What's new
What's new

Turning long tapers (42-47")


Mar 22, 2007
Vancouver BC
I started this project by searching the forum and the web for anyone who had a similar experience and found nothing. Hopefully this will help someone in the future or give ideas to others.
The project started as approximately 60 spindles for a handrail in a high end house. The spindles were to be solid brass, 36” and 42” long, with the majority being 36” long. The five longer ones were to be sunk into concrete. The kicker is that the spindles are tapered, 1” dia at the bottom and 1/2” dia at the top. That’s a fair old taper for me. Couldn’t find anything indicating anyone else had done something like this, so started thinking. The job has to be done in a single cut, since any taper attachment must be fixed at one diameter. I did try a spring loaded steady finger to see if I could get enough support, that didn't fly.
If I could set the taper attachment just ahead of the cutter and pick the right insert or make a toolbit, then it should be possible. The customer wanted a proof of concept quickly, so I set up my two big lathes with the same setting on the taper attachments. Machined half of the taper on each lathe. That got me just 36”, my taper attachments being 18” long each. Of course this meant I had to blend the start and stop point which was a pain. However being a proof of concept, it just had to pass inspection by the designer and the homeowner. Size is not really an issue, just a really nice finish and even taper. The other point which the alert will have noticed is that the longer pieces wouldn’t work this way. So the answer seemed to be to make a longer taper attachment. I decided 48” would be enough, and bought a piece of aluminum flat bar and a chunk of cold rolled. The machine I was going to use was a Colchester Mascot 1600. The taper attachment is a dovetailed piece of tool steel, hardened and ground, with a 1/2” x 2” guide bar on the top that sets the angle. This all runs in castings bolted to the carriage. I decided for a short run that the aluminum would be good enough, sufficently lubricated. I machined the dovetail on the aluminum in two set ups, my mill not being long enough to do it in one. A pivot and two arcs for lock screws completed the aluminum. The cold rolled just needed filing and stoning to fit and holes for the pivot and the screws.

So far so good. Of course at this point, Murphy showed up. The customer and designer had decided they needed longer spindles. Oh and now there are 124 of them. So now they are 42” and 47” long. Just too long for my new taper attachment. Start again.
Same design, longer pieces. Six foot long this time. I decided not to machine the dovetails at this point. I sent the aluminum to a shop with a long bed mill and they did the dovetails in one cut. I figured this job had enough failure points and the dovetail could use a nice parallel cut. A few days later I have my new improved taper attachment.
Now the fun starts. The steady for my Colchester is a two finger style, with brass tips. I cut some test pieces and started. It was immediately obvious that this was not going to work. Chatter and vibration from the start. So, what to do. The steady from my Standard Modern was the three finger kind, but about an inch and a half too tall. OK I can work with that. I bandsawed the feet off and machined the bottom of the casting. Then machined the cut off pieces and made them so a standard thickness was missing. Cut some O-1 ground stock and drilled the holes so I could use the steady on the original machine again.
Back to the Colchester. Drill and tap holes in the carriage wings next to the original holes and bolt up the steady. OK new part. Better this time but still not what I need. So I’m thinking that the problem is not enough support, the tips on the steady being cone shaped and about 1/4” in diameter at the contact point. I decide to make new fingers for the steady, full 1” in diameter. I have some nice old bronze propellor shaft in stock, so that will be good and tough. After making these, I put a boring bar in the chuck set to 1” and bore the tips so they are on centre and good for size. Success! Perfect finish, even taper. Very pleased with myself. For one part. Halfway through the second, the vibrations re-appear. Now what? Lube. Must be the answer. Grease, moly, oil, Fluid Film, same answer. The tips were wearing out before I finished the cut. So I could nip up the screws but there was always some chatter or a line where the support was re-established. What to do?

The problem seems to be that the tips are wearing out on the long pass with lots of pressure. Lube doesn’t seem to be the answer, so harder tips. I come to the conclusion that bearings are the answer. OK more prop shaft and shortly we have bearing fingers. This proves to be the silver bullet. Solid finish, no wear and now nothing to do except shovel chips. I wanted to do this from the start, but time pressure from the customer and homeowner led to a sub-standard technique.

