[Fairlane6t9]

I have an SL 10. I'm programming a part that has an R8 shank taper near the chuck. I'm using MasterCam X4 to generate canned cycles for this. When the lathe starts the last rough pass, it starts tapering in towards the chuck and cutting the diameter smaller than it should. This is weel before it gets to the R8 taper which it seems to cut just fine. When I say it tapers, I mean it moves in X as it goes along the Z axis. I have run this same program in 2 HAAS simulators and neither sim will move in X when it's not supposed to. Here is my code. I have MasterCam set to put the tool nose offset in at the controller. This is posted for a generic 2 axis slant bed lathe, as I've not been able to get the HAAS post running yet. Does anyone see what could be causing the problem?

%
O8989
(PROGRAM NAME - PROTOTYPE1)
(DATE=DD-MM-YY - 12-03-10 TIME=HH:MM - 12:37)
(MCX FILE - H:\CLEANCUTTERTOOLPATH UPDATE.MCX)
(NC FILE - H:\PROTOTYPE1.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
G20
(TOOL - 3 OFFSET - 3)
(OD ROUGH RIGHT - 80 DEG. INSERT - WNMG332MP)
G0 T0404
M8
G97 S364 M03
G0 G54 X2.1 Z.15
G54 X2. Z.1
G50 S3600
G96 S200
G71 U.05 R0.1
G71 P100 Q102 U.02 W.01 F.01
N100 G42 X.95 S200
G1 Z-3.06 F.003
X.9716
X1.25 Z-4.
N102 G40 X2.
G0 Z.1
G50 S1500
G42 X.95
G70 P100 Q102
M9
G28 M05
T0400
M30
%

[CNCRim]

As far as programming wise I don't see anything wrong with the program, what is the dimension you got when measure?

[ken70ss396@yaho]

Try removing the G42 from the N100 line and put it in a new line, G42 X2., after the G54 X2. Z.1 line. Remove the X2. from the G54 X2. Z.1 line.
G0 G54 X2.1 Z.15
G54 Z.1
G42 X2.
G50 S3600

Also move the G40 to a line after the end of the cycle.

[Fairlane6t9]

I've not measured it yet as it's still sitting in the lathe. I reset the machine when it started moving in X to avoid a potential crash. I'm wondering if there's a setting or parameter that needs to be turned on/off in the controller.

[CNCRim]

Fairlane6t9,

Not try sound to be rude/anything, but it's very hard to understand what you are saying with fragment sentence.

[Fairlane6t9]

I didn't realize I had used any sentence fragments. Sorry about that.

[mookh1]

hi there.
ur programming is not right for using tool comp, ur G42 starts wrong.
N100 X.9
G1 G42 Z0 F.003
X.95
Z-3.06
X.9716
X1.25 Z-4.
X2.
N102 G40 X2.
G0 Z.1
G50 S1500
G70 P100 Q102
If i am right in what you are trying to achieve you should find that X will Not move With Z. the only reason it was, cause you trying to open tool comp on X it always needs to be started on Z.
Hope it Helps.

Mookh1.

[Fairlane6t9]

Thanx.....it's starting to make more sense now.

[mookh1]

Hi there.
Glad it helped, don't want to be rude, but the way you are programming is making it look very difficult, could give you a few programming examples which might make it look easier, if you would like.

Mookh1.