Thread Milling

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

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.

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

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

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

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

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

**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

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

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

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

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

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.

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

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

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

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

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

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

- Nick

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.