Turning Accurate Tapers - my take on an old task.

Let’s say you need to cut a male taper on your lathe like maybe a #4 Morse. A #4 Morse has 0.62326” total taper per ft according to Machinery’s handbook. You have no taper attachment. You have a good sleeve to use for a gage. You want the first trial of the taper to be as accurate as possible.

First order of business is to determine if the taper is to have a driving tang or is cropped like the shank end of a dead center. If you need a tang, center drill both ends 5/16” in the lathe and then mill the tang detail according to #4 Morse manufacturing data.

Let’s assume the #4 Morse taper shank tool you have to make is 14” long over-all. You need an accurate length to calculate the correct tailstock offset. The center penetrates some distance into the center drilled hole so the question is what is the effective depth of the center and how much deduction do you take from the overall length. A good assumption is midpoint on the conical land of the center drilled prep.

Another consideration: the taper axis is inclined with respect to the spindle axis and the offset tailstock axis by a amount to generate the half angle of the taper. The tension on the center and the cutting forces make the conical centers “waller out” the center drilled conical lands until it resembles an annular section of a torus. An inclined plane intersecting a cone generates a type of ellipse. A torus by definition is round. Thus a torus inclined on a cone makes contact at two points – in our example in the horizontal plane. There will be some uncertainty in the vertical plane but one safe to ignore because forces affecting the taper turned in a lathe lie in the horizontal plane.

Given the above, it would appear that some metal deformation could be expected as work progresses requiring occasional center take-up to minimize lost motion along the taper’s axis. In effect the over-all length will be reduced by what I have come to call an “important trifle”. These are small details but significant when cutting accurate tapers from the get-go. Looking at our original problem: a #4 Morse taper has 0.0519 taper per inch. If the overall part length is 14.000 inches, the tailstock offset is (0.0519” / 2) x 14.000” or 0.3636”.

The effect on the taper is proportionate to over-all length / effective length. In our example where the effective length is 13.955 (or some such figure) the proportionate error factor is 1.0032. Since the #4 Morse taper is roughly 4” long the taper error calculated by our example is 0.0129” on the radius – larger on the big end. Total taper error on the big end is 0.0256. These small trifles have a way of stacking up. You may have a rough idea of how to determine the effective length between centers (don’t neglect the cosine of the half angle in your calculations) but rough is not precise. The effective length has to be precisely determined otherwise whatever tailstock offset you may use will be a stab in the dark.

The question is how to eliminate these uncertainties so they don’t plague us with accreting trifles?

Consider: a ball resting in a conical recess (like a center-drilled hole) makes circular contact at the plane of intersection. The ball can be spun in any direction but its circular intersection with the cone remains unchanged.

This may exploited for our purposes. Anneal some 3/8” dia balls salvaged from a defunct bearing. Grip them one by one in a collet and center-drill 5/16” full depth and with a dinky little boring bar tool out the conical recess to clean up. Make plenty because you will lose them in the chips. Re-harden and draw to Rc58 or so. Make some of larger and smaller sizes. I call these little aids “olive balls” because they resemble pitted olives to my overheated imagination. .

A 3/8 ball contacts a 60 degree cone on a 0.328 dia. Make your center-drilled center preps accordingly. Apply a small blob of sticky grease in the center-drilled holes, stick in the balls and mike over them. Deduct one ball diameter from the mike size to obtain the effective part length between ball centers. Use this length to calculate tailstock offset. Using the olive balls in the center-drilled holes place the part to be taper turned between centers and go to town. The balls will accommodate the nutating part axis as it rotates between offset centers. They will burnish a little land in the center prep that in no way interferes with later operations where a center has to be employed.

If your offset is accurate and your tool on center you should be able to cut an accurate taper from scratch. Chances are you will need to make a few offset corrections because that is how it goes in the machinist’s trade

BTW. Machine tapers have to be accurate as hell if they are to seat properly. If I was to make the taper tolerance call, I’d hold taper sockets nominal to -.0002 per inch of diameter and the male taper nominal to +0.0002 per inch of dia. Axial tol on the gage line is widely available and is usually +/- 1/64.” In the absence of proper gages most shops use new or nearly new sockets and shanks for gaging. While this expedient has its hazards I’ve seen good tooling made this way. Few lathe hands bother tooling the last little refinement to a machine taper. They get it a thou or two oversize and stone or polish to final fit. A good lathe hand can with care fine tune tapers rivaling work generated on a cylindrical grinder in about the same time for the first few parts.

Comment? Analysis?

Thank you for a very useful and informative post!

