Mach3 Lathe Threading Struggles

[mondrota]

Thank you 👍
Just before I go spending £££ on more stuff, there is this thing that keeps bugging me.
Like I said in the original post:
If I have the "Use Spindle Feedback In Sync Mode" checked, the program starts to run but pauses just before it is about to cut the thread and sits there waiting for something I assume.

From what I could gather reading forums, people say that this option should be ticked for threading.
Does anyone know why this is happening?

Thanks!

[battwell]

that was only tested on a few versions- it doesnt work in most as it wasnt succesful. only the spindle index pulse is used. (unless you get a motion controller)
the main reason for this is that the code is being processed in software- it has to see the pulses- calculate and pass the motion info on. this can take more than 1 slot of processing time- so it will always be done late. if it takes 2 processing slot time cycles because the pc is doing something- then its definately out of sync. - so it fails.
while these processing periods are very short time spans- the job is rotating fast- so it can make a big difference.
in hardware in a threading cycle- the interupt to the hardware processor is shut off- so all it does is the threading cycle- it can process the information in nanoseconds.

just today ive tested rigid peck tapping - which is the holy grail in the world of motion syncronisation. and it worked perfectly using the uc300 eth from cnc drive.com and using their uuccnc software . (which is my goto controller now for most things as it works so well!

[m_c]

What should happen with Mach3 threading, is the tool moves to the start point, it then waits for the spindle speed to stabilise, and then the threading move should synchronise with the spindle pulse.

However I did just remember, if Mach calculates that the axes can't respond quick enough to the spindle speed for the given move, then motion will just hang. It could be worth dropping the spindle speed down a good bit, and re-running the code.

[battwell]

multi slot indexing- does not work at all.
only single slot index. (and that index window has to be quite a wide slot- so it can be seen by the sensor in under 5ms.)

i widened the index slot on my boxford 125 to about 20mm long- and it would index every time. - but would still break tools etc.
i have to cut a new index wheel now- so i can run mine with uccnc. - next job once the triac is finished.

[m_c]

Just had a search, there is a quite a good threading guide here - http://www.machsupport.com/forum/ind...c,13017.0.html
However it doesn't cover that much of the setup, and even the main turn manual (http://www.machsupport.com/wp-conten...3Turn_1.84.pdf) is a bit sparse on details, other than saying the pulse has to be a minimum of 200 microseconds. Battwell is correct in that multi-slot doesn't work, so ignore that.

Battwell, the 5ms is likely to be the sensor response time, which is another often overlooked problem. I always used sensors from a reputable source with known response/trigger times. I've seen some sensors that have quite a long response time, and some from cheap sources give no figures, so are a bit hit or miss as to whether they work reliably. They also have to switch cleanly, which can be affected by non ideal sensors, and any optos in the signal chain (some BOBs use low speed optos, which may increase response times).

You just need to work through everything one step at a time.
Is the index pulse being fed back reliably?
You mention you have the RPM displayed, but is it accurate. Unless you're running closed loop, it should always be off from the requested RPM by at least a few RPM. From what I remember, Mach will show the commanded speed by default, not the actual speed.
Also, is the index LED going on and off on the diagnostic page when you move the spindle slot back and forth through whatever sensor you're using?

Are your axis tuned to accelerate/decelerate fast enough?
If they're set too slow, Mach will calculate they can't move fast enough, and just hang at any threads. Try running the spindle as slow as possible, and air cut a very small pitch thread. If it works, then check your motor tuning. Lathes will appear to run very well with low acceleration, it's only when you try threading that the poor acceleration will show.


If none of that shows a problem, then post on the machsupport forum. There are guys on there who know far better about potential problems than on here.

[Ger21]

There are plenty people who've successfully threaded with Mach and a parallel port.

And there are also plenty of people that haven't.
Last time there was a lengthy discussion about it on the Yahoo group, the general consensus was that it's broken, but does work for some people.
It apparently worked better on older versions of Mach3, which of course had other issues.

[magicniner]

And there are also plenty of people that haven't.

I'll ask Ian what version he uses which works for him.
One common denominator in his implementations is that he's not tight and buys good quality components, I suspect it makes a difference.