Single point depth of cut

I am trying to get to grips with my Rocketronics ELS ( threading) there are a few parameters I need to put into the controller before auto threading, pitch (metric ), ( if imperial tpi convert to metric) length of thread, depth of cut, angle of cut, it’s the depth of thread I am having trouble with, a google search turns up 6 or more formulas for working out, same on YouTube so I am totally confused ( not difficult at my age ) , if it wasn’t auto threading it would be a trial & error method cut try a nut cut and so on, I am sure someone on here will have a definitive answer.
Some of the clocks pre 1900 I do the manufacture had there own thread forms and they were made using thread plates and although I have some they don’t cover all manufacturers, it would be nice to also be able to work out a way to find the pitch and form of them as well , I know I can use a pitch gauge to find something near but is there a formula for doing it, for example did they all use tpi per inch or something else.
thanks Dell

Threads are complicated subject, and pre-standard threads are a complete muddle! I don't see any alternative to measuring their pitch and form.

I highly recommend Tubal Cain's "Model Engineer's Handbook" because it contains most of the technical data needed in a small workshop in digestible form. Section 4 covers standard threads: Whitworth, BSC, BA, Unified, Holtzapffel and Metric. Near the end there's a table summarising lathe infeed data for Metric, UNF, Whitworth and BA, note that internal and external threads are slightly different, and that threads can be sharp or rounded.

The infeed is related to Pitch, so step one with a TPI thread is to calculate it. If the ELS is programmed in inches, the pitch is simply 1/TPI. Otherwise, convert inch pitch to metric 1/TPI*25.4

The infeed varies by system, exact values in the book, but for an external thread the infeed is about:

• 0.6 x pitch for rounded, or
• 0.8 x pitch for sharp

I rarely cut big threads to exact specification, and - so far - they have all been metric. So I infeed by about 0.6p or a little more. Most fasteners are a loose fit; more care would be needed if I was targetting a tightly specified thread.

My approach to medium threads is to lathe cut them to about 0.5p and then finish off with a die. The lathe does most of the work and guarantees a straight helix; the die finishes the thread to correct form.

Not my thing, but I've successfully made the equivalent of a thread-plate for a non-standard thread:

• Determine the pitch and diameter of the wanted thread, usually by measuring it
• Set the lathe up to cut that pitch, or as close as the banjo & available gears allow.  (With luck it will be 'good enough' for a short thread
• Cut a sharp thread into a length of silver steel of the correct diameter.
• File or mill the silver-steel lengthways to make a tap and harden
• Tap drill a larger diameter disc of silver steel, countersink one side slightly, drill or file 2, 3 or 4 lengthways notches and use the home made tap to thread it. The disc, (or strip of gauge plate if a thread-plate is wanted), need not be as thick as a commercial die. Then heat harden.

Don't expect the result to be long-lasting or tip-top, but the tap and die will both cut provided the lengthways notches provide a sharp edge with some relief.

Dave

Edited By SillyOldDuffer on 21/05/2023 09:40:26

Frankly, Dell … I think the only way you can be sure of the thread pitch/form of any special screw is to measure it.

Ideally this would involve sectioning a sample but, if that’s impractical, there are work-arounds

Happy to discuss this further if you wish.

MichaelG.

Depth is very dependant on the tip of the tool used, unless you can accurately grind the very small tip radius for the given thread form then trying to put a number to the depth so the flanks end up in the right place is going to be near impossible.

Throw into the mix tool and workpiece deflection particularly with small threads, backlash, etc and things get even harder.

Edited By JasonB on 21/05/2023 10:02:36

Thanks for the replies

MG yes please what are the work arounds.

SOD I have ordered that book, yes I think I am capable of making taps and dies but it’s measuring said threads

JB I have only used taps& dies because most of what I do is either small BA or metric although both very similar but it’s more for the odd ball , I have both HSS and indexing and my understanding was that indexing would do a range of threads.

Dell

Quality inserts are generally ground to a specfication so they cut a book thread with book infeed. As do the Johannesson / SKF / Dormer 3/4 circle chasers I prefer when screw cutting external threads. Which makes life easy if you re lucky enough to have them.

Hand ground tooling will almost certainly be too pointy so extra depth is needed for clearance. Which can either be added as an empirical, usually works, factor as Dave does or you can try being a bit more scientifically investigative about things as I do when using the zero-to-zero threading method. Functionally zero-to-zero is pretty much equivalent to using an ELS for threading as you stop at a depth pre-determined during set-up. If that initial depth turns out to be too shallow I make successive slightly deeper passes until sufficient clearance is obtained for parts to screw together. Just like CNC and and ELS the zero-to-zero method lets me add feed in accurately determined increments so that once success has been achieved I can adjust the set-up parameters to compensate so all subsequent threads are right. In an important application I use increments to something close to the specified thread tolerances so the difference between the last doesn't fit and first does fit threads will be small enough that the does fit one will be within tolerance.

Alternatively you could cut flat bottomed threads where the root is flat rather than curved. The flat width being sufficient to encompass the correctly shaped thread from end. Using calculation and drawing board or CAD techniques the difference in depth between a sharp point and a flat of the correct width can be determined. As can the infeed depth needed. Creating the tool is a simple(?) matter of grinding a sharp point of the correct angles then flattening the end by the desired amount. Something that is easy to keep track of by measurement.

