Canned Cycle Drilling on G19 Plane with Right Angle Head

[sm2000]

Good afternoon

I am hoping that someone could let me know why this canned cycle will just rapid instead of feeding to the depth of the hole?

2022 Takumi 3 Axis Mill

Fanuc Oi Control

I have a right angle head setup and my drilling in the G19 plane

%
O1111(RA DRILL CYCLE)
G20
G00 G17 G40 G49 G80 G90
(T23-2 CENTER DRILL)
G00 G90 G54 X-2. Y0. S1450 M3
G43 H23 Z1.
Z-2.925
X-.1
G19 G81 G98 Y0. X.03 F5.
G80 G00 X-.1
G17
G0 Z1.
M9
M5
G91 G30 Z0.
M30
%

 

[angelw]

Good afternoon

I am hoping that someone could let me know why this canned cycle will just rapid instead of feeding to the depth of the hole?

2022 Takumi 3 Axis Mill

Fanuc Oi Control

I have a right angle head setup and my drilling in the G19 plane

%
O1111(RA DRILL CYCLE)
G20
G00 G17 G40 G49 G80 G90
(T23-2 CENTER DRILL)
G00 G90 G54 X-2. Y0. S1450 M3
G43 H23 Z1.
Z-2.925
X-.1
G19 G81 G98 Y0. X.03 F5.
G80 G00 X-.1
G17
G0 Z1.
M9
M5
G91 G30 Z0.
M30
%

Hello sm2000,
The following won't affect the operation of your cycle, its just a comment on form. After completing the drilling cycle the drill should return to the Initial Level, in your case X-0.1 without having to specify the coordinate in the Cycle Cancel Block, as you have, with G80 G00 X-.1. Further, any Group 01 G Code (G00, G01, G02 and G03) will cancel a canned cycle; accordingly, both G80 and G00 don't have to be specified in the Cycle Cancel Block, only one or the other.

With regards to your actual issue, take a look at parameter bit 5101.0, it should be set to "1" to be able to drill in an axis other than "Z".

Regards,

Bill

 

[DouglasJRizzo]

Bill is correct. Check parameter 5101 bit 0.

 

[sm2000]

Thanks, I normally will just put the G80 to cancel the canned cycle but, saw someone do it on another page. I apreciate the suggestion and will take a look at that parameter.

 

[DouglasJRizzo]

G80 would, indeed, cancel the cycle, but the machine needs to look in the right place for it to happen.

 

[Jashley73]

Are you in G94 (feed per time)? G95 (Feed per spindle revolution) would look awfully fast if you were in fact feeding at 5" per revolution.