G71 help

[NID]

Here's my problem...
On this G71 cycle I need to have the tool be farther away from the part each time it rapids back to the starting point in the Z axis. I am stumped and have tried adjusting just about every line with no change.
(using Fanu 3T lathe)
Here's the program segment:

G0Z0.1
G01G41X2.063Z0.03F0.025
G71U0.175R0.025
G71P99Q111U-0.016W0.005S880F0.0065
N99G0X5.45S1300F0.0045
Z0.05
G01Z0.001
X5.3634
X4.5796Z-0.6269
N111X2.1Z-0.6269
G70P99Q111

Any suggestions?
Thanks much,
Jeff

[Geof]

I am most familiar with Haas and on these controls when they run in Fanuc mode the tool retraction is controlled by a Setting. Canned Cycle Retract Distance or something like that.

And a hint if you find this is the same in your case; if you change it to a large retraction remember this before you use G71 for boring. Large retractions, large boring tools and tight holes are not compatible without a lot of noise.

[swarfmaker]

Hi Jeff,
I would put comp on/off with-in the cycle and alter start pos for cycle

G0X2.063Z0.1
G71U0.175R0.025
G71P99Q111U-0.016W0.005S880F0.0065
N99G0X5.45S1300F0.0045
G01G41Z0.001
X5.3634
X4.5796Z-0.6269
X2.1Z-0.6269
N111G40X2.
G70P99Q111

Regards
Steve

[tobyaxis]

Hi Jeff,

Old Fanuc controls set the tool return distance in the Xaxis through the R input in the first line G71 U(Depth of Cut) R(Return in X amount from stock)
The second line G71P(sequence block start)Q(sequence block end)U(leave for finish Xaxis)W(leave for finish Zaxis)F(feedrate)

Example:

T101M8
G50S2000
G96S950M3
G0X1.2Z.1
G71U.07R.075>the R designation on this line of code changes X distance away radial
G71P101Q102U.005W.002F.01
N101G0G42X0
G1X.95F.005
X1.0Z-.025F.0025
Z-1.0F.006
N102X1.2F.005

Here is a tip.
Notice how I changed the feedrates for each move in the canned cycle. These feeds will only be active in the G70 finishing, not the roughing. Use this method if you have a difficult material to machine or if the finishes have to be improved on different surfaces.

Feel lucky that you are using this Fanuc Control, the newer ones have a parameter in which has to be changed in order to change the distance of the X axis return.

Also you can call tool nose radius comp in the canned cycle, it will cancel it's self after each pass, and initiate it in the beginning of each pass.

If you have anymore questions send me a private message. Milling or Turning

I hope this helps you

tobyaxis