Clive

Dell it really depends on what inserts you are using. Full form will only do that specific pitch so you would need to buy a specific insert for each individual form and pitch. Partial form will do a range of pitches but the radius on the end is sized for the smallest pitch in the range so adjustment is needed for anything else and you would also have to do any rounding of the crests manually. They will tend to only come in the common thread forms so may not cover the unusual ones you mention

Even with the Flat ended method that Clive mentions it requires a correct width, which if you are mostly doing small threads could only be a few thou so not the easiest to grind, measure or determine your zero setting. So trial cuts are often needed to determine exactly how deep you need to go rather than just using a calculated depth

As Jason says even the flat end tool is by no means easy to grind in smaller sizes.

Objectively you are in micrometer adjustable jig territory. The great advantage is that measuring how much you have taken off the sharp pointed tool you start out from is relatively easy and, if the flanks were jig ground at the correct angle, the width must be right. So even if things don't work you know exactly what you have giving a reasonable change of figuring out what to do next.

Being able to reliably get "the same" wrong result is always a better start than wondering "what went wrong this time?".

But it all starts on the drawing board or CAD screen. Home Shop Guy hasn't a hope of measuring this stuff so all he can do is carefully work out what is needed then establish reliable techniques to do it.

Had a few "D'oh twot!" moments after carefully plotting out what I'd done on the CAD to prove that it was right only to discover the connection between the effects of what was done and correct was somewhat nebulous.

Clive

With the older threads, the problem is that some predate standards which were started by Whitworth. Also, some makers purposely used proprietry sizes to make sure that spare pasts were always supplied by them exclusively. I think the only solution would be to produce test threads on spare material and make careful notes as to which ones were the best size.

Once again thanks for replies

my test was only on a M8X1.25 as I have the required nut to test, I watched a Joe Pie video and he suggested that the flat on the tool should be approximately 1/8th of the pitch , as the HSS tool I was using had a sharp point that was probably the reason, so has Clive said that if said tool had a flat of the correct size ground on the end then the tool would need to go in further to give the correct depth, so it makes sense that if the flat ground onto the end of the tool removed say 1mm then the tool would need to go in that 1mm on -X, single point is all new to me but hopefully I am learning.

But the next problem comes with how much to grind the bit down and how to measure it.

Dell

There are comprehensive diagrams of most thread forms on either Wikipedia or here:

https://www.gewinde-normen.de/en/index.html

They will tell you exactly the form of the root and tip.

If you have an HSS bit, grind it to a sharp point as suggested above. Measure the overall length if the bit. Grind or stone a small amount off the end. Re-measure the overall length. There is a relationship between the two measurements, the included angle of the bit and the length of the flat.

Exactly as suggested above, you do not need to see the flat you have ground, just establish a reliable technique using measuring instruments you already have to infer the length of the flat.

Dell

The only way I've ever been able to get this sort of thing clear in my mind is to draw things out accurately as overlaid diagrams so as to see exactly what the dimensions need to be if things are to fit.

CAD makes this so much easier. And clearer if you use coloured lines. A decent CAD drawing will also easily give you the amount you need to take off the tip and find the length of tool plus flat tip that you will actually measure.

Clive

Double post deleted.

Edited By Clive Foster on 21/05/2023 15:22:19

If it is not a fine thread and you can determine the width of the flat you need, a quick and not all that nasty technique is by using a diamond slip together with a reasonably good several times magnifier. Compare the flat as you stone with the small graduations on a decent quality steel rule, or with the threads on a small screw of known pitch. It is possible to judge down to a flat of about 0.1 mm. It is then also feasible to round to a passable radius. You can combine this method with some of the measurement techniques suggested above.

There's a table in one of GeorgeThomas's books about how much to flat off for different pitches. Probably doesn't work for metric

.

First and best [for measuring male threads] is probably an optical projector [Shadowgraph or similar] … but note that for accuracy ‘telecentric’ lenses are required, so a home-brew version is tricky.

After that [for the small sizes that particularly interest you] a digital photo with a good macro lens, or a microscope, is a decent place to start … plenty of software available to measure images to ‘pixel-dimensions’ and to calibrate to real-world dimensions.

[ Again, a telecentric lens is most useful, but ‘needs must, when the Devil drives’ ]

If you only have the female thread available, then take an impression of it … using wax, resin, or a low-melting-point alloy.

Have a think about those, and shout if you need anything more.

MichaelG.

.

I will find a demonstration of telecentric lens optics later … need to put the shopping away now !

Edited By Michael Gilligan on 21/05/2023 17:09:41

[ Telecentric ]

For the non-specialist reader, this is likely to be ‘heavy going’ …. but the excellent illustrations are very informative, so just skim through the text:

**LINK**

https://wp.optics.arizona.edu/optomech/wp-content/uploads/sites/53/2016/10/Tutorial_Hu_Haosheng.pdf

MichaelG.

[ Shadowgraph ]

Classic versions, and modern alternatives: **LINK**

https://www.bowersgroup.co.uk/brand/baty

MichaelG.

I think that just for one thread form for one clock then the optical projector is wasted money , I need to have am easy way just to cut the one off thread and carry on using taps and dies for the common threads even if it means grinding HSS to suit , I have used peg wood in the past to cut a thread on to measure using pitch gauges..

MG I will have a look at the link you posted.

Dell

Perhaps one of those cheap USB microscopes and you could have a close look at the thread angles on the computer screen.