Screwing without screwing up.

[tonyfoale]

I have recently been converting my lathe to electronic control.

Click for full size

It is more than an ELS (electronic lead screw) but in some eyes it is less than CNC. I did not want to be hindered by a full CNC - Start the computer, use a wizard, write some G code, use the MDI or make a drawing and pass it through CAM to make a simple item. Not for me.

A while back I made a post about changing the cross slide screw to a ball screw
Lathe cross slide conversion to a ball screw

I liked it so much in use that I decided to do the same for the Z axis. However, putting a hand wheel on the end like the cross slide is impractical to use unless you have a very short lathe. I don't. That meant that it had to be motorised and then it had to be controlled. if the Z axis is motorised and has controls it would be daft to not do the same to the X axis. I call this mission creep.

Now I have all the mechanical stuff needed for a CNC conversion but I did not want a full CNC. However, it seemed like it would be simple enough to use a microcontroller and a few buttons to automate a few standard operations to a CNC level without the setup hassles.





The above is just the intro to what this post is about. I shall be making a video series showing details of all aspects of the conversion but you will have to wait for that.

Multipass screw cutting was incorporated into my dedicated software to control the ESP32 micro. Initially for testing I used the same DOC (depth of cut) for each pass. Anyone who has done lathe screw cutting knows that will result in very little metal removal on the first passes and excess removal on the last passes. So last night i sat down and worked out what DOC each pass needed, to ensure the same amount of material was removed on each pass. Obviously the first pass needs more DOC than the final cut. Here is the derivation, I will point out that for simplicity it is based on the assumption that the total thread depth is small compared to the workpiece diam. Here is the derivation that I came up with;



I programmed this into my system and did some tests. For a given thread depth and number of passes the even amount of metal removal per pass gave a smoother lathe operation and the final finish was better. The better finish is due to the smaller DOC on the last pass. I made a spread sheet which allows a selection of passes and thread depth and which outputs the DOC for each pass, this is applicable to manual lathe screw cutting and is the main purpose of this post. If all went well the spreadsheet should be attached. just enter the thread depth (in any units) that you want and the sheet will calculate the optimum DOC (in your input units) for each pass for total number of passes from 4 to 9.

To see the effect of using different DOCs for each pass let's use 6 passes on a thread depth of 1. Refer to the spreadsheet.
If we used the same DOC for all passes that would have to be 1/6 = 0.16666. using the spreadsheet we see that the optimum would be 0.408 for the first pass but only 0.087 for the final pass. The final pass would have approximately 1/2 of what it be with constant DOC for all passes. The first pass would cut more than before with a depth of 0.408.

just testing.

Keep watching there is a lot more to come.

[NortonDommi]

Thank you for that helpful spreadsheet Tony, much appreciated.

[metric_taper]

I interested if the video shows how you attached a spindle encoder so you can keep the thread timing. I'm hung up on putting an encoder on my big lathe (it has a 100mm OD spindle shaft, so I'm thinking a timing pulley with belt to the encoder shaft). I want to see if I can make a software program that uses an encoder on the feed screw as well, with the intent of enabling metric threads, where I can disengage the half nut, and get a timing signal from a LCD screen for when to engage again. It gets tiresome to reverse it back to where the carriage was, for all these threading passes. My lathe has both Imperial and Metric threading gears with just the flip of one lever. But the feed screw is Imperial. Which is odd with European style metric headstock taper (and delivered to the USA).

[dagrizz]

Now that'll be useful even without electronic controls! Danke!

[DIYSwede]

Thanks Tony - yet another brilliant aid, both the spreadsheet and its derivation!

This is one of these machining problems I've "just haven't gotten myself into yet",
just lessening the repeated DOCs on a somewhat intuitive "hunch"
(which with 20-20 hindsight was way off - took too big a bite in the last passes).

Following your derivation was to me a spiritual experience - but then I'm just a cheapskate!

Ta

Johan

[tonyfoale]

I interested if the video shows how you attached a spindle encoder so you can keep the thread timing. I'm hung up on putting an encoder on my big lathe (it has a 100mm OD spindle shaft, so I'm thinking a timing pulley with belt to the encoder shaft). I want to see if I can make a software program that uses an encoder on the feed screw as well, with the intent of enabling metric threads, where I can disengage the half nut, and get a timing signal from a LCD screen for when to engage again. It gets tiresome to reverse it back to where the carriage was, for all these threading passes. My lathe has both Imperial and Metric threading gears with just the flip of one lever. But the feed screw is Imperial. Which is odd with European style metric headstock taper (and delivered to the USA).

