View Full Version : Problem: how to machine a spiral groove in a flat disk (like a record groove, but...

07-03-2014, 06:12 PM
I have more ideas than I know what to do with. Probably we all do. The latest seizure involves a spiral groove on a 6" diameter flat disk, conceptually like the groove on a record. But, I want it to advance 1/2" per revolution, from an initial 1" radius offset from the center out to 3" radius offset, and the groove needs to be about 1/8" wide by 1/8" deep. That works out, I think, to four revs to get to the outside.

I tried setting up the power cross feed on my lathe to cut it, but even after I outrageously rearranged the screw and stud gears and set the QC to coarsest possible thread, the best I could get was about 1/8" advance per revolution on the power cross feed.

CNC would make it simple...but is there a clever way to do it on manual machines?

07-03-2014, 06:46 PM
You might be able to put timing pulleys and a belt on the threading dial and the crossfeed wheel, and setup the ratios for the feed/revolution you need. But the dial moves rather slowly and the cross-feed needs to advance rather quickly. It sounds as if you are making a spiral for a self-centering lathe chuck. It might be difficult to get a good SFM to make the cuts under power, but maybe a spindle crank would work as it does for my square thread cutting. If you are copying an existing spiral, maybe you can disengage the cross-slide feedscrew and rig up a follower to ride in the grooves on the sample in the tailstock.

Just a quick brain dump - I've probably been reading too much roughage... :rolleyes:

There is more info on PM; do a search for lathe chuck scroll spiral. I found a wood turning site but it was about how to avoid cutting a spiral.


and right here (but long ago):


07-03-2014, 08:05 PM
I have seen one milled, the table was geared to a dividing head set vertical, i wish i had paid more attention but there was a banjo on the end of the mill table with change wheels, thats all i can remember at the moment, i know the guy so i will give hime a ring, which i was thinking of anyway

07-03-2014, 08:22 PM
The way it was done before CNC: You put a universal dividing head on a universal vertical mill and gear it to the main spindle. The dividing head faces "UP" .
As the machine moves forward (X) the spindle geared to the dividing head turns the part clamped in the dividing head chuck and you can produce any type of spiral. We used this a lot to make cams for screw machines.
The gearing depends on the type of machine you have and the type of dividing head being used.
We had a Nr. 2 B&S Universal with all the gears and a B&S Universal Dividing Head. The gears to use could be found in a Machinist Handbook,
or you could figure it out by yourselves. Dividing Head was 40:1 and the spindle on the machine was 1/4" per turn.
So if you gave the dividing head 40 turns to make the chuck on the dividing head make one full revolution and you geared it 40:1 to the spindle than you could cut a spiral advancing 1/4" per turn. All combinations are possible.
Today a CNC with live tooling should not have a problem cutting anything you need.
This is how the dividing head would be positioned. The chuck with the blank would screw on top and on the left you can see where the gears would be to make the connection to the machine table.

07-03-2014, 10:02 PM
I've got a 2-axis CNC mill and could probably do that in a few minutes for you. Where in Maine are you? Coastal near NH, no problem. North of Caribou, shipping would be best. :D

Rich Carlstedt
07-03-2014, 10:26 PM
You need to tell us what tooling you have at your disposal.
Do you have a mill, or an indexing head, or a rotary table?
Do you have a set of gears for your lathe headstock ?
What level of precision is acceptable ?


Jaakko Fagerlund
07-03-2014, 11:47 PM
CNC mill or a manual lathe like the Störebro we have at work, it can do threads like that.

07-04-2014, 12:20 AM
There you go! Ship it to Finland!:D

07-04-2014, 01:39 AM
Spiralling in at 1/2 inch per revolution- on my mill with .1 inch feed per turn of the dial, that would mean a 5 to 1 reduction ratio between the feed handle and the disc. What I might try is to first set up a pivot point in a t-slot. Then make a disc from mdf that can plant over this point. You can first use this setup to machine the disc so it's perfectly round. You also mount something round on the crank handle- the ratio of the diameters would be 5 to 1. Then you set up a temporary pair of idler pulleys such that a string wrapped around the larger disc can pass over these idlers and around the crank pulley.

A piece of dyneema or other similar high-tech fishing line can be fastened at its center point to the edge of the larger disc. Put a couple wraps of line around the disc, over an idler, and fasten to the disc on the crank (leadscrew). Put a couple more wraps from the other end of the line around the large disc, over the other idler, down to the smaller disc, pull tight and put about twenty turns around the small disc and fasten it. Now as you crank the table back and forth the larger disc will turn.

