[bmlw]

Hello ALL!

Just ran into a problem when I view or post code the tool change come in with a negative move as discussed bellow.

In FANUC 11T POST
Under FORMAT “TOOL CHANGE” I have the following information.


G97S<CALC-SPEED><SP-RANGE><EOB>
<MOTION>X<X-RETURN>Z<Z-RETURN><SPINDLE><EOB>
T<$TOOL>00<EOB>
M01<EOB>
N<TOOL>G50S<SP-MAX><EOB>
T<TOOL><OFFSET#><EOB>
{<MOTION>}X<X-COORD>Z<Z-COORD><COOLANT><EOB>
<IF><CSS-ON><THEN>
G96S<CSS-SPEED><EOB>
<ENDIF>
G04U2.<EOB>

This results in the below G-CODE output with an X-axis –11.0092 move that drives the turret down to the over travel and stops the machine.

G97S450M42
G0X--11.0092Z3.4908M3
T0300
M01
N06G50S4000
T0606
X6.45Z0.0349M8
G96S760
G04U2.

Any ideas as to what I am doing wrong?
Thanks

[kuyohtay]

Here at Hardinge, this is how we do it.

"<MOTION>X<X-RETURN>Z<Z-RETURN><SPINDLE><EOB>"
change to...
M98P1<SPINDLE><EOB>

Add a sub program for SAFE travel (P0001).
O0001(SAFE INDEX PROGRAM)
G0G40G97G98Xnn.nnn2Znn.nnnT0
M99

Adjust Xnn.nnn and Znn.nnn to a safe turret position for rotation as needed.
Usually we fix this at something like X10.500 Z6.000
Dependent on your X and Z travel of course.

We call this out at the beginning and end of EVERY Tool motion.
You decide what you want, don't wastetime on Post Development.


Kuyohtay.
PS
Sample Program:
(#500 IS STORED WORK OFFSET // -NN.NNN FROM Z-ZERO)
%
O1122(TEST-01)
N1(RGH TURN)
G10P0Z#500M64
M98P1
M4G97S2000P1T0101
G0X2.1Z.1Y0
G50S2500
G96S600
G99
G71U.100R.025
G71P700Q701U.025W.004F.010
N700G0X0.
G1G99Z0.F.004
X.75,C.1
Z-1.1,R.05
X1.7,R.1
Z-1.5
N701X2.1
M98P1
M30
%

[bmlw]

Kuyohtay,
Thanks for the input, I will now learn about inputing sub progarams. I appreciate the answer and I will let you know how it works.

[rick_7037]

If you have a value in the tool change position in the Post Proc it is getting its info from there if youve put -- in it it will transfer over