If you look at the pdf referenced in
Improving a lathe spindle head.
you will see how I fitted a magnetic pickup inside the head of the lathe for a cheap tacho, the type that many on this forum use. Of course that is not a solution for everyone because it is rare to have an empty headstock.

This pickup only gives 1 pulse per spindle revolution and the usual reaction is "that is not enough" but it is what the tacho works with. I did an error study using different number of pulses/rev. and concluded that 40 would be a good number. My plan was to 3D print a notched wheel and sandwich it behind the drive pulley.

Click for full size.

These pix show the notched wheel to get RPM and direction for a swirl meter on my flow bench. For the lathe I was planning a much larger version with 40 teeth and a large centre hole, which would fit over the rear of the spindle and clamped behind the pulley as shown here. Then I would use an optical sensor like the one in the above pic. to get the signal pulses which I would pass through a comparator to sharpen the pulses.



The Mach3 CNC software requires only a single pulse/rev for screw cutting, other systems use precision rotary encoders with 1000s of pulses/rev.
When I analysed what you will do with the pulses I concluded that there was no point to having a very large number. The purpose is to get the time duration between pulses. A single pulse gives the duration of a single revolution, multiple pulses just chops this up into smaller periods. Using single pulse only allows you to calculate the average speed over one revolution but there are several factors which cause the speed to vary over a revolution, such as eccentricity in the spindle and motor pulleys, lack of roundness in the pulleys, lack of homogeneity in the belt/s, beating between motor and spindle, the list is long. Multiple pulses per rev allow the speed variation over a revolution to be accounted for in the calculation of the required carriage feed. The questions are; Is the speed variation over one rev significant? If so, then how many pulses do we need to smooth it out.

Simple turning or facing would be quite tolerant of spindle speed over a revolution but screw cutting was the critical task. Mach3 were happy with one pulse/rev. As I already had the speed sensor on the lathe I thought that I would see just how good a job could be done with it. The first test threads were by no means excellent but the variation seemed to be from rev to rev not over a single rev. Examination of the pulses from the magnetic pickup showed that it was not firing in exactly the same spindle position from rev to rev. Good enough for a tacho but not for this job. I have noticed this type of variation in hall effect engine ignition systems so it was not a surprise. To get precise spindle location I added a short vane to the rotor on the spindle and made an optical pickup to fit where the magnetic one did.



This gave very accurate info about the spindle position once per rev. The threads cut with this were excellent, particularly when I built the optimised depth of cut into the software. I see no reason now to continue with the original plan of the notched plate with multiple slots. I have no need to measure direction of rotation, because that is set by a switch. Otherwise it is only a question of having two optical pickups instead of one.

There are stacks of videos on the net showing the mounting and belt driving of off the shelf optical encoders if you want to continue down that path. On youtube channel Clough42 there is a long running series on a electronic lead screw conversion which I think shows the encoder mounting.

I think that a lot of the benefit of my system is due to the precision of the ball screws in place of the original ACME thread and half nuts. I suspect that the limitations of the stock screws/nut exceed the limitations of a single pulse/rev.

I will go into all this stuff and more in the planned videos. I have filmed a lot and it is a big project to describe so it will take a few videos to do that. I will make a quick intro video soon showing screw cutting.

Oh BTW. One way to get closer to constant spindle speed over a revolution is to run the spindle fast and let inertia help. Because the electronics are in control I can run much faster than you would dare by hand. My testing has all been above 1000 rpm.

[tonyfoale]

I forgot to mention that I treat the feeds for screw cutting in the same manner as for turning. So i might set the feed/rev at 0.05 or 0.1 mm/rev for turning. (I can set that in steps of 0.01mm/rev) and say 1 to 5mm/rev for screw cutting. There is no difference in method between metric and imperial. e.g. if I want a 26tpi thread, that is a feed of 1/26 = 0.0385"/rev or 0.98mm/rev. So I would set a feed of 0.98mm/rev.
The only difference between normal turning and screwing is that in the screwing mode as the depth of cut is increased on the X axis I have it programmed to advance the Z axis in accordance with the thread angle. I only envisage using 60 deg threads and so the Z advance is tan(30) or 0.577 times the X advance. Of course any thread angle could be programmed in but that would need an additional operator input and I like simplicity. I am also running out of pins on the ESP32 micro.

[tonyfoale]

Here is a pic of the pulses from the optical pickup. The camera speed caught more than one pass, the lateral displacement of the two pulses is due to operator camera shake not variation in the timing point.

[DIYer]

Thanks tonyfoale! We've added your Screw Cutting DOC Spreadshet to our Machining category,
as well as to your builder page: tonyfoale's Homemade Tools. Your receipt:

Screw Cutting DOC Spreadshet by tonyfoale

tags: machining, calculator