G41/42 cuttercomp Problem...

[Swemill]

Hi everyone, here comes problem from Sweden.....
I have bought an old Kitamura Mycenter-1 cnc mill (1983) with Fanuc 3M-C control (only G92).
When i try to mill a simple rectangle part outside with G41 it dont go right,
Have tried lots of combinations but it wont go 90 degree - straight line with the compensation as it should.....
At work i have a "new" YCM with 16i and there never is this problem...

The parts external cornercordinats is:

X0 Y0
X0 Y-50.
Y-50. X-100.
Y0 X-100.

If i go in compensation from x0 Y10. to x0 Y2. (with compensation 5mm) it goes right (5mm from the absolut line). Outer with g41 and inner with G42 so that seems to work. But then i go to Y-50. and it "stops" at Y-45. (instead of Y-50. + comp as it should). Then i go straight to X-100. and it goes "wryly" down to X-95. Y-50. After that i program Y0 and it goes to x-100. Y-5. Then i have X0 and the machine goes up to Y0 and X-5....?
It seems to "count down" the cuttercompensation at each axles movement and dont "calculate" it right / doing "shortcuts".....!?

Can it be a Parametric issue?

Sorry for my bad English and explanation.... Don't write much in that but i hope you understand my problem!
I do cuttercomp every day at work but not in this machine or with Fanuc 3M....

Best regards and with hope of a solution...

/Jocke

[tony784]

let me see your g-code program....maybe I can help you

[dcoupar]

I believe the 3M required those G39 I J blocks to tell it which way the next move was going... I don't have an example, though.

[Mitsui Seiki]

Posta hela programmet.
I alla fall den del som krånglar.
Det är enklare att se vad som är fel.

[tauntdesigns]

Right hand cutter:
climb cut = G41
conventional cut = G42

[Swemill]

Ahh.... More "Swedes" here! :-)

I thought you wanted the program and i belive it's like this:
(dont have an exact sample here)

%
O0001
G0 G91 G28 Z0
G28 X0 Y0
G92 X175. Y55. Z307.
G80 G40 G49
G0 G90 G43 X0 Y0 Z2. H2 S1000 M3
G1 Z-2. F500. M8
G41 X0 Y2. H22 (H22=5mm)
Y-50.
X-100.
Y50.
X2.
G0 Z20. M9
G40 X20.
G91 G28 Z0 Y0
M30
%

With this prg. i want a 100 x 50mm rectangle....
The machine dont have any D and only uses H. I also have G17 connected in MDI!

Must say BIG thanks to dcoupar.... I really thinks that G39 is the solution in the old 3M!!!
Have read about it but thought that it was an alternative to get radius at corners (not sharp edges) and not a necessery thing. To bad of me...

That would also explaine why i couldnt connect G41 from X10. Y10. to X0 Y10. and then go in Y- with G1 !
Could only do that sucsessfully (G41 and right comensated) with a straight line in Y like the prg. above!
To do that i then would have needed a I and J value also...!?

I also hope that it would be able to do very small radius at the 90 degree corners to go around a angular part!?
Any suggestions how the program would be with G39?

Shall try this at home tonight after work...

/Jocke

[Swemill]

After more searching it seems that I and J replace X and Y in G39 and is assumed to be the same! That must mean that no radius have to be made to get it work and it will be "right and sharp angles"... ?

[bugzpulverizer]

Why can't you just do this?

%
O0001
G0 G91 G28 Z0
G28 X0 Y0
G92 X175. Y55. Z307.
G80 G40 G49
G0 G90 G43 X10. Y10. Z2. H2 S1000 M3
G1 Z-2. F500. M8
G41 X0 Y2. H22 (H22=5mm)
Y-49.
G2 X-1. Y-50. I-1.
G1 X-99.
G2 X-100. Y-49. J1.
G1 Y-1.
G2 X-99. Y0 I1.
G1 X-1.
G2 X0 Y-1. J-1.
G40 G1 X20.
G0 Z20. M9
G91 G28 Z0 Y0
M30
%

I think this will put 1MM fillets around every corner. You had a Y50. in your g-code almost like you were programming with a G91. Hope this helped.

[Swemill]

Oops... The Y50. should be Y0!

I suppose your version with fillets also would work but to do it without G2 it seems to be the right way with G39 and I - J !?

[bugzpulverizer]

Yeah, it's a habit of mine. Even when I programmed at the machines I put fillets on every corner I could. I don't like deburring anything. Hope it all goes well for you.

[Mitsui Seiki]

Try this.If it's possible.I don't know what the part looks like so maybe the X10Y10 doesn't work for you.

%
O0001
G0 G91 G28 Z0
G28 X0 Y0
G92 X175. Y55. Z307.
G80 G40 G49
G0 G90 X10. Y10. Z2. S1000 M3
G43H2Z10.
G41 X0. Y2. H22 (H22=5mm)
G1 Z-20. F500. M8
Y-50.
X-100.
Y0.
X2.
G0 Z20. M9
G40 X20.
G91 G28 Z0 Y0
M30
%

G0 G90 G43 X0 Y0 Z2. H2 S1000 M3 G1 Z-2. F500. M8 G41 X0 Y2. H22 (H22=5mm)

The movement you have between X0Y0 to X0Y2 is smaller than the radius of the tool.

[Swemill]

ahh... Oops again.... Really sorry Stefan but the Y0 offcourse should have been Y10. It seems that i was a bit careless when i wrote it here..... In the machine i have Y10. but it didnt help.... Have tried a lot of diffrent "running-ins" with G41 and have no alarms but it still wouldnt go the right way. I could'nt run in from X10. Y10. either but it probably also have with the 3M - G39 "issue" to do. Straight from X0 Y10 to X0 Y2. the G41 run-in worked, but not the rest.....

I´m 99,9% convinced that the problem is the G39 i didn't run. There seems not to be time to try it out tonight but i sure will tomorrow!
If anybody else here have experience of Fanuc 3M and / or programming with G39 i'm very intrested of any more tips / info!

/Jocke