Thread Milling

[mike TParticipant @miket56243]

John Stephenson wrote

"You can also use a tap with all but one flute ground off.

One pitch cuts all if it fits into the hole."

John, how well does this work? Have you tried it? Is it really a viable method or wishful thinking?

Mike T

[Bob RodgersonParticipant @bobrodgerson97362]

Hi Andrew,

I have used the thread wizard in Path Pilot to make a thread on an induction pipe for a 1933 Sunbeam motorcycle. I measured up the thread from the lock nut that was on the original tube that was badly corroded. I couldn't believe how well it fitted without having to make any adjustments to the cutter diameter to change the depth of cut etc. OK it was an imperial thread 1 1/8" X 16 TPI but it worked great. I have tried it on one or two other jobs and it seems to be good.

[Chris Evans 6Participant @chrisevans6]

Oh gosh I and J. When I first went on a course to learn how to use a wire cut machine in the early 80s it made my head hurt. It took me weeks to understand it. Most thread milling operations produce a slightly deformed helix angle but not enough to worry about.

[mike TParticipant @miket56243]

I asked how well a single point thread mill made by grinding off all but one flute of a conventional HSS tap would work. The answer is remarkably well. Some of the cleanest threads I have cut.

I mounted the work piece in a rotary table and the home made single point thread mill in the spindle. The RT rotation is synchronized to the downward Z axis movement of the head by the single line command G01 A-3600 Z-10 F1. This cuts ten turns of thread at 1.0mm pitch into a blind hole, did not even need to run a tap down the thread to clean it up.

Jobs a good un.

Mike T

Edited By mike T on 10/01/2016 15:47:43

[Ian PParticipant @ianp]

Posted by mike T on 10/01/2016 15:46:59:

I asked how well a single point thread mill made by grinding off all but one flute of a conventional HSS tap would work. The answer is remarkably well. Some of the cleanest threads I have cut.

I mounted the work piece in a rotary table and the home made single point thread mill in the spindle. The RT rotation is synchronized to the downward Z axis movement of the head by the single line command G01 A-3600 Z-10 F1. This cuts ten turns of thread at 1.0mm pitch into a blind hole, did not even need to run a tap down the thread to clean it up.

Jobs a good un.

Mike T

Edited By mike T on 10/01/2016 15:47:43

Mike, I am not conversant with G code or thread milling and do not really understand the process fully. However, if the RT and the Z axis motions are controlled does the single point cutter traverse a path that is identical to what screwcutting an internal thread in the lathe would be?

If it is the same then presumably the full depth of thread is done in several passes otherwise I cannot see how what is left of the original tap would be strong enough.

I can sort of visualise the single point cutter (with its cutting radius very small in relation to the hole size) rotating at speed and then following the correct helical path, 'milling' the threads but I would imagine that an ordinary tap might not have the exact profile for milling purposes?

Ian P

[mike TParticipant @miket56243]

Ian

Correct, the thread mill diameter needs to be smaller than the hole, but not by much. Unlike a lathe, the single point thread mill is rotating and cuts a 60 degree Vee in a helical path down the hole. The speed of rotation of the cutter is fast and the feed along the helix ( rotation plus Z motion) is slow. very little material is removed for each revolution of the cutter. i.e. the chip load is small.

It should be possible to go to full depth in one pass but I have not tried it yet. The single point of the modified tap survives because the chip loading is so small.

The thread of a modified tap will never be quite as perfect as a £70 thread mill cutter but it works adequately. When I use this method in anger, I will mill the thread slightly undersize and finish the thread with a full size bottoming tap.

Mike T

[mike TParticipant @miket56243]

Ian,

Forgot to add, that line of G code simple says rotate the RT 10 times while moving the Z axis down by 10mm and that produces a 1.0mm pitch thread. Change the sign from minus to plus give you right or left hand threads

Mike T

[Anonymous]

Chris: Not sure I see how thread milling causes a deformed helix angle? I can see how the thread form might be slightly off, depending upon the geometry of the cutter. But as far as I can see the helix angle is set by the feed parameters and therefore takes its accuracy from the machine tool?

Mike T: What feedrate type are you using? With Mach3 I found that normal mm/min feedrates were a fantasy when combining linear and rotary axes. The only thing that worked for me was inverse time feedrates.

