[L98FIERO]

I have to groove a bearing and the drawing specifies 1.5 pitch double start and it starts in one end groove and ends in another. I don't have a problem with the spiral groove from one end groove to the other but how do I get it to do the double start and still start and end at the same places? Is the manually repositioning the bearing the only way?

[fordav11]

use 2 threading cycles with a different start point and double the feed.
let's put in some sizes for a real example.

diameter 100mm, start Z -10.0mm, end Z -50mm, depth 1mm and with your 1.5mm pitch (I guess you're working in metric?)

O1234
G50 S1000
G0 T0101 M8
G97 S200 M3
G00 X105.0 Z-10.0 M24
G76 X98.0 Z-50.0 I0 K1.0 D0.1 F3.0
G00 X105.0 Z-8.5 M24 (2nd Z is first Z minus or plus 1.5mm)
G76 X98.0 Z-50.0 I0 K1.0 D0.1 F3.0
G00 X200.0 Z200.0 M9
T0100 M5
M1
M30
%

[L98FIERO]

Thanks for the reply Fordav11 but no I'm not working in metric, sorry for not mentioning that. The groove is 1/16 inch radius groove with a 1 1/2 inch pitch double start groove in a 1 1/2 inch bore. I'm not at work now and don't have the drawings but I think the grooves at the ends are about 3/16 inch wide. I knew I could get a double start by changing the start point by 1/2 the pitch but because I have to start in the first groove that's not an option, is there another way?

[fordav11]

new controls have an added P on the G76 line for number of starts but not on a 6-series.
it depends on how accurate the starts need to be but if it's not that important, blue the face of the part and scribe a line across the face. set up a scribe or sharp point tool or even a turning tool in the machine, bring in the tool/pointer in X and rotate the chuck by hand to locate the pointer and the clamped part centrally on the line. lock the chuck so it can't move (or put in the lowest gear but you may need to re-locate/align the chuck again if the chuck moves) then unclamp the part and rotate it 180 degrees so the pointer lines up with the opposite scribe line then re-clamp the chuck. you should be able to get it within 1/2 a degrees or better easily with a few minor adjustments (unclamp, rotate slightly then re-clamp until perfect). Just make sure the chuck doesn't rotate while it's unclamped and you'll be fine.

[L98FIERO]

Thanks Fordav11, that's what I thought would be the only way but didn't know if there was a better one.

[L98FIERO]

I've finally got to trying out the oil groove/threading at 1.5 inch pitch in a 1.5 inch bore and have run into an issue.
The groove is .13R x .01 deep in bronze so there isn't a problem with cutting the groove in a single pass however when I try it, it will always do at least two passes. While they start at the same place the pitch doesn't exactly match, it's significantly different to the extent that it will be about 1/4 inch pitch different after 2.25 inches. I tried at 100 rpm first and when that didn't work I tried 50 rpm which was no better. I had changed parameter 068, threading minimum pass depth, to zero with no effect. Is there another parameter or something to get it to do it in one pass?
Would it be better to use G92 instead?

[L98FIERO]

I found out what I was doing wrong. I had written the canned cycle program:
...
...
G0 X1.4 z.25
Z-.3
G1 X1.51 F.005
G4 P200
G0 X1.45
G92 X1.51 Z-2.81
Z.25
...
...
So it was making a threading pass between Z-.3 and Z-.25, the line after the G92 must have a G0 or G1 to cancel the cycle.
Now the question still is, why does the G76 threading cycle not follow the same path every time?

[fordav11]

G76 should work fine. Maybe you're doing something else wrong?
If you post part of the program we can have a look....