Speed Reduction Angle Head

[CrossfireX]

HI Everyone,

I'm building a Right Angle head for my mill to, basically, use it as a horizontal borer. However, due to my mill being 1:1 (motor:spindle) and I often do larger bores, I'm gearing down the angle head 2:1 as I'm usually boring at 60-150 RPM. My Main question is, and I know there's a couple of people on here that will know the answer but I thought I'd leave it open, can I use a gear selection in in the software to trick the system into thinking I'm in low gear (and Reverse) when I attached the Angle head?

The main concerns for wanting to do this are:

1. Rigid Tapping (although I am aware I can just use a different Speed and Q value, and use G74 instead of G84)
2. Tool retraction during G76 Boring Cycle (although I am aware this is a luxury and not specifically required)
3. Correct feed rates in conjunction with the feed override knob etc.
4. Reduced likelihood of error in the above examples, and when drilling, boring, milling, etc. (I will be far less likely to make an error if I can just tell it to use low gear, and program normally, as opposed to calculating everything every time with different speeds and feeds (an spindle direction)..

I guess the next part of the question is: If the encoder in on the motor (which it is) and I have a 2:1 reduction in the angle head, when I do an M19, will it still randomly stop at either point 180 degrees apart, or is there a way to get it to stop in the same position each time. This will be mostly important for tool retract in g76 cycle, but I imagine will be equally as important with tapping cycles If I needed to go back into the hole for any reason.

Feel free to tell me I'm an idiot.

Thanks in Advance.

Jason

[cncsnw]

Yes, since your mill does not already have a back gear that you need to account for, you can just treat the angle head as the low gear range. In your example, you would set Parameter 65 = -0.500. If you do not want to install a "low range" detection switch, then you can program one of the Aux keys to be a range selector/indicator.

Yes, spindle orientation will stop at the first index pulse that comes around, and therefore it will be unpredictable which of the two positions it will end up at.

As far as I know, the tapping and boring cycles only work along the Z axis. However, you could experiment with M333. I think the syntax is something like "M333/X/Z/Y" or "M333/XZY" or similar, to make Y do the work of Z and vice versa.

If you can get rigid tapping to work along a horizontal axis: you would need to add 16 to parameter 36 (e.g. set it to 17) so that the control will compensate for the unequal ratio and direction between the encoder and the spindle, in low range. Peck tapping or otherwise reentering the same hole will not work, because your encoder index pulse will come around twice per tool revolution.

Feed rates and feedrate override will not be affected one way or the other. Outside of rigid tapping, all milling feedrates are time-based, and do not depend on spindle speed.

If the G76 boring cycle, or something like it, is a high priority, then you could install a prox sensor on the right-angle head, to detect something that really does come around just once per revolution of the tool. Then you could write an alternate M19 that runs the spindle at a slow RPM; waits for that sensor to trigger; and stops the spindle. It would not be exact, but it would be close enough to get the boring tip clear of the wall.

[CrossfireX]

Thanks CNCSNW, I knew you would know the answer for sure.

Before I get into the bones of it, I currently send some stuff out to a guy in town who has a gantry mill converted over to a GSK controller. I know he just uses G19 in his canned cycle to do his drilling and tapping, for example:

G19 G81 Y120. Z120. X-30. R5. F350.

Or:
G19 G84 Y120. Z120. Q1.5 X-25. R5.0

If I can get this working, I won't need to send anything out to him any more unless it's over 3metres long. It's not so much about the cost of sending it out, but about being able to do it in my timeframe and also having complete control over the quality.

Yes, since your mill does not already have a back gear that you need to account for, you can just treat the angle head as the low gear range. In your example, you would set Parameter 65 = -0.500. If you do not want to install a "low range" detection switch, then you can program one of the Aux keys to be a range selector/indicator.

Perfect, I'm happy with that outcome.

Yes, spindle orientation will stop at the first index pulse that comes around, and therefore it will be unpredictable which of the two positions it will end up at.

Exactly as I assumed...

As far as I know, the tapping and boring cycles only work along the Z axis. However, you could experiment with M333. I think the syntax is something like "M333/X/Z/Y" or "M333/XZY" or similar, to make Y do the work of Z and vice versa.