Andrew

[mike TParticipant @miket56243]

Andrew

I am with LinuxCNC and it appears the feedrate defines the linear axes motion and the rotary axis keeps pace.

I used 1 inch per minute linear for the Z axis motion, but it would probably go much faster. I don't want to be to brave as the modified HSS tap milling cutter only has one tooth and I have still to do the real job.

Chris, The helix will be exact but the 'vee' form may be slightly out, more so with a cheepscate modified tap cutter

Mike

Edited By mike T on 10/01/2016 17:37:49

Edited By mike T on 10/01/2016 17:43:19

[Chris Evans 6Participant @chrisevans6]

Andrew/Mike. You are correct it is the vee form not the helix angle, old age and brain fade apply.

We used to cut threads on a Hurco mill with a home made single point cutter very effective to.

[Ian PParticipant @ianp]

Posted by mike T on 10/01/2016 16:46:03:

Ian

Correct, the thread mill diameter needs to be smaller than the hole, but not by much. Unlike a lathe, the single point thread mill is rotating and cuts a 60 degree Vee in a helical path down the hole. The speed of rotation of the cutter is fast and the feed along the helix ( rotation plus Z motion) is slow. very little material is removed for each revolution of the cutter. i.e. the chip load is small.

Mike T

I see in one online catalogue that thread milling cutters are available down as small as M1.6!

Presumably there are no 'home workshop' CNC milling machines that are accurate and repeatable enough for that sort of thread size?

Ian P

[Anonymous]

Mike T: Thanks for the explanation. It looks like LinuxCNC does what it is supposed to do, ie, combined linear and rotary motion feedrates are in mm/min (or iches of course). Now that I've upgraded to Tormach PathPilot I'll have to do some experiments and seem what happens. The threading mill wizards in PathPilot also look sensible, so in due course I'll give them a go. I can't remember if there were any thread milling wizrads in Mach3, but the other wizards were such a mess that I never felt inclined to use any of them. The thread milling 'function' in my CAM program is also a fantasy so up until now I've been faced with writing my own code.

Andrew

[mike TParticipant @miket56243]

Andrew

I am not sure if I actually helped you as we are both doing completely different things. I rotate the A axis and down feed on the Z axis, the feed rate appears to control the linear Z axis. I am NOT doing helical interpolation like you in X, Y and Z. I rotate the work piece while you spiral round the outside (or inside).

I am trying to get Pathpilot running on my Linux setup. It looks to be a first class control panel and the wizards look exciting. Pathpilot and LinuxCNC are basically the same thing, Pathpilot has gone one stage further

Mike

Edited By mike T on 10/01/2016 19:31:46

[Bob RodgersonParticipant @bobrodgerson97362]

Hi Mike, the wizards in path pilot are pretty good. I occasionally hijack and modify them to suit my needs. The last one I did was for a tapered bore. I have just finished making a timing sprocket that has an internal thread that was done using Path pilot wizards. I will be posting this on You Tube in the next day or two.

[Anonymous]

Mike: Indeed I will be using helical interpolation for thread milling. However, your information has definitely helped, as I had all sorts of trouble with feedrates when trying to 'thread' mill a worm using the 4th axis. Like you the required movement was rotation and linear in one axis, X in my case as the rotational axis was horizontal.

Andrew

[MuzzerParticipant @muzzer]

Posted by mike T on 10/01/2016 19:13:20:

I am trying to get Pathpilot running on my Linux setup. It looks to be a first class control panel and the wizards look exciting. Pathpilot and LinuxCNC are basically the same thing, Pathpilot has gone one stage further

Good luck with that Mike! If you look on the LinuxCNC forum you will see that it is considerably more complex than grafting the PP GUI onto a more general LinuxCNC install. Unless you are very experienced in both Linux and LinuxCNC, you would be best to wait until the experts there have done the work.

I naively bought the restore DVD from Tormach (they are happy to supply to non-Tormach owners) and discovered that it's an image of the Tormach controller installation, not any kind of setup disk. Although there are examples of systems that have been apparently "hacked" successfully, they aren't very robust and lack many critical features.

At first glance, these apparent hacks may give the impression that there isn't a lot left to bottom out but they are examples of the 80:20 rule or possibly even a 90:10 rule. The remaining 10% will take 90% of the time and effort. Try LinuxCNC Features in the meantime if you fancy a better looking GUI with conversational functions. That's what I plan to do until the higher beings have brought PP and LCNC together for us.