I have been faced with this conceptual issue while trying to get my lathe/tailstock set up to a.) accurately turn a 12" long 2.000 diameter plastic rod WITHOUT taper, from a 2.005" blank, and b.) figure out the taper setup with the tailstock for a double-ended plastic housing taper of same approximate overall size. The detail presented by Forrest Addy confirms my vague foggy notions of some of the areas of possible concern in trying to get everything set correctly for parts with little oversize material to work with. Now I'm even more concerned.;-)

Forrest Addy said:

<>

BTW. Machine tapers have to be accurate as hell if they are to seat properly. If I was to make the taper tolerance call, I’d hold taper sockets nominal to -.0002 per inch of diameter and the male taper nominal to +0.0002 per inch of dia. Axial tol on the gage line is widely available and is usually +/- 1/64.” In the absence of proper gages most shops use new or nearly new sockets and shanks for gaging. While this expedient has its hazards I’ve seen good tooling made this way. Few lathe hands bother tooling the last little refinement to a machine taper. They get it a thou or two oversize and stone or polish to final fit. A good lathe hand can with care fine tune tapers rivaling work generated on a cylindrical grinder in about the same time for the first few parts.

Comment? Analysis?

Click to expand...

Nice discussion for sure. One thing you did not mention is the idea of relieving the mid portion of the taper thus making no attempt at contact here. Most of the commercial tapers I have are made that way with about 30% of the length making contact at each end and the mid 40% (or so) relieved 30 -60 thousandths. When I have made a few tapers, I have followed this same routine as it does make life easier with respect to getting a good fit at the inboard and outboard portions of the taper where it really counts. Also makes for less area to polish with a stone or fine si-carbide paper to get a good blue-up or for really final inspection "shine-up" of the crests of the surface irregularities where they contact the female taper. I assume you would endorse that practice? Maybe it is a sign of my second-rate skills.

Thanks for sharing that neat and effective technique Forrest.

First description I saw was in Model Engineer by Geo. H Thomas around 1971 and later reprinted as a chapter in his book Model Engineers Workshop Manual. Was well worth a read as it covers pretty much all the sane methods of taper turning advising on strengths and weaknesses with tips on making set-up easier. He goes into a bit more detail about calculating the effective length of the blank so that the taper can be set directly by measuring the offset applied to the tail-stock using a plunger type dial gauge. Also a few numbers on the effects of errors and the tolerances to be met for a well fitting taper. Geo. says BS standard is 0.0002 exactly end for end regardless of diameter. Geo. doesn't do things quite the way you do, he suggests the use of two loose balls running in hollow centres at tail and head stocks. Also goes into a bit more detail as how to trim the ends of the blank to get the effective length needed. If you are doing things by calculation and measurement that length needs to be pretty accurate, around 15 thou error there will use up pretty much all your tolerances on diameter.

All to much faff for me. Everything I've owned which can properly be dignified by the term lathe, as opposed to mangle wiv extra bits, got or came with a taper turning attachment. Two bed-stops and length rods or a selection from the third best gauge block set to define saddle travel and a tenths gauge indicating on centre height makes direct measurement of taper set easy.

Clive

dgfoster said:

Nice discussion for sure. One thing you did not mention is the idea of relieving the mid portion of the taper thus making no attempt at contact here. Most of the commercial tapers I have are made that way with about 30% of the length making contact at each end and the mid 40% (or so) relieved 30 -60 thousandths. When I have made a few tapers, I have followed this same routine as it does make life easier with respect to getting a good fit at the inboard and outboard portions of the taper where it really counts. Also makes for less area to polish with a stone or fine si-carbide paper to get a good blue-up or for really final inspection "shine-up" of the crests of the surface irregularities where they contact the female taper. I assume you would endorse that practice? Maybe it is a sign of my second-rate skills.

Click to expand...

Many years ago, my English comp teacher taught the class about the importance of limiting the scope of a writing project to keep it within an acceptable length and to prevent interesting but irrelevent material from diverting the reader from the work's thesis.

Accordingly, I did not treat relieving diameters, taper retention schemes like draw keys, collar nuts draw bolts, positive driving features, quick release designs, or for that matter math and formulae, standard tapers, employment of accurately fitted tapers in other machine elements like gibs, taper pins, wedge jacks, valve seats, collet tooling, venturis, and keys, Nor have I mentioned the making of gages, taper metrology, theoretical considerations for self-holding and self-releasing tapers, the various standard documents for Metric and Imperial, and the specific situations for the employment of one Vs another. The topic of tapers used in machine technology is huge; probably worthy of a book if addressed in detail. There might even be such a book: I've never looked for one until now.