Where can I find out more about M333? I checked the manual and it simply says it's experimental. Do you do this at the start of program, in the setup, or is it done in the sequences somewhere?

If you can get rigid tapping to work along a horizontal axis: you would need to add 16 to parameter 36 (e.g. set it to 17) so that the control will compensate for the unequal ratio and direction between the encoder and the spindle, in low range. Peck tapping or otherwise reentering the same hole will not work, because your encoder index pulse will come around twice per tool revolution.

Would I need to change this every time I connect the angle head? or would this only relate low range? also, would halving the thread pitch in the canned cycle achieve the same thing? for example; if I'm tapping a 2.5mm pitch, would I put a Q1.25 in the canned cycle? or would altering Parameter 36 solve for this when in "low range"?

Feed rates and feedrate override will not be affected one way or the other. Outside of rigid tapping, all milling feedrates are time-based, and do not depend on spindle speed.

Understood.

If the G76 boring cycle, or something like it, is a high priority, then you could install a prox sensor on the right-angle head, to detect something that really does come around just once per revolution of the tool. Then you could write an alternate M19 that runs the spindle at a slow RPM; waits for that sensor to trigger; and stops the spindle. It would not be exact, but it would be close enough to get the boring tip clear of the wall.

I do use G76 a lot to get a good finish, but if I had to sacrifice it to get this working, I could switch to using G81 or G85 for boring, and just compensate accordingly. it's not ideal, but If I had to I would.

assuming I wanted to add a sensor, and have it on a connector, how would I go about using an alternate M19?

assuming all of the above, and saying it's worst case scenario that I cannot use G84 or G74 on the X or Y axis, could I use a floating tap holder and use a G85 for tapping? I've never used one but I assume I would have to use M109 to disable feedrate overrides??? IF it's what I have to do, I will.

[cncsnw]

As far as I know, Centroid does not change the plane of canned drilling and tapping cycles when you use G18 or G19 to change the circular-arc plane. You could experiment, though, to find out.

If I recall correctly, I was told that M333 was implemented for multi-head routers with parallel Z axes. You could apparently use it to make a second Z axis (perhaps labeled 'W') respond to Z commands in lieu of the primary Z axis.

I have never experimented with M333, and to the best of my knowledge there is no more documentation than what you saw in the manual. Your primary source of information is probably going to be trial and error.

You set Parameter 36 once, for all ranges. Bit 4 tells the control whether the spindle encoder turns 1:1 with the spindle in all ranges; or whether it turns 1:1 with the spindle only in high range, and turns at the ratios specified in P65, P66 and P67 in the other ranges.

Once you have a proximity sensor wired to some available input (say, for example, INP16) then you could do rough orientation with code like this:

Code: Select all

M3 S30
G4 P1.0
M100/50016
M101/50016
M5

If you have a working spindle-at-speed signal (say, for example, INP15) then you could change the G4 dwell time to 0.1, then follow it with "M101/50015" to more reliably wait for the spindle drive to report it is actually running at the requested speed.

Yes, you should be able to tap with a floating (tension/compression or self-reversing) tap holder. Ideally you would use M109/1/2 to disable both the spindle speed override and the feedrate override for the duration of the tapping moves.

[CrossfireX]

Thanks CNCSNW,

I tried a couple of things this morning before I got stuck into my work for the day, and you're certainly correct, tapping cycles (G84, G74) do not work in the G19 plane.

It appears to automatically use the Z value as the hole depth regardless of the plane.

This is good to know at least. I will head over to a place I used to work at and find out how they use the angle head on the horizontal machine to see what I can find out there.

I will try the G81 and G85 cycles this afternoon and see what happens.

I don't think I'm going to run with the proxy switch for now, it's something that can easily be added later through various methods, so I'm not going to worry about it until I absolutely need it, if I ever do. If I can get away with basic helical interpolation on the G19 plane for rough boring, then use a G85 for Finish boring, and provided I can use a G81 or G83 for drilling, and get a floating tap holder and use a G85 for threading, that is all I will need.

I'll play around with M333 this afternoon too.

I'll let you know how it turns out.

Thanks

Jason