HAAS Error 369 on Outside Contour

[brcasey3]

Hey Guys,

First time post here! I'm hopeful you all will be able to help me out.

We have a HAAS TL2 at work. I wrote a program that runs a G71 canned cycle. The program runs fine without tool nose compensation. However, when I plug in a G42 for TNC, the G71 cycle stops at the end of the last "finish" pass. I get HAAS error code 369: Tool Too Big. The strange thing is, the contour that the error code comes up on is the very last outside contour. How is it possible for the tool to be too big for an outside contour?

Attached is the picture of the geometry, and below are the tabulated values.

(GEOMETRY INPUT)

(D1 = 0.75")

(D2 = 1.25")

(FACE LENGTH = 1.0001")

(FACE OFF = 0")

(EDGE 1 = 0.0625 RADIUS")

(EDGE 2 = 0.125 RADIUS")

(EDGE 3 = 0.0625 RADIUS")

(SPINDLE STICK OUT = 0.5")

(TOTAL STICK OUT = 1.6251") Below is the section of G-Code with TNC issues: N300 (SHIFT G54 WORK COORDINATES Z-ZERO = FACED END) (ROUGH TURN PART) G10 L2 P1 G90 X0. Z1.5626 (SET G54 TO X0. Z1.5626) (Z-ZERO IS THE FINISHED FACE) G00 G28 U0. (HOME OUT TURRET) G00 T101 (OD RGH TURN TOOL) G97 S1000 M3 (CANCEL CSS, START SPINDLE FWD) G54 (G54 WORK OFFSET) G42 (TNC = ON) G00 Z0.05 (Z START POINT OF CANNED CYCLE) G00 X1.35 (X START POINT OF CANNED CYCLE) M08 (TURN ON COOLANT) G50 S1800 (SET MAX RPM) G96 S350 (CONSTANT SURFACE FOOTAGE) G71 P301 Q302 D0.06 U0.04 W0.02 F0.007 (SEQ.#'S/CUT-DEPTH/X-LEFT/Z-LEFT/FEED) N301 G00 X0.625 (SMALLEST DIAM.) G00 X0.625 Z0. (MOVE TO FACE) G03 X0.75 Z-0.0625 R0.0625 (EDGE 1 END PT.) G01 X0.75 Z-0.8751 (FACE CUT) G02 X1 Z-1.0001 R0.125 (EDGE 2 END PT.) G01 X1.125 Z-1.0001 (SHOULDER LRGST DIAM.) G03 X1.25 Z-1.0626 R0.0625 (EDGE 3 END PT.) N302 G00 Z0.05 (Z START POINT) G00 X1.35 (X START POINT) M09 (TURN OFF COOLANT) G40 (TNC = OFF)

Any help or ideas is greatly appreciated. Thank you for your time.

Best regards,
Bennett

Similar Threads:

• Contour/pocket error
• I J error on Haas
• error message during rough flowline or contour
• Need Help!- Bad contour error
• Bad Contour Error while Pocketing

[rcs60]

i would try a small g01 z move that is slightly bigger that the tool nose radius
if the tool radius is .015 make a z move .017
or the other thing i can think of is to use a g01 x (2+ x tool radius to clear the radius in the x axis to be able to rapid to g0 z.05

[dcoupar]

rcs60 is correct:

Add a block before N302 with a straight Z move of at least the tool radius comp amount.

N302 needs to retract X to the start diameter (1.350) so, if your tool radius comp value is 0.03:

G03 X1.25 Z-1.0626 R0.0625 (EDGE 3 END PT.)

G01 W-0.032

N302 G40 X1.350 (RETRACT TO X STARTPOINT OF CANNED CYCLE)

[brcasey3]

Thanks for the input guys. I'll give it a shot on Monday when I can get access to the machine. The tool nose radius is 0.0315". I'll use the incremental move dcoupar recommended, but will code in: G01 W-.035

dcoupar, I'm curious as to why you included the G40 in the N302 line. The very last line of my N300 routine is G40. Would one of the G40's be redundant?. Is there a reason to put G40 on the N302 line and not the last line? I'm pretty new to G-coding, so any advice is greatly appreciated.

[dcoupar]

I did it that way because that's how it's shown in the Haas Lathe Operator's manual. The 2nd G40 would be redundant, and could be eliminated.

While you're at it, I'd move the G42 from where it is to the N301 block.

N301 G00 G42 X0.625

Also, the G00 in that block is redundant, but in the overall scheme of things, it isn't hurting anything.

(Just my 2¢ worth)

[brcasey3]

dcoupar, your suggestion worked great. Thank you very much. I also made the changes to the G40 and G42 commands you suggested, that worked well too. Sorry for not getting back to you guys sooner, things have been pretty hectic at the shop.