I limited myself to turning accurate tapers addressing the traditional method used on an engine lathe and suggesting an easy to implement refinement.

I'll leave it to the responders to expand the topic of tapers into related areas of interest as you, Mr Foster, rightly and cogently commenting on relieving and fitting tapers.

I look at all the calculations that I used to do in mold making. Darn near everything is tapered. Threaders (to make female threads in the part) were the worst. You are either making a "straight" thread which most places will allow you 1/2 deg draft or tapered pipe. Figure out everything and then apply the shrink factor. Did all that and usually had somebody check your math. On a tapered pipe threader, you might have 4 hours in the part before you mill the threads. Can't afford many screw ups or you're no longer working.

Unless you're over 50, you probably don't know how to do the math for the above without a CAD system. When was the last time somebody used a trig table?
JR

Haven't used printed tables for a while but use the calculator functions all the time. Doing some math in grease pencil on the vise top or table has saved my butt any number of times. It's a cross check for what's happening on the machine to make sure what comes out is as expected.

One place I worked for a while the boss wasn't that good with the math (among other things) and one of the jobs he gave me involved some tapers. The parts were duplicating a laser beam dump so it had a tube with an inside taper and cone in the middle - two parts. He's worked out what he thought they ought to be and gave me a sketch with angles and diameters. To make sure I worked it right I checked to see where the taper should run out. And it didn't work out. If I used the large diameter, at that angle, the small diameter was too big. Asked him about it but he said just do it like that angle and large diameter. Okay. After farting around, machining it to show it wouldn't work, making design mods to compensate we finally had to shrink the parts together because the flange design he'd first sketched was out the window. Some trig would have saved time and effort and he'd have preserved some respect that he just pissed away.

Interesting way to cut a taper.

Wouldn't you lose center force and the ability to hold the work piece against the chuck end center once you move to far from center line?

How much of an angle relative to the chuck could one expect to go before issues with driving the work piece at the chuck happen?

Our taper attachments suck balls at work from so much slack.We have been fortunate to be able to use our power feed 6" travel compound and setting the taper by calculating how much
indicator travel in XX distance.I can never remember the formulas and really have never tried because we have machinist hand books in our tool boxes which can be just as important
as your tools,can't measure or cut what you can not figure out what the dimensions are supposed to be.
The method above may be the best choice if we ever have to turn a longer accurate taper than we can handle with the compound.

Just had a thought.....
If one was in a pinch what if a plate was made that fit your steady rest with a pivot bearing mounted to the plate on the steady rest.
Allow means with slots or what ever so you get the correct offset off center line to get your taper right then lock it down.Now you have support
to help you tailstock center keep chatter down.
If the taper was short enough and shaft large enough no tail stock would be needed.

I have used Forrest's method but used a ball end mill to cut a depressed partial hemisphere in the work ends. The headstock and tailstock centers were similarly depressed hemispheres. This was on A2 shafts about 18" long and 1.125" at the thick end and about .75 at the thin end. Drove them with an offset 1/8th pin in the head stock center which engaged a correspondingly offset loose fitting hole in the headstock end of the work. Chatter was a problem that was overcome with a very very sharp HSS cutter with a small nose. Once I got that figured out, it worked well. I liked not having a dog flying around on the headstock side. That allowed working right up to the end of the work piece.

Denis

Forrest,
Thanks for taking time to explain such a simple task that usually is difficult to execute (for me). I saved this post so I can reread this as many times as it takes to fully penetrate my small brain. I have read of the concept of using a ball in a work piece center and against a taper in the headstock and tailstock before but never really liked the idea of a ball that had nothing to stop it from turning in the tailstock taper. The concept I liked. The ball that would be against a headstock taper would be running against a renewable taper. As usual, you have presented an excellent technique to accomplish an often needed task! I have been blessed with the availability of taper attachment equipped lathes the last several years but not in my home shop!
Rick

Is there a reason using a dial indicator on the carriage over a measured distance wouldn't be a better way to set the offset? Of course you'd have to turn the od straight first.

G01 x??z??

I am curious as to how well driving tapers have to match in order to work. In the electric scooter motors I have been building and testing I use a 20:1 taper (length to diameter difference). The taper is .787" at the large end and is about 1" long, an M8 bolt pulls them together. I make both the male and female tapers with the compound rest, which I set as accurately as I can with a dial indicator. I have made about a dozen motors, with a new setup for each. I don't have a master gage and I don't do any checking with bluing between male and female while I am cutting the parts.
I was expecting to see signs of slippage due to mismatched parts after full current stall tests but so far they have all held. The torque that these motors generate at stall is 75Nm or 55ftlbs.

