What's new
What's new

Semifinish with G71 on Fanuc O-TC controllers?

Rolka

Plastic
Joined
Mar 22, 2018
In an attempt to get semi-finish pass, with easy-to-adjust amount left for semi- and last finish pass, I tried to program something like this:

(ROUGHING)
[...]
G0 T0909
G50 S900
G96 S500 M03
G0 Z1.
X3.
Z0.1 M08
G71 U.107 R.02
G71 P60 Q80 U-.06 W.005 F.014
N60 G00 X3.91
G1 Z0. F0.01
G01 X3.85 Z-.03 F.006
Z-6. U-.0015 F.01
N80 X3.
G0 Z1. M9
[...]
M00

(SEMIFINISH)
[...]
G0 T0707
[...]
G0 Z1.
X3.
Z0.1 M08
G71 U.9999 R.02
G71 P60 Q80 U-.03 W.005 F.01
G0 Z1. M9
[...]
M00(MEASURE -.03, ADJUST OFFSET IF NEEDED)


(FINISH)
[...]
G0 T0707
[...]
G0 Z1.
X3.
Z0.1 M08
G70 P60 Q80
G0 Z1. M9
[...]
M30


Tried on O-T and O-TC controls, in both cases it alarmed that it could not find sequence blocks at 2nd run of G71.
From what I have learned on this forum (or was it from Peter Smid book?) - control looks for sequence numbers from current position down to M30, then from beginning of program down to current position, so this should work just

fine, but it doesn't.
Of course I can program semi in long form instead, but it is prone to errors if more complicated toolpath is in play (all is coded on controller), and must be recoded when operator decides to leave different amount for semi-finish.

What am I missing? Is behaviour of controller set in one of parameters maybe?
 
It has been a while sense I programed a lathe.

That said it looks like your "semifinish" would be a full roughing cycle. Can you change that to a G70 if memory serves correct the U/W will apply and leave that stock on a finish pass.

If that doesnt work you could use a different offset and a clean G70

Edit: Averthought the G71 is searching from current position to m30 the g70 is searching from beginning to current position.
 
Tried on O-T and O-TC controls, in both cases it alarmed that it could not find sequence blocks at 2nd run of G71.
From what I have learned on this forum (or was it from Peter Smid book?) - control looks for sequence numbers from current position down to M30, then from beginning of program down to current position, so this should work just

fine, but it doesn't.
Of course I can program semi in long form instead, but it is prone to errors if more complicated toolpath is in play (all is coded on controller), and must be recoded when operator decides to leave different amount for semi-finish.

What am I missing? Is behaviour of controller set in one of parameters maybe?
Hello Rolka,
The control is behaving as it should, as there is no scope for a G71, G72, G73 cycle to use a profile defined between P and Q Blocks up-steam from whence they are executed. The P Block should be specified immediately after the Second G71 Block and the Q Block, down stream from the P Block.

There are two basic Multi Repetitive, G71 Cycle Formats, FS15 (One G71 Block Format) and Standard FS16 (Two G71 Block Format). On controls FS16 on, either formats can be set via parameter. There have been many iterations of the Multi Repetitive cycles by Fanuc over the years and the version used with the FS10, 11 and 12 controls actually had a included addresses for a Semi Finish allowance (Fanuc called this allowance Rough-finishing) within the respective Roughing Cycle and was specified with I (X allowance) and K (Z allowance). Your FS "O" control I suspect is circa mid 90s and not the later "O" Series. That being so, there is no scope to being able to set the control to use the FS15 (One Block G71 Cycle).

deljr15 said:
Can you change that to a G70 if memory serves correct the U/W will apply and leave that stock on a finish pass.

Hello deljr15,
There is no scope to have the G70 cycle leave a Semi Finishing allowance. The only parameters that can be specified are the P and Q Block.

Regards,

Bill
 








 
Back
Top