Accuracy of centre drill holes

[eKretz]

Here's a thought; get a 3-jaw chuck large enough to accept the largest bars to be drilled but not so heavy that it will be awkward. Machine a threaded adapter with a reamed 3/8" bore so the guys on the floor can use a 6" long 3/8" shank center drill. That can be your jig.

Won't get the centers inline, but will get the bar up in the machine. (What if the ends of the shaft are sawed out of square? What if the bar is not straight? What if the bar is a piece of hot rolled and isn't even round? Etc...)

The horizontal mill will get the centers straight and inline - so long as the operator sets it up correctly and the machine is in decent shape.

 

[michiganbuck]

If you have enough stock on the part OD to turn off then centers can be put in with a drill press, with a well placed out end block in to hold the part close to straight and on center. A combination square center V and a scriber, punch with a loop view adjustment should get .005 to center so needing .010/.012 to take on the part.
You can move, or true -up a center with a Norton point mounted center lap on the tail stock, but you don't want to do that for a 1000 part run.
Way out of whack centers can cause some problems on a high precision part that is why grind shops do a little lapping with an abrasive point lap, most/many lathe shops don't bother. Your machine centers should be near dead on true center, figure what error you see in the machine center you will get double that in the part.
With poor machine centers it is good to have a line up mark on the center and one on the part so if you have to put it back in or do another operation at least it will match while in your shop.
I have had to move a center .0001/.0002 on repair parts using a Norton center lap, agree nobody would want to do that for 1000 parts.

 

[Marty Feldman]

Yosiu: Your frankness in making clear your level of experience with this is appreciated:
"As I'm not familiar with turning between centres..."
"I saw some guys doing them with handheld drills on shop floor so i can't be crucial,right?..."
"Sorry for newbie question but this is far from my regular work..."

With that level of experience in mind, I think it would be wise to consider seriously what eKretz said in post #14. He has summarized in one brief golden rule almost all of the advice you are getting in this thread:
"Getting things right from the start means more accurate work and longer lasting, more accurate tooling."

-Marty-

 

[michiganbuck]

OT
I think t is foolish to make a precision bearing shaft (or the like) with it not made between centers. Why put <.0002 bearings on a bearing fit that runs out .0001/.0002.end to end.
The max given spec on a precision part is the most error it can have to being scrap, not the expected norm IMHO.

 

[eKretz]

OT
I think t is foolish to make a precision bearing shaft (or the like) with it not made between centers. Why put <.0002 bearings on a bearing fit that runs out .0001/.0002.end to end.
The max given spec on a precision part is the most error it can have to being scrap, not the expected norm IMHO.

Not necessarily. I've made shafts like that with the entire thing machined in one chucking, then faced off the extra chuck end stock later. But I do get the gist of what you're saying. Generally I agree that if one should need that kind of precision the job would usually be best served with finish grinding between centers.

 

[michiganbuck]

Out of a precision chucker or a very good lathe one can run to .0002 or so at each end. so almost a half thow error possible end to end running in an almost perfect bearing. Nobody would want a half thow error in a precision assemble but likely nowadays that is what one gets,
I have run near dead on bearing shafts on just OK lathes, with running the part between centers.

 

[Joe Henderson]

If the mill will handle it that could work. If you have a big enough steady rest for the lathe, set it up close to the chuck and set it for the diameter of the piece you're wanting to center drill. Move it out and chuck one end of the 21.5" shaft in the three jaw chuck and face and drill in the steady end. Flip it and do again. You can do that for all parts once the thing is set.

 

[Terry Keeley]

I haven't read all the posts but am I missing the obvious here?

When a shaft is turned between centers wont it be as round/straight/true on the diameter as the machine is capable? Even if the ends are not drilled exactly in the center of the stock?

 

[eKretz]

I haven't read all the posts but am I missing the obvious here?

When a shaft is turned between centers wont it be as round/straight/true on the diameter as the machine is capable? Even if the ends are not drilled exactly in the center of the stock?

The only correct answer to that is: "maybe." Bad centers can cause all sorts of problems. They may or may not manifest in any certain instance, but a professional shouldn't leave things like that to chance, they should set themselves up for success with every step of the operation. Read the thread...

 

[eKretz]

If the mill will handle it that could work. If you have a big enough steady rest for the lathe, set it up close to the chuck and set it for the diameter of the piece you're wanting to center drill. Move it out and chuck one end of the 21.5" shaft in the three jaw chuck and face and drill in the steady end. Flip it and do again. You can do that for all parts once the thing is set.

Not if you have hot-rolled stock. Or out-of-round stock... that's why I mentioned the cathead as an option earlier. If you have those conditions, much faster to do the work on the mill. And I would never run any unmachined surface on a roller rest - good way to damage the bearings. Good quality roller rests use very expensive bearings - near on par to spindle bearings. And you're still left with the problem of getting an out-of-round center if your stock OD isn't round. The shape of the center will be affected by the surface the steady rides on.

 

[Terry Keeley]

The only correct answer to that is: "maybe." Bad centers can cause all sorts of problems. They may or may not manifest in any certain instance, but a professional shouldn't leave things like that to chance, they should set themselves up for success with every step of the operation. Read the thread...

The OP's original question:

is it really important to get both centre drill holes spot on coaxial and parallel?

My answer: NO!

 

[EmGo]

My answer: NO!

That answer is wrong, because center holes are not spherical surfaces that touch the angular centers in a circle. (It would be an oval if the centers are offset.) They are both 60* cones. Therefore, if the cones are not in line, then the part will be riding offset and/or bent while machining.

As an example, think if the cardan joints in your dyno. They only work if you have a pair, offset at 90* to balance their uneven rotations. If you try to use just one, the coupled pieces will have a speed and position variation as they rotate. This is like that.

