G71 problem on Fanuc 15-TF

[serickson]

Trying to start using G71 multi-repetitive cycle on Puma 8HC turning center.

This is simple code I am trying:

G20 G90 M17
G28 U0. W0. T0600 S600
M42
G50 S2000
G57

M03
(TURNING TOOL #6) 
G0 X2.2 Z.2 T0606
(TOOL CLEAR OF PART)
G96 G99

G71 P100 Q101 D.05 U.02 W.02 F.010
N100 X.5 Z0.0
X0.7 Z-.45
Z-.105
X1.25
G03 X1.75 Z-1.55 R.5
G01 Z-2.5
N101 X2.2
M05
M30
%

When the G71 line is executed I get alarm: "Illegal use of decimal point"

Can anyone tell me what I am doing wrong?

Cheers,
Steve E

Similar Threads:

• Problem Fanuc 18-T
• Need Help!- FANUC 11M-A problem
• PMC problem with Fanuc 18i TB
• Need Help!- Problem with fanuc 01
• Fanuc 6T problem

[yardbird1969]

Apparently it's not liking one of the decimals in one of the variables in the canned cycle.

See if it runs this way?

G71 P100 Q101 DO5OO U0200 W0200 F0100

You need a G1 in the N100 line.

I don't understand the Z-.105 move. Is it a typo?

Brent

[mbservice]

Try
G71 P100 Q101 D05 U.02 W.02 F.010

If that doesnt work try taking the point out on feed
If you send me your email I'll send you the manual

[serickson]

Apparently it's not liking one of the decimals in one of the variables in the canned cycle.

See if it runs this way?

G71 P100 Q101 DO5OO U0200 W0200 F0100

You need a G1 in the N100 line.

I don't understand the Z-.105 move. Is it a typo?

Brent

Yup, that was a typo. It should be Z-1.05 So I'll try that & see what happens, and if that doesn't work I'll remove the decimal points as suggested.

Cheers,
Steve E

[serickson]

My control did NOT like decimal point for the 'Dxx' parameter. I had to use 'D0500' for a .050" deep rough pass.

Here is my working code:

G20 G90 M17
G28 U0. W0. T0600 S600
M42
G50 S2000
G57

(TURNING TOOL #6)
G0 X2.2 Z.2 T0606
(TOOL CLEAR OF PART)
G96 G99

M03
G01 U0. W0. F0.01
G71 P100 Q101 U0.01 W0.010 F0.01 D0500
N100 G01 X.5 Z0.0 F0.005
X1.0 Z-.45
Z-1.05
X1.25
G03 X1.75 Z-1.55 R.5
G01 Z-2.0
N101 X2.2
G70 P100 Q101
M05
M30

Thanks for the guidance.

Cheers,
Steve E