Fanuc T6 G71 type 2 G-code troubles

[Snowie]

Hi all
Not sure if this is the right place to post this or not.. but here go's

I'm having troubles at setting up Type 2 G71 Canned cycles witch i need as there is pocketing in the Z axis

The machines errors out 065 when it runs the first line of the roughing cycle

%					' This program Machines the Z profile
'Material 2in out 65mm from chuck
:0003						'Program number
N010 G50 S1500;					'Set max chuck speed
N020 G96 M04 S200;				'Turn on constant surface speed, Start splindle clockwise  @ 200M/Min chuck speed
N030 G99;					'Turn on feedrate mm\rev
N040 /M08;					'Option turn on coolant
N050 G00 X52.00 Z1.00;				'Rapid positioning, Move to position X52 if a bit bigger than the diameter of the stock work peice
N060 G71 P070 Q190 U0.5 W0.00 D1000 F0.25;	'(G71)Z Profile,(P060)Start of facing cycle,(Q070)End of facing cycle,(U0.5)Finishing allowance X directing.(W0.25)Finishing allowance Z directing,(D500)Depth of cut 0.5mm.
N070 G00 X31.00 Z0 ;				'Start of tit on the end  ---------Errors here-------------
N074 G01 Z0.00;	
N075 X31.75 Z-0.5;					'Tit in the end
N080 X37.00;					'Start of taper
N090 X40.45 Z-5.70;				'Cut taper
N100 Z-17.10;					'Thread leadin start
N110 X45.00 Z-19.38;				'Thread lead in
N120 Z-28.25;					'Thread length
N130 X41.50 Z-30.00;				'Thread lead out taper
N140 Z-33.40;					'Tharead Clearence
N150 X49.30;					'Start of taper
N160 X50.8 Z-34.10;				'Cut taper
N170 Z-39.25;					'Head flange length
N180 X49.3 Z-40.00;				'Cut taper
N190 Z-45.00;					'Clearence cut

'finishing
N200 G70 P070 Q190 F0.15; 			'(G70) Finishing cycle,(P060)Start of facing cycle,(Q070)End of facing cycle
N210 /M09;					'Option turn off coolant
N220 M99;                          			'	 Return from sub program
%

As expected the code runs if i leave out the Z0.00 but the pocket is missed out on the roughing cycle but is done on the G70 finishing


Then manual says it can do it but there is no examples. I've had a Google and the examples i find have the same issue

What am i missing

Cheers

[fordav11]

what is alarm 065?

The manual states pocketing in the Z axis with G71 can't be done even if Type II is enabled.

also read this thread....
http://www.cnczone.com/forums/fanuc/...-t_help-2.html

it has a lot of info about type II roughing cycles.

[Snowie]

Hi
Sorry i might have lead you a-stray. The pockets are along the Z Axis (Shaft with groves and shapes along the length of it)

Code 065 is a long windered one. But here is the tail end of it

"in G71 & G72 , Z(W) has been commanded (G71) OR X (U) has been commanded (G72) in the block of Sequence No. Commanded by P"

When you say

Type II is enabled.

I take it my machine could not have it enabled??
If so How do i check

Page 158 & 159 of my manual goes on about type 1 and type 2

Cheers

[sinha_nsit]

Type II is not available on your machine.
Is it 0i Mate series?

[angelw]

Originally Posted by Snowie Hi Sorry i might have lead you a-stray. The pockets are along the Z Axis (Shaft with groves and shapes along the length of it) Code 065 is a long windered one. But here is the tail end of it "in G71 & G72 , Z(W) has been commanded (G71) OR X (U) has been commanded (G72) in the block of Sequence No. Commanded by P" When you say I take it my machine could not have it enabled?? If so How do i check Page 158 & 159 of my manual goes on about type 1 and type 2 Cheers

To expand on Sinha's comment, Type II G71 and G72 are initiated by programming both X(U) and Z(W) in the block referenced by the P command in the G71 or G72 cycle. Error 065 is raised if an attempt is made to initiate Type II G71 or G72 cycle with a control that does not have that option.

The result that you achieved by leaving out the Z move in the P referenced block is typical if you include a non-monotonous X move when using Type I G71, which is what you have when only an X(U) command is made in the P referenced block. Its also typical that the G70 cycle will follow the profile; it will always follow the finished profile exactly. In fact you can use G70 to run a profile between Sequence numbers referenced by the P and Q commands in the G70 block without having previously executed a G71 or G72 cycle.

Regards,

Bill