(Also why I really like those spherical center drills, but you can't expect them to solve all your problems.)

Of course you can sometimes "get away" with some stuff, but running 1000 parts trying to "get away" with a shit setup is not going to turn out well. This isn't how we do things, if we even pretend to be professionals.

And all this other crap is silly. You guys try running a thousand parts through a lathe with steady rest or some of these other suggestions, and get the lengths down pat at the same time ... it's sily. The problem has been solved for decades. That's what facing and centering machines are for (and they go to great lengths to make sure the centers are in line, like ANYONE who has ever run a cylindrical grinder understands). He's just trying to do the same thing in a horizontal, which has also been done. A lot. It's a standard method of dealing with a common problem.

 

[Terry Keeley]

That answer is wrong, because center holes are not spherical surfaces that touch the angular centers in a circle. (It would be an oval if the centers are offset.) They are both 60* cones. Therefore, if the cones are not in line, then the part will be riding offset and/or bent while machining.

As an example, think if the cardan joints in your dyno. They only work if you have a pair, offset at 90* to balance their uneven rotations. If you try to use just one, the coupled pieces will have a speed and position variation as they rotate. This is like that.

(Also why I really like those spherical center drills, but you can't expect them to solve all your problems.)

Of course you can sometimes "get away" with some stuff, but running 1000 parts trying to "get away" with a shit setup is not going to turn out well. This isn't how we do things, if we even pretend to be professionals.

And all this other crap is silly. You guys try running a thousand parts through a lathe with steady rest or some of these other suggestions, and get the lengths down pat at the same time ... it's sily. The problem has been solved for decades. That's what facing and centering machines are for (and they go to great lengths to make sure the centers are in line, like ANYONE who has ever run a cylindrical grinder understands). He's just trying to do the same thing in a horizontal, which has also been done. A lot. It's a standard method of dealing with a common problem.

"is it really important to get both centre drill holes spot on coaxial and parallel?"

I see your point of course, for a perfect set up the center drilled holes should be coaxial.
So the real question then is what is the definition of "spot on"?

 

[eKretz]

"is it really important to get both centre drill holes spot on coaxial and parallel?"

I see your point of course, for a perfect set up the center drilled holes should be coaxial.
So the real question then is what is the definition of "spot on"?

Within a few thousandths is generally good enough to never see any ill effects. Sometimes though, even that won't do it. (Think very slender and long parts, or those with extremely tight roundness callouts). Sometimes, you could put centers in with a blindfold on and a hand drill and it might just work... But whether your answer of "NO!" is correct or not really depends on the exact job at hand and what your definition of "spot on" is.

 

[BoxcarPete]

Within a few thousandths is generally good enough to never see any ill effects. Sometimes though, even that won't do it. (Think very slender and long parts, or those with extremely tight roundness callouts). Sometimes, you could put centers in with a blindfold on and a hand drill and it might just work... But whether your answer of "NO!" is correct or not really depends on the exact job at hand and what your definition of "spot on" is.

How about for tapers? If you offset your tailstock a couple hundred thou to form a tapered feature, wouldn't that be effectively the same as parallel but non co-axial centers by a similar amount? Certainly if you did a big offset for a significant taper it would be worse than a few thou or a handful of MoA error.

 

[eKretz]

How about for tapers? If you offset your tailstock a couple hundred thou to form a tapered feature, wouldn't that be effectively the same as parallel but non co-axial centers by a similar amount? Certainly if you did a big offset for a significant taper it would be worse than a few thou or a handful of MoA error.

Yep, it sure is. If you need a very accurate taper or have a lot of parts to do, that's not a great way to do it. You can help out a little by using a spherical center. On light stuff that's still large enough diameter to be pretty rigid you can get away with a little more. If you have a very heavy workpiece, or a very picky one, use a piece of equipment made to turn or grind tapers. A lathe with a taper attachment or a universal grinder with a swivelling table. Both will keep the centers inline.

 

[Superbowl]

I am wondering if the depth of the centering holes can be an issue if they are not in perfect alignment. For instance if you drill into each end 1/4" vs. 1/2" assuming the drill and the dead centers have the same angle. The deeper the holes perhaps the more error between them becomes.

 

[eKretz]

I am wondering if the depth of the centering holes can be an issue if they are not in perfect alignment. For instance if you drill into each end 1/4" vs. 1/2" assuming the drill and the dead centers have the same angle. The deeper the holes perhaps the more error between them becomes.

Yes again. If misaligned, the deeper the 60° hole, the bigger the gap at the opposite end with the same angle...

 

[BoxcarPete]

Yep, it sure is. If you need a very accurate taper or have a lot of parts to do, that's not a great way to do it. You can help out a little by using a spherical center. On light stuff that's still large enough diameter to be pretty rigid you can get away with a little more. If you have a very heavy workpiece, or a very picky one, use a piece of equipment made to turn or grind tapers. A lathe with a taper attachment or a universal grinder with a swivelling table. Both will keep the centers inline.

So you're telling me it's a bad idea to try and taper the ends of a hanbo (40" long 1.25" diameter hard maple martial arts staff) by loading it up cross-centers (was planning on putting a pair of centers .300" apart to index the diameter along its length) and taking a bit off the ends?

 

[eKretz]

So you're telling me it's a bad idea to try and taper the ends of a hanbo (40" long 1.25" diameter hard maple martial arts staff) by loading it up cross-centers (was planning on putting a pair of centers .300" apart to index the diameter along its length) and taking a bit off the ends?

Nope. Unless you're worried about holding the taper and diameter a hell of a lot tighter than you really need to... For what amounts to a decorative item, (no tight sizes...) all bets are off. I say go for it.