Murray

[mike TParticipant @miket56243]

Murray

I expect we have all bought the Tormach restore DVD. I expect we have all hit the same disappointments. All we can now do is wait until the real Gurus bring it together. But Pathpilot looks so good.

I will dig around LinuxCNC Features, as you suggest, and see where that leads

Mike T

[Martin ConnellyParticipant @martinconnelly55370]

Drawing of a drive part.

**LINK**

Item 6 being machined. Ø33mm 16tpi UNC thread. I know it is far from standard but that is what was required, using 316L stainless pipe as raw material. The tool is home made using Horn inserts. Hand written Gcode with G03 as the code.

**LINK**

The finished item between the two parts it joins.

**LINK**

The drive is driven from one end and braked at the other and a left hand thread was required to ensure it tightened rather than loosened because of the applied torques.

The issue of helix angle and internal thread milling has been covered in the past by manufacturers and users of tooling and the figure quoted as a rule of thumb for not causing a problem is that the tool is 70% of the finished thread size as a maximum. This fits in closely with the 2mm thread being cut with a Ø1.55mm tool.

Martin

[mike TParticipant @miket56243]

Andrew

I have a copy of the Tormach Pathpilot install disc. It installs OK and gives a Sim screen, but obviously nothing moves as I do not have the Tormach machine. I would like to play with the thread milling wizards to see if the will produce Gcode that I could use elsewhere. Do you know if the wizards will produce and save Gcode in Sim mode?

When I try to save the thread mill wizard, I get an error message " Please fill in XY locations in drill table then return to thread mill and post" I an not sure what that means. what/where is the drill table? Can you explain if you have a moment spare.

Thanks

Mike

[Martin ConnellyParticipant @martinconnelly55370]

**LINK**

This video shows a Vardex M6 milling cutter being used to cut an oversized thread for an insert. The material is an aluminium alloy and the G-code for the cutter movement was generated by a program downloaded from Vardex. You tell it the tool part number and a few other parameters and it produces the code. This can then be used on its own or cut and pasted into a program. In this case there was a PCD wrapper around the Vardex code so that the holes were each at x=0 y=0 for the threading process so the Vardex code could be used at any point designated as 0,0.

The code has a circular approach and retract from the centre of the hole to the cutting radius and uses two passes. I did not check the code but I suspect that it was cutting equal volumes at each pass.

Martin

[Anonymous]

MIke: I'm afraid I can't help with the PathPilot sim mode. I didn't know it had one! Presumably if it doesn't get a response from the machine when the 'reset' button is pressed it goes into a simulation mode?

As for the thread milling wizard I had a quick play this morning as I was wondering the same thing. It turns out that the thread milling wizard takes its X-Y positions for the threads from the drill table in the conversational wizard for drilling. It may have been nicer if the wizard was self-contained, but for small internal threads at least it may well be that the drill table is already filled in.

Hope that helps.

Andrew

[mike TParticipant @miket56243]

Andrew

I have downloaded and tried the Thread Milling Wizard from Chestnut pens http://www.chestnutpens.co.uk/misc/downloads.html

Who would have expected to find a thread milling wizard there?

It is quick and easy to use, the wizard is simple, well laid out and everything is on one page. The G-code saves and loads into LinuxCNC without a problem. It cuts air beautifully. The circular moves are in 360 degree steps.

Appears to be a very user friendly thread milling G-code generator

Time to thread some metal.

BTW I have discovered that Pathpilot opens automatically in Sim mode if it cannot find a machine. You can then use all the wizards, save the G-code files etc. and do everything except cut metal.

Mike T

[Bob RodgersonParticipant @bobrodgerson97362]

 

I finally got round to adding some video of me making a sprocket for a 1920's Sunbeam motorcycle. There is some thread Milling in there somewhere.

Part 1

Part 2

Part 3

Part 4

Edited By JasonB on 12/01/2016 18:29:25

[MuzzerParticipant @muzzer]

Hi Bob

Thanks for taking the time to make the video and post it here, warts and all. It's a learning process!

Hadn't realised how big the Duality actually is.

Murray

[Bob RodgersonParticipant @bobrodgerson97362]

BobHi Murray, Basically the nDuality lathe is the same as a Seig SC3. I've just finished making the puller to go with the Sprocket, another thread milling job.

[Author]

Posts