Considering a Full Rewire on a Working Schaublin 125 CNC

The main errors:
K0.75 is radius mode while in diameter mode.
I1 is radius mode (X34-X32) while in diameter mode
G96 D2500 ? 2500 m/min surface speed? Cutting steel with carbide  is typically only 1/10 that or less.
Maybe consider G97 S500 just to remove a variable while you are getting used it it?

Assuming a thread major diameter (stock OD) of 32, with you drive line at  X34, I-2. In practice, the major diameter is probably more like P/8 smaller. Somewhere around 31.8mm. Andy has programmed all that into his lathe macros, so you just give it major diameter (32mm) and it takes a first turning path at P/8 smaller before starting threading.
Since this is G7 diameter mode, the final depth K is also in diameter, so that will be 32-30.5 K1.5. Actually it is more likely to be about 30.38, so you will tweak this number to get your thread to fit, if you don't have perfect full profile inserts. Dont be surprised that you need around K1.62 to get the nut to fit.
J0.3 is reasonable. You will need lots of passes. See if you can get the insert to survive at J0.5
The R 1.6 means your cut will get heavier at each pass. I tend to set that at R2 for constant area, of course leading o increased number of passes.
The rest looks good.

G7 G18 G21 G90 G94
G0 X34 Z10
G97 S500 M3 M8
G76 Z-15 P1.5 I-2 K1.5 J0.5 Q29 H2 E0.75 L2

RotarySMP wrote:

G96 D2500 ? 2500 m/min surface speed? Cutting steel with carbide  is typically only 1/10 that or less.
Maybe consider G97 S500 just to remove a variable while you are getting used it it?


 

"D" is max spindle speed, not desired surface speed.

Thanks for the replies. The spindle.0.revs seems to be right when turning by hand, and when driving with the VFD active it is hard to tell exactly, but it seems to be correct as well.

Trying in constant speed instead of surface speed is a good idea, I will try that next.

And regarding diameter and radius, the man page I even linked says:

Note: When G7 Lathe Diameter Mode is in force, the values for I, J, and K are diameter measurements. When G8 Lathe Radius Mode is in force, the values for I, J, and K are radius measurements.

I don’t know how I overlooked that, it is really obvious now.

I am still struggling with threading.I have tested it at very low speed (100 RPM) in the hope to see something that helps me find what is wrong. But I cannot really say what I am looking at. The result is repeatable, and at least to me it looks like a constant offset that makes it wrong. I have set the cross-slide angle to 0, so that is not the reason. It is supposed to be an M8.

I would have expected a more random result if the spindle index was jittery, so that is probably not it. And spindle.0.revs, I tested it by turning the spindle by hand 25 turns, and spindle.0.revs was almost exactly 25. The remaining very small error can easily be attributed to me doing it by hand.
Additionally, I set the spindle to 1200 RPM and let it run. After it settled, I made a video filming the HAL Show screen and watching spindle.0.revs so I could later check it, and I got 1206 RPM that way.
I tried to make sure that the spindle really had 1200 RPM with a laser tachometer and by watching the encoder velocity RPM. Both agree within a margin of under 10 RPM. I don’t have any RPM measurement tools that are more reliable or accurate.

All these tests point me in the direction of the spindle encoder being OK. Are these tests the wrong way of testing this? What else can it be?

These are cheap as (can find them for half this price) and are well worth having
www.amazon.com.au/Mengshen-Tachometer-2-...ctive/dp/B0BFHXMKR3/

That is the exact type of “laser tachometer” I used. I agree that they are useful.

I double checked our ini's, and we both have the encoder scaling set to 8000 pulses/rev. Not sure what would cause that drift you are seeing.

Dudelbert wrote:

I am still struggling with threading.I have tested it at very low speed (100 RPM) in the hope to see something that helps me find what is wrong. But I cannot really say what I am looking at. The result is repeatable, and at least to me it looks like a constant offset that makes it wrong. I have set the cross-slide angle to 0, so that is not the reason. It is supposed to be an M8.



All these tests point me in the direction of the spindle encoder being OK. Are these tests the wrong way of testing this? What else can it be?

 

Take the below with a grain of salt, of course.

Spindle speed:  there is a bug in LCNC which causes a different start point during spindle synchronized motion if successive passes aren't at the same speed.  Constant surface speed is not OK in multi-pass threading.  Same reason folks have reported trying to do thread repair and lining up on a thread by hand, only to wipe out the threads when the spindle is run because the start point is different.

I don't think this was your problem, as I did a screen-cap of your video looking for the start point on each pass.  Pretty constant start point near as I can tell.

It looks like your thread is cutting mostly on the left (leading) side, which would correlate with the Q value you have set.  But it doesn't appear to be going much deeper each pass.

Like you cut one pass deep, then scrape the left side each successive pass without really going much deeper.  The chips look terrible... instead of a 'wire' each pass, you have scrapings.

 

Maybe run another attempt, but change the Q, E, and L values to 0 (straight in),  make sure I/J/K are diameter values, an R-value of 2.0, and ensure you have the spindle in G97.

This might help troubleshooting by taking out a few variables which may be obscuring machine issues.

EDIT - I jut re-watched the video and it's cutting the RIGHT side, not the left.  Like the "Q" value is backwards or something. The tool is moving at the same pitch each pass, but it's offset to the right slightly each successive pass.  Weird.