Thread Milling

[Anonymous]

Bob: Thanks for posting the videos, it's always interesting to see how other people tackle jobs.

Mike: Thanks for the link – I'll download the file and give it a go. Let us know how you get on with cutting for real.

Andrew

[mike TParticipant @miket56243]

Andrew,

Found a problem with the Chestnut pens Thread milling wizard. It climb mills external threads OK, but insists on conventional milling the internal threads using G02 from top to bottom. I talked with the author and he will bring out an update shortly to climb mill the internal threads from bottom to top using G03.

Mike T

[Anonymous]

I downloaded the program and gave it a very quick trial. In NCPlot it seemed to just generate a vertical line, even though the code clearly uses G02? However, NCPlot did barf when opening the G-code file due to no spindle speed commands. When I have more time I'll look in more detail and see if I can find what I was doing wrong.

By default the program works in metric – anybody know how to change to imperial?

Andrew

[mike TParticipant @miket56243]

That's very interesting but why?

The Chestnut generated G-code opens and display the helix path correctly in LinuxCNC.

LinuxCNC accepts 360 degree G02 segments. Some other software does not.

The Chestnut G-code has a G21 command to inform the machine controller, that the measurements that follow are Metric.

LinuxCNC can switch instantly between a metric and imperial display for the same program, and can accept G20 (inch) or G21 (metric) input.

The G20/ G21 G-code commands don't do the conversion. That's done in the Linux CNC controller software.

Hearsay has it that Tormach only works in imperial. That cannot be correct, can it?

You can always enter the metric equivalent of your inch i.e. multiply by 25.4 That allows you to create some unique threads. I am considering a special 1" x 1.0mm thread for an engine I am building. I enter 25.4 x 1.0 into the wizard and it does the rest. The 1.0 mm pitch is dictated to me by my available thread mills.

Mike

[Anonymous]

Posted by mike T on 14/01/2016 12:53:44:

LinuxCNC accepts 360 degree G02 segments. Some other software does not.

Ah, that may well be the issue; the I and J values did look a bit odd.

Hearsay is just that, hearsay. The Tormach works just fine in metric. I always program and run in metric, even if the part has been modelled in imperial.

Of course I can convert from metric to imperial, but for thread milling (exception to the rule!) I'd prefer to use TPI rather than an 'odd' pitch value. I think that the Tormach wizard varies the parameters between thread pitch and TPI according to whether G21 or G20 is active.

Andrew

[Nick HulmeParticipant @nickhulme30114]

Having read this I'm thanking the powers that be that my CAM just works 😀

– Nick

[Raymond AndersonParticipant @raymondanderson34407]

Hello Andrew, If you look at one of me albums titled Various heavy stuff you will see a piece of equipment made from Inconel 718, the 2 big holes and all the next size down were thread milled. [ although the threads start a bit down and are not visible on me pic ] The software was Siemens NX. I did see the thread mill the brother used and it had multiple teeth . I think it was made by Emuge Franken. When I see him I will ask and see what he did and maybe it might be of use to you.

cheers.

[John HaineParticipant @johnhaine32865]

Sorry to resuscitate this thread, but I can feel thread milling creeping up on me! I need to cut an M14x1 thread on the backplate for a collet chuck and found the turning tool I was planning to use won't quite fit. One option is to grind a bit off but there is much meat there anyway, and the tool lacks any top rake. I was wondering about making a tool from a tap then though, well, why not grind two flutes off and use my CNC mill to do the job? Interesting YouTube video here. Running the tap much faster will give a much lower tooth load and I shouldn't be so concerned with rigidity. It seems to me that I just need a tap for a 1 mm pitch which is smaller than the tapping size hole (13mm), correct? Obvious one is M6 but I may have a metric fine M8 or even M10 x 1 that could be used.

Anyone with any experience of doing this, please advise!

[JasonBModerator @jasonb]

I would have thought that the smaller you go with the modified tap the more the helix angle will start to become an issue and rub behind the cut .

Plenty of M14x1 taps about too.

[John HaineParticipant @johnhaine32865]

Found my invaluable tin of surplus taps had a nice M8x1 second HSS so it has shed 3 of its 4 flutes. Now to find out how to generate the code!

[duncan webster 1Participant @duncanwebster1]

Helix angle of 14*1 is 1.4 degrees, for m8*1 it is 2.3 degrees. As Jason points out you might be in for a disappointment. Grinding a single point tool to go down an M14 hole wouldn't be difficult, you could use a bar with an insert cutter (broken taps are my favourite)

[JasonBModerator @jasonb]

It is not so much the difference in helix angles between the finished thread and the tap used but the fact a thread mill has zero helix angle so there is no rubbing.

