[WiggZero9]

So I am having an issue, after a tool change my machine wants to rapid on the G1. When I run the program through or if I just start and run the tool before the one with the problem it cuts my groove at rapid feed. If I start from the tool with the problem then it works fine. The top line pasted is the taping cycle that is before the problem, you can see the codes through the tool change, feeding into the part and starting the profile. What really confuses me is starting at the tool chamge (#5) it works just fine but running through the program or starting at the tool just before I run into this problem.


G98 G84 X-0.0049 Y-1.3572 Z-0.5 R0.1 P0 F0.0393
X2.4001 Y-1.3842
X0.9577 Y0.6485
G80
(OP2 MILL .12 SLOTS)
M9
G28 G91 Z0
G28 X0 Y0
M1
N14 T5
M6
G0 G90 G55 X1.02 Y-1.4369 M3 S6500
G43 Z2.5 H5 M8
G0 Z0.1
G1 Z-0.025 F26.
G2 X0.5428 Y-1.2602 I0 J0.7328 F32.5
G3 X0.2431 Y-1.6012 I-0.1478 J-0.1723
G1 X0.7915 Y-2.095

[Superman]

Your previous tool was tapping a 1mm pitch thread,....... going by the feedrate, it was feed per rev ( G95 )
- there is NO change back to feed per minute ( G94 ) ...so it is doing 26" per rev feedrate

I suggest that at the end of EVERY tool that a G94 is stated ie on or after the G80 line.....sort of like a safety code
this