![Quote](images/misc/quote_icon.png)
Originally Posted by
Josh-PTP
Hey guys,
I am having a little problem with a tool nose radius program on my lathe. The tools radius is .031" Here is the part of the program that is giving me problems. I keep getting a 041 alarm. Thanks for any help.......
N1
M98P1
T0101(80 DIAMOND TOOL RADIUS = .031 TOOLNOSE QUADRANT = 3))
G97S800M13
G00X1.4Z.0
G50S2500
G96S600
G99
G01G99X0.F.005
G00Z.1
G00X1.55Z.1
G42X1.45Z.05
G99
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0X1.0
G01G99Z0.F.005
X1.191,R.03
X1.375Z-.875
Z-1.0
X1.4
N200G0X1.45
G70P100Q200
M98P1
Thanks for any help........
You need to set the TNR in the Tool Geometry Page and the Tool Tip Designation or your comp won't work. Setting the tool at least 2 times the radius away from the cutting point too.
![Quote](images/misc/quote_icon.png)
Originally Posted by
xyzer
HMMMMM...our Fanucs won't use cutter comp in a canned cycle.
I see a couple of issues, Don't forget the tool type settings and tool radius in the geometry screen. It may be a tad longer but you can see the G42 install and cancel
G0X1.45Z.05
G71U.05R.015
G71P100Q200U.03W.01F.005
N100G0X1.0
G01Z0.
G1X1.137Z0.0
G03X1.1966Z-.0269R.03
"X1.191,R.03(WON'T WORK)" iF IT WAS AT 90 DEG IT WOULD NEED R-.03
G1X1.375Z-.875
Z-1.0
N200X1.45
G0X1.5Z.1
G42X1.45Z.05
G0X1.0
G01Z0.
G1X1.137
G03X1.1966Z-.0269R.03
G1X1.375Z-.875
Z-1.0
X1.45
G0G40X1.5Z.1
XYZer,
The reason your comp isn't working is one or both of these reasons.
1) Your using a control that is older than 1984.
2) You need to call the TNR Comp in the Canned Cycle or it won't work.
Here is an example:
%
O0086
G0 G40 G97 G99 T0 M5
G28 U0 W0 M9
G50 S2000 M41
M1
N1(REMOVE SKIN/R-FACE/TURN)
G28 U0 W0 T0
T101 M8
G96 S475 M3
G0 G42 X3.99 Z.3
G1 Z-1.3 F.01
X4.05 F.015
G0 G40 X4.1 Z.2
G72 P10 Q15 W.005 D400 F.008
N10 G0 G41 Z0
N15 G1 X0 F.004
G0 G40 X4.0 Z.1
G71 P20 Q25 U.02 W.002 D850 F.01
N20 G0 G42 X1.0
G1 Z0 F.0025
X1.325 F.003
G3 X1.375 Z-.025 R.025 F.0025
G1 Z-.75 F.004
X2.75 F.0035
X3.975 Z-.9141 F.0025
G1 Z-1.08 F.004
N25 X4.1 F.0035
G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1
N2(F-FACE/TURN/U-CUT)
G28 U0 W0 T0
T303 M8
G96 S650 M3
G0 G41 X1.5 Z0
G1 X0 F.004
G0 G40 X4.1 Z.1
G70 P20 Q25
G0 G40 Z.1
(U-CUT)
G1 X1.3755 Z-.725 F.05
Z-.755 F.004
G4 U1.0
G1 Z-.75 F.006
X2.8 F.003
G0 G40 Z.1 M9
G28 U0 W0 M5
G97
T0
M1
N3(DRILL)
G28 U0 W0 T0
T505 M8
G97 S400 M3
G0 X0 Z.25
G1 Z-2.25 F.0072
Z.05 F.2
G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1
N4(R-BORE )
G28 U0 W0 T0
T707 M8
G96 S400 M3
G0 G40 X.75 Z.1
G71 P40 Q45 U-.02 W.002 D320 F.0075
N40 G0 G41 X1.214
G1 X.814 Z-.1 F.003
Z-1.3 F.005
N45 X.75
G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M1
N5(F-BORE)
G28 U0 W0 T0
T707 M8
G96 S550 M3
G0 G40 X.75 Z.1
G70 P40 Q45
G0 G40 Z.1 M9
G28 U0 W0
G97
T0
M30
%
BTW: Look at the notes in the Fanuc Manual. It will explain everything.
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com