Is it the formula you need help with, or writing the spreadsheet, or both?

You can work out the X-Y coordinates of the surface from the formula for a circle (X^2 + Y^2 = R^2) where the origin is the centre of the arc.

It's easiest to work with a round tool (e.g. a pattern following tool or a carbide button).

Translating the surface coordinates of a concave surface to the centre point of a tool of radius r then boils down to scaling the X & Y coordinates by R/(R+r).

You can then choose a known reference position and offset the coordinates wrt this to get your cross slide and feed readings. The devil is in the detail in getting the sign conventions correct!

I used this method to turn some accurate curves in my model jet engine – there's a fairly detailed description part way down this page

Intake Nozzle

Link

I find it easiest to set the top slide parallel to the bed and use this for the Z feed, rather than the carriage. I set a stop on the lathe bed where the tool just touches the face of the part and zero the top slide dial. Cross slide dial is zeroed by touching off on the OD. I can then wind the carriage back, increment the cross slide and set the desired Z travel on the top slide without cutting any metal whilst making the adjustment.

I have also sent you a PM

Andy

Edited By Andy_G on 21/03/2022 13:57:13

Dave

Here is a starting point in mm

Emgee

Do your smoothing with a round graver, much more control and vision about what's going on.

Unfortunately, while it's pretty simple trigonometry to work out the coordinates of the curve, those aren't quite the coordinates that you need to machine said curve! Possibly not even good enough (given that this curve swings through near 90deg) for this cosmetic-not-bearing-surface curve. The reason is that in order to position the tool, assuming that you are using a circular button tool, you need the coords of the centre point of the tool. The actual contact point – where the cutting takes place – is a bit more difficult to calculate than just the curve itself as there is an offset of tool position from the curve that depends on the curvature of that curve at a given point. At the largest end of the curve you are using the side of the tool so need to offset along the lathe axis while at the small end this offset is near zero but the infeed offset is now maximum – and these change all the way along.

It's unfortunate that the OP is not a CAD user. I reckon the easiest way to get the required list of coordinates is to draw the profile in CAD and use its CAM module to calculate the path. I guess you could do this by generating the lathe tool path needed although not having any experience of doing that, I would pretend that the profile is going to be machined on a mill, specify a tool of the diameter of my lathe tool button, and generate the gcode accordingly. It's then easy enough to edit out the XY coordinates from the gcode and put that into a spreadsheet – or just print as text. I'm sure I could do the work needed to come up with a formula for the correct tool path manually but it's very much a case of letting the software and the PC take the strain, and a whole lot less error-prone!

For doubters, I (and plenty of others) have taken this path to get "manual numerical control" coordinates before; I use the technique to machine loco wheel flanges because I'm a whole lot better with CAD/CAM than I am grinding a form tool… A DRO on the lathe helps a lot as well.

No argument, Andy – I was thinking "general case" but if you are cutting a truly circular arc, then the tool path follows a similar arc struck from the same centre but reduced by the radius of the cutter. I had completely missed the "special case" nature of this one where the sums actually become very easy. The technique that I described is of use for anything other than a circular arc – possibly for aesthetic reasons it is a part-ellipse, for example. My loco wheel flanges fall into this category. All the same, personally speaking, I would probably still use the CAD/CAM route, justified by this quote from Leibniz:

"It is unworthy of excellent men to lose hours like slaves in the labour of calculation which could safely be relegated to anyone else if machines were used."

I guess that it's the difference between needing to look for an elegant solution to avoid lots of calculation or similar effort, and just throwing lots of CPU cycles at a brute-force solution!

In practical use on a manual machine it's often easier to use the side of the tool as the ref that way you simply touch the tool and set your handwheel or DRO.

So for Dave'd job he needs to generate the curved surface with a series of cuts from his button tool. I do hope it's a RCMT06 or RCGT06 as that's what I have worked it out for.

First turn your stock so it looks like this and then mount up your button tool. With topslide set parallel to lathe axis touch against the diameter and set your cross slide handwheel or DRO to zero. Then touch the side of the tool against the face and set handwheel to 0.088. EDIT 0.082

Then wind in the topslide to 0.000 and feed tool in 0.375. Topslide to 0.025 and feed in to 0.375. etc After a while the cross slide feed in will start to reduce but just keep winding in the topslide in 25thou increments as per table. The last cut will be with the dial reading 0.082

This is what it takes to get the dims in the table, did someone mention cluttered drawings

Edited By JasonB on 22/03/2022 07:11:20

You could also machine the curve on a milling machine with a rotary table and a 3/4" dia cutter