[Bob RodgersonParticipant @bobrodgerson97362]

I have milled plenty of threads on my CNC mill but I use the single thread type thread mills. They cost around £50 but work very well.

[MWParticipant @mw27036]

Might want to check out either Cromwell or cutwel tools for that kind of thing. I'd imagine most M.E suppliers wouldn't stock thread mills.

Michael W

[MuzzerParticipant @muzzer]

Fusion 360 supports thread milling, so that's one simple way to generate the code. I haven't got round to trying it myself yet but the cost of the tools is eye watering. On that basis, I'd want to be making my own tools first.

In Fusion, you can easily create your own form milling tools in the tool library, then use that to cut the thread.

If you are talking about a large diameter female thread that is effectively a very fine pitch, perhaps a standard internal threading insert tool would do the trick – used as a milling cutter. This sort of thing. All this discussion about taps, clearances, expensive single point tools etc would go away. Model it up as a milling cutter and off you go?

Murray

[richardandtracyParticipant @richardandtracy]

If you use Mach3 & possibly some other controllers, I've written a little program to do internal & external threads assuming a single point cutter (which could be made from silver steel). This is a windows 32 bit program.

Look forCNC thread milling here: http://www.chestnutpens.co.uk/misc/thread.html

Regards,

Richard

[Nick HulmeParticipant @nickhulme30114]

Most thread-mill manufacturers publish utities or web pages which generate thread milling code.

[John HaineParticipant @johnhaine32865]

Posted by richardandtracy on 02/01/2018 20:21:31:

If you use Mach3 & possibly some other controllers, I've written a little program to do internal & external threads assuming a single point cutter (which could be made from silver steel). This is a windows 32 bit program.

Look forCNC thread milling here: http://www.chestnutpens.co.uk/misc/thread.html

Regards,

Richard

Hello Richard, I have emailed you via your web page – John.

[BowberParticipant @bowber]

A few years ago I got 2 single point thread mills from America via Ebay for sensible money, I've not looked to see if they are still available though.

They work very well and I use the threading wizard in Mach3, my first one was a twin start M6 brass bolt and it fit perfectly, the great thing about thread milling is you can mess with the mess with the sizing to get a nice fit if it only mating with the one thread.

Steve

[Bob RodgersonParticipant @bobrodgerson97362]

Steve, that is what I find so good about using the threading wizard in either Fusion 360 or on the conversational programming on the Tormach mill. Adjustments are easily made but in general if I am using a standard recognised screw thread from a wizard it fits perfectly straight off.

[John HaineParticipant @johnhaine32865]

Well, there are a couple of YouTube videos of people successfully thread milling with modified taps so I reckon it's worth a go. Richard's excellent utility starts from the bottom of the holes and climb mills out, so I suspect it might not be so good with a modified tap as it will start cutting on all the teeth which could be quite a load! Best I think to write code that starts at the top and spirals down. Sir John also says near the top of the thread that you can use a tap. Worth a punt I think, on a test piece first. Will report back.

[John HaineParticipant @johnhaine32865]

Right! I generated the code using Richard's utility then hand-crafting the result to spiral downwards from the top, a relatively trivial change as it turned out (editing the gcode that is, not the utility itself). Drilled a 12.9mm hole in a miscellaneous bit of 3/4 mild steel bar, centred it on the Novamill table using my electronic centre finder, set the code running and bingo I had a threaded hole M14x1 about 5 minutes later. The thread looked very clean and fits the Unimat spindle well, first go, with little shake and a smooth action as you screw it on.

After some though I decided that the helix angle of the tap isn't really a problem. You have to remember that the tap is significantly smaller than the hole you are threading. Yes, in principle as the tap rotates the helix may cause some rubbing, but both the smaller tap radius and its form relief are quickly taking the cutter surface away from the work, as it were.

Thread milling rocks!

[BowberParticipant @bowber]

Well done, it's great watching the machine make such a nice thread isn't it.

The first time I used it was to correct a mistake when I accidentally used an M6 twin start tap I didn't even know I had so I had to create a brass bolt to fit.
I've been looking at jigging up a motorcycle cylinder head to thread mill the exhaust nut thread out to a larger size and make a new flange nut to suit but it didn't need to be done in the end.

Steve

[richardandtracyParticipant @richardandtracy]

Brilliant John.

Possibly I need to add a tickbox to the utility to tell it to mill the way you did it. Originally I had it working that way and changed it to climb milling because my cnc router/engraver can really only cope with climb milling.

Regards,

Richard

[John HaineParticipant @johnhaine32865]

That would be really useful Richard, enabling the use of cheap modified taps, though I'm sure proper cutters will give a better result. Thanks, John.

[Author]

Posts