I would use the strongest fishing line that you can find. That might be 100 lb test, but the important thing is that it's not stretchy. Spectra might actually be the name of the fiber- it might be called Dyneema- there are other names that I can't recall, but they are all basically a high-tech strong fiber- dacron is another name. You might be able to get away using 1/16 inch steel cable instead, though it will have trouble going over small idlers, and it will take up too much room on the crank disc.

At any rate, the large disc you made is now a mounting pad for the disc you want to machine the groove into. Since the large disc has a hole drilled through it so it mounts over the pivot point, that hole can serve to center the workpiece.

You will obviously want to cycle the setup back and forth a few times to make sure the action is reliable and tight, and to set a starting point for the revolution of the large disc. You would also want to make sure the cutting force from the endmill tends to turn the disc against the tension side of the line so you are having to 'pull' the disc into the cutter. Also, you would want to withdraw the cutter, then recycle the setup before taking another cut to ensure that the groove you're making comes out properly- kind of like thread cutting.

07-04-2014, 03:14 AM
Another idea is to create a bevel gear drive from the X axis so a shaft can stick straight up. This shaft would normally not stick up above the table surface so it would not interfere with normal operation of the mill. A sprocket could be mounted and coupled to another sprocket mounted on the large disc. You select the ratio based on what result you are after. The large disc goes onto a pivot point which you secure to a t slot in whatever placement suits the length of coupling chain. Similar to the previous idea, but more practical. It's still a sort of redneck rotary table, but quite workable.

Ideally, the bevel gear drive from the leadscrew would have at least a few different, workable ratios.

07-04-2014, 06:10 AM
A friend of mine with a CNC mill has offered to do it for me (though thanks for the offer, PixMan). I'll probably take him up on it, but darryl, your #9 reply sounds like something I ought to try just to see if I can get it to work. If I wanted to be elegant about it, WM Berg has some round cogged belts that can change direction and would probably work.

Rick, I've got a H/V rotary table, a homemade diving head(horizontal shaft only), a 7x30 vertical mill, and a South Bend 10K lathe. I've got gears for the lathe headstock. I'd like to have the groove accurate to within, say, +/- 0.002". '

Forrest Addy
07-04-2014, 10:19 AM
You''re talking about making a scroll like the scroll in a three jaw chuck, a radial thread in effect.

You've already jiggered as much ratio out of your thread index train as you can but you need more. Your next step is to work out the cross feed machine ratio - the amount of radial feed per revolution of the spindle when the index is 1:1 from power shaft to spindle gear and work the ratio accordingly. You will find some limitations.

For one thing the power shaft driving the apron may spin faster than the spindle to get the radial advance per spindle rev you need. If the cross feed screw has a 0.200 pitch and you desire a 0.500 scroll pitch you have a 2.5:1 ratio right there. Multiply that by the crossfeed gear ratio within the apron. It would be nice if you could open up the apron and count teeth but decyphering the feed chart or a travel dial and a controlled rev or two of the spindle will get you pretty close to the radial machine ratio. You might - probably will - need some additional gearing.

Then there is tool design. 0.500 scroll feed at the small radius will require a bunch of radial clearance. Draw a diagram and work the math. You could get the gearing right and still screw up the job by dragging the flank. Make a trial blank to get your settings right before you cut the money part.

Oops! Adding: if you disengage the cross-feed to dial back for the next pass you will lose the timing - no half-nut. You will have to reverse the spindle to run the tool back to the origin. No biggie. There's only 4 revolutions plus the over-run.

Neat problem. I've cut several accurately pitched scrolls on a mill using the lead attachment and rotary table but never on a lathe.

07-04-2014, 01:56 PM
Forrest, you aroused my curiosity, so I checked to find out exactly what feed ratios the lathe has.

When the QC is set for 8tpi, the most coarse thread available without manually swapping the stud gear, Cross slide travel with power cross feed is 0.012"/rev, approx. I put a dial indicator on the cross slide and measured the travel as I rotated the spindle by hand.

So, I would need to set up the headstock gearing to run the leadscrew 0.5"/0.012" ~ 41-2/3 times faster than it does for 8tpi. That would certainly require a couple of compound gear sets possibly more, and I suspect one would want to turn the spindle by hand. With that kind of ratio though, turning the spindle by hand would be very difficult. All in all, it doesn't seem terribly practical, unfortunately.

Don Young
07-05-2014, 09:37 PM
When you have a leadscrew turning much faster than the spindle it is generally recommended that you drive the leadscrew and let the gears drive the spindle. This does require consideration of the necessary spindle torque for the machining being done so that the gears are not overloaded.