Fanuc 31iA G68.1 Lathe

[Josh Kinney -Elite Engineering]

Gents,

I'm getting killed on a Mori NZX200/800-SY. I'm trying to use 15deg angled heads to drill/tap. Nothing I do seems to be working and even worse nothing I see the machine do makes sense. Everything I do either puts the tool in the wrong place or over travels. The Fanuc manual is not very helpful...

 

Any tricks I should know about?

 

N7(Sequence #7.) 

(TAP 15DEG HOLE) 

(TAP IS GUHRING 3939 M8X1.25)

M69

M45

G00G54G98G17 

G28H0. 

G0C0.

M68

T0

G68.1X0.Y0.Z0.I0.J1.0K0.R75. 

T0909

M8 

G0X1.0508Z3.

X1.0508Z1.

M329 S500

G84.1X1.0508R-.225Z.10F24.6M68

C90. 

C180.

C270.

G80

G0Z2.0

T0 

G69.1

G28U0

G28W0

 

Thanks,

 

-Josh

[Josh Kinney -Elite Engineering]

I think I got it. Trying to be smart and Fanuc said NO! It feels like I'm fighting a Mazatrol control today....

[Greg Williams]

Below is some code from a NT1000, working ot 15 degrees on the sub spindle, it has a G49 before G68.1

 

G28 U0
G28 V0 W0
G55
G00 T1018
G361 B65.0 D0.
G00 T1010
G59
M269
G98 G17 M246
M304
M245
G28 H0
G43 H18.
G97 S6000 M13
M269
G00 C0.0
M268
G49
G68.1 X0.0 Y0.0 Z0.0 I0 J1 K0 R155.0
N43 G43 H18.
G00 X0 Y0 Z6.
(**** SHIFT ****)
G52 X#547 Y#546 Z0
(**** SHIFT ****)
G332 R3.
G05.1 Q1
 
(22MM WIDE PART HERE)
G00 X23.6 Y14.416 Z6.0 M484
Z0.0
G01 Y-10.683 F1500.
G02 X19.6 Y-10.683 I-1.0 J0.0 (R1.0)
G01 Y10.8

[Josh Kinney -Elite Engineering]

Its different for a "non b-axis" machine.

 

I got it to work but its being strange. I can drill and then tap at 15deg. Cancel everything. Do some face live milling without g68.1. If I stop and go back up to the drilling at 15deg it misses the part and over travels....

 

MDI T0 G69.1 and it runs fine..

 

Apps guy has no idea...

[Josh Kinney -Elite Engineering]

I'm stumped.

 

Only way to use the angled heads in memory mode is to clear the G68.1 by typing the following in MDI:

 

T0;

G69.1;

G28 U0.;

G28W0.;

 

The turning works great.

 

So here's what happens. Clear via MDI. Run the program through doing the turning, gets to the drill and it's in the wrong spot. Clear again through MDI and it drills at 15deg, toolchange and taps at a 15deg and then finishes turning. If you jump back up and try to drill it's in the wrong spot. If you try and start over it runs till the drill and then drills in the wrong spot.

 

Bottom line is if you do any turning you have to clear via MDI to drill and tap at 15deg.

 

Stupid xxxx control. Why does it have to be so difficult? I thought my VariAxis500 was a diva....

[Josh Kinney -Elite Engineering]

Book was TOTALLY wrong. Wouldn't have worked in a million years.

 

Here's what worked:

 

N6(Sequence #6.) 

(DRILL 15DEG HOLE) 

(DRILL IS GUHRING 5510 7.4MM)

M69

M46

T1111

G98G17 

M45

G28H0. 

G54

G0C0.

M68

G68.1X0.Y0.Z0.I0.J1.0K0.R75. 

M8 

G97S2500M13

G0X1.082Z[3.+#600] 

X1.082Z[1.+#600] 

G83X1.082R[-.225+#600]Z[.150+#600]F20.M68

C90. 

C180.

C270.

G80

G0Z2.0 

M05

G69.1

G28U0

G28W0

M01