A morse taper that does not have a drawbar pulling the taper together is a different animal and I realize that runout at the tool tip caused by taper mis-match is also an important consideration.

If you are fortunate enough to have enough compound travel I have seen it done where one chucks up the sample piece, indicates the sample piece so the compound is parallel with it, then just turned it the hard way using the (usually hand feed only) compound screw. I even saw a guy once make a piece of round stock about 6 inches long with 1/4 of it milled away for a sine bar shelf, centers on both ends so a compound or taper attachment could be fine tuned for angle off a sine bar rather than relying on the scale on the taper attachment or the compound rest scale.

I am fortunate to have a ton of compound travel and have cut a couple Morse tapers for my own tooling- mostly for my rotab, which has a MT center hole. If memory serves I just chucked up a clean MT sleeve, dialed it in true, then fiddlefarted around with the compound angle and a .0001" indicator until it showed no change when run into the taper. It did work "ok" for my purposes. Mr. Addy's ideas are way cooler though!

Forrest,

What an elegant solution!

I don't often need to turn a taper by offsetting the tailstock, but the next time I do I will try the ball bearing method. McMaster sells machinable steel balls, for those who don't have a collection of used ball bearings.

Forrest,

Thanks for the post.

I'm not clear on exactly what your "olive ball" looks like. Specifically, I don't understand what to do with "a dinky little boring bar".

I understand a 3/8 sphere, mounted in a collet, center drilled to a 5/16 diameter x 60 degree countersink. Have I got that right?

Please explain (expand) what you're recommending to do with "a dinky little boring bar".

Regards,

Bore the center after drilling it, that gets the cone concentric with the lathe axis.

extropic said:

Forrest,

Thanks for the post.

I'm not clear on exactly what your "olive ball" looks like. Specifically, I don't understand what to do with "a dinky little boring bar".

I understand a 3/8 sphere, mounted in a collet, center drilled to a 5/16 diameter x 60 degree countersink. Have I got that right?

Please explain (expand) what you're recommending to do with "a dinky little boring bar".

Regards,

Click to expand...

Sorry. Presumption on my part where my narrow experience is the whole world.

Olive ball. Consider a pitted olive. Take an actual pitted olive and you can see the little hole where the pitter went in and a larger one where the pit was forced out. Consider a steel "olive ball" used for taper turning in my grand design above: a ball with a center-drilled passage through the ball's center. Big hole at one side where the big end of the 60 degree conical center went in and the little hole at the opposite side where the center drills pilot (or may not have) emerged. It's not too great a leap of imagination to think of a pitted olive when examining a centering ball.

Since you are drilling a ball the centerdrill may wander. The axis of the cone has to intersect the ball's center. If it doesn't you may have to tool it out with a "dinky little boring bar".

Grind a pointed boring bar suited for taking a skim cut in the center hole The tool looks like an engraver cutter if your familiar with them or a long skinny uniflute countersink. It's actually a single point lathe tool intended to cut at the tip, fed along the cone wall with the compound swiveled at 30 degrees. It's designed take a light cut along the conical surface of the center hole.

Back in my day, a ffrequent third year apprentice assignment was when the boss pointed to a raft of pallets covered with electric motor armatures. The main task was to re-tool the centers bruised up by the motor guys pulling pulleys, couplings, bearings etc but often additional work was required for each like straightening, welding, stubbing. After the survey and preliminary work was done, the centers had to be trued to the bearing fits from which all othere diameters are referenced.. You set each up in the lathe dialing-in the bearing seats and running the overhung seat in a steady rest. Then you re-tooled the centers prepatory for plating and grinding battered or corroded bearing seats, seal areas - or re-cutting bearing nut threads after weld build-up - or the shaft after weld build-up or re-stubbing. A hundred or so armatures could keep a sharp apprentice hopping routing the work, ensuring everything that had to be done was done, keeping lists, folowing up etc. It was a job of trust, a dubious honor.

A good lathe hand could re-cut the centers of 6 to 12 armatures, pump shafts, transmission shafts etc per shift depending on size and complexity. Whopper shafts weighing tons took took longer as did tiny sensitive ones.

If you've ever done any machining on shafting removed from service or repair, you've performed a quick check between centers for concentricity and straightness, and if necessary re-tooling of the center holes. This is a routine procedure in any competent shop.

BTW, pullers are like air hoses: indespensible but capable of damage leading to dire consequences if mis-applied. Practice safe pulling: if you have to pull a bearing or gear off a shaft, use the center protector - or make one.

Who knows how to make a center protector?