better because.....there is no pip to bust off with a spot drill as can happen with smaller centre drills, and the drill smoothly in a cone the same shape as it vs bouncing/chattering around the rim a 60 degree hole.

unless you are only using the very end....in which case they are being used as a small dia spot drill

Can you start a hole with centre drill? sure and do so if its what you've got, but the spot drill is the better tool for the job

Doozer
01-29-2016, 02:50 PM
I have never busted the tip off of a center drill.
Maybe stop buying yours from India.

-D

Jaakko Fagerlund
01-29-2016, 04:45 PM
I have never busted the tip off of a center drill.
Maybe stop buying yours from India.

-D
If you've got the time to doodle around with the center drill, then have fun while others just do spotting & drilling meanwhile.

Mcgyver
01-29-2016, 04:49 PM
I have never busted the tip off of a center drill.
Maybe stop buying yours from India.

never? such an isolated existence. Smaller centre drills are more easily broken than a spot drill. A statement difficult to disagree with, even for the most disagreeable.

Doozer
01-30-2016, 05:58 PM
I am not shltting you.
I can't remember ever braking a center drill.
Most of the ones I have are an assortment from various tool scores
and old tool boxes I have bought over the years. Most are Keo brand
USA made. Never looked too close.
But honest to Abe Lincoln, I don't think I ever broke one.
You do know that you can't dwell with the some bitches, right?
With no margin relief, it is easy for chips to pack and break one.
Peck it and get out of there.
Maybe that is what you are experiencing.
Or maybe I have a golden horseshoe up my azz. I dunno.
Heaven forbid it may be that you're a clumsy baztard.

-Doozer

Mcgyver
01-30-2016, 08:35 PM
I can't specifically remember breaking one either, but I know have at least once. Small ones are fragile if there is any run out then can break. The point is though, to repeat for the umpteeth time, you can't break the pip on a spot drill, and a spot drill leaves the proper shape for the drill to start perfectly. They're also faster. There, three reasons. Have you used one? its beyond me why anyone who's used both wouldn't prefer a spot drill. whatever, its flogged to death.

Richard P Wilson
01-31-2016, 03:38 AM
I can't specifically remember breaking one either, but I know have at least once. Small ones are fragile if there is any run out then can break. The point is though, to repeat for the umpteeth time, you can't break the pip on a spot drill, and a spot drill leaves the proper shape for the drill to start perfectly. They're also faster. There, three reasons. Have you used one? its beyond me why anyone who's used both wouldn't prefer a spot drill. whatever, its flogged to death.

I didn't break a centre drill for over 20 years, then I broke 2 in a month! Haven't broken any since though. I have also broken a spotting drill admittedly a 3mm one, and probably my own fault for going in about 1/4" with it, rather than just 'spotting'.

dalee100
01-31-2016, 08:39 AM
How do you set a speed and feed with a centering drill? Particularly with cnc.

Hi,

I just program a linear move rather than a drill cycle. Rpms might be set to S1000.
A rough approximation might look like this.
Mill, G0 X1.Y1.
Z.1
G1Z-.05F2. (or however deep needed for spot)

Or Lathe G0Z.1
X0.
G1Z-.1F.004

Dalee

old mart
01-31-2016, 04:37 PM
I read somewhere on this forum that centre drills ideally require greater rpm than a lathe can manage. As for four faceted drills, I live and learn, I use some Guhring mt1 drills with tips cut in that fashion, and they are fantastic hole producers. As for using milling cutters for holes, I used a 1/4" slot drill on aluminium and the holes varied from a nice 0.25" to a nasty 0.257", you live and learn. I have some centre cutting four flute carbides which would probably be ok due to their stiffness.

jhe.1973
01-31-2016, 08:10 PM
Well..... it looks like this thread is starting to wind down.

In the interest of keeping the popcorn coming, maybe we can hijack the discussion to, "Is it possible/impossible to machine a truly round hole?

This can actually last for a loooooooooooong time!

:D

Doozer
01-31-2016, 08:56 PM
Well...
"Is it possible/impossible to machine a truly round hole?


:D

http://img.machinio.com/1fzv3sq/4117.jpg

Let's just say a PW 3B has about the best chance.
(not mine, but I wish)
Now come the Dixi pics.

-Doozer

jhe.1973
02-01-2016, 12:13 AM
Yeah, that might get ya close!

;)

old mart
02-02-2016, 12:54 PM
I looked through all the replies and noticed that jhe.1973 had NOTHING positive to say at all.

Carm
02-02-2016, 03:03 PM
I looked through all the replies and noticed that jhe.1973 had NOTHING positive to say at all.

Hmmm, wouldn't say that. Mebbe you're reading it the wrong way.
Arguments re: truly round could go on for some time!

PStechPaul
02-03-2016, 03:52 AM
I have an ordinary spotting drill, with a long shaft, that looks like this:

http://enginuitysystems.com/pix/tools/Spotting_Drill_20140506015036.jpg

And the tip is sharpened so:

http://enginuitysystems.com/pix/tools/Spotting_Drill_20140506014849.jpg

But I also have one that is simply ground like this:

http://enginuitysystems.com/pix/tools/Spotting_Drill_2_20140506015353.jpg

And the point is like this:

http://enginuitysystems.com/pix/tools/Spotting_Drill_2_20140506015734.jpg

Seems to work OK. I think it was repurposed from some other tool, maybe a center drill.

Black_Moons
02-03-2016, 10:52 AM
http://enginuitysystems.com/pix/tools/Spotting_Drill_2_20140506015353.jpg

Wow, now that is one rigid looking drill! Although I doubt it can go much deeper then the tip.

MyrtleLake
02-03-2016, 02:27 PM
That grind is a "flat drill (http://www.sommatool.com/catalog/cutting.tools/flatblanks.asp)." It has been around for a very long time--much easier to find in metalworking texts from the early 20th century. Sorta like a small spade drill in principle.