Now I expect some of you are screaming ‘hope you got time and materials!!!’. No such luck. Quoted job. So now you are screaming ‘yer an idiot!!’. Well yes, but not on this one. The quote was comfortably fat enough that I could go through these convulsions and still make out quite well. The point of this post is to hopefully help someone else who is stuck in some aspect of a job like this and not waste time and money that isn’t there. So in the end it was a rewarding job, but there were some sleepless nights trying to figure out how to do it.

Hope the wall of text helps someone out, and let me know if anything is unclear.
Possibly, I'm not sure if the tailstock has 1/4" of offset. Also, would the steady work like that? I think it needs to be parallel with the spindle for the steady to work. I've not tried it, maybe someone else can pipe up.
deltap has the right idea. You don't have to make anything special. Most manual lathes have all the "special" equipment right there. If you don't have a lathe dog you can cobble one up pretty quick or use a cheap die handle. If you don't want to disturb the center of your tailstock get a threaded arbor for a cheap boring head and use that to offset the center. Offset the tailstock end 1/4" and you are on your way to fun and profit!
I do tapers like that in wood up to 36" (pool cue shafts, e.g.) rotating between Hardinge centers on my metal planer with live tooling.
Don't use a steady, but you would have to with metal.
I'd be comfortable taking that up to 6' or so in metal with a suitable full contact follower (actually, "leader") like on a back knife lathe.

Depending how you arrange the tooling approach and the centers, you can cut either straight tapers (live tool on center) or very gradual hyperbolic curves (live tool above center).

With my centers on a pivot table and a follower on the column, my set up will even do mild shapes

Or you can make your life really interesting and offer to put reeds on the tapered spindles :)
Then it is simple indexing instead of continuous rotation.

Can you convince them to leave a foot long, or 2 ft long straight section at the bottom? Every inch you don't have to taper is a big savings in effort, time and tooling.

But i think the way they actually do those in metal is rolling or hammering.

Last edited:
That's an interesting way to do a taper, for sure. Amazing what one can come up with to get the job done...
I'm with you for sure on the rolling method, and tried to get them to go that way, but the designer and owner wanted solid. There was no negotiating the style or material. Hence the big fat quote. I believe the final tally for the whole handrail (spindles, antiquing, concrete work, oak hand rail) was close to $75k
Mount the material using a tailstock no offset (bad idea.)

use a follow rest

Use a tool that's ground into 2 1/8" wide cutting faces, offset in the direction of cut maybe a 1/16. So the max cut any face of the tool will cut will be 1/8" wide. So at the start you will be cutting full depth and producing 2 streams of chips, half way along only one stream of chips until you get to the end.

That's how I would do it.
Mount the material using a tailstock no offset (bad idea.)

use a follow rest

Use a tool that's ground into 2 1/8" wide cutting faces, offset in the direction of cut maybe a 1/16. So the max cut any face of the tool will cut will be 1/8" wide. So at the start you will be cutting full depth and producing 2 streams of chips, half way along only one stream of chips until you get to the end.

That's how I would do it.
If you are going to use a single point tool as opposed to live tooling, design it as a skive tool.

A device I think called a culminater was available and a few sites show how to make one. It's used to extend the taper cut length of the taper attachment. Simply put it moves rather than a fix clamping location for the taper draw/push bar.
Well I must be behind the times, is there really a cnc lathe that can do a 4' long taper from 1/2" to 1' in brass with one line of programming? I want one!
Back in the day you could order an attachment with a lathe purchase that was called a "Geared Taper Attachment". This attachment would cut long tapers, only limit was the travel of the carriage on the lathe. I have never seen one, just pictures of them. Parts were run with slow RPM's with old conventual tooling. Like Steven said, skiving tools were used or hi-positive cut tooling used.
I could have the 123 parts made in the time you've been talking about it.

You could also make a box tool to turn a long taper. But that would also involve doing some actual work.
Last edited:
SIP6A, got a sketch of a box tool for long tapers? That's not something in the complement of tooling I've got for my DSM. All the box tools are fixed diameter, and all the taper tools are "swing" of one variety or another without the guide/backrest built into a typical box tool.
Well I think the customer was hoping for something a little more pro than a guy with a south bend and a bunch of emery. However it could work with a lot of time. But since they specified a machined finish, it's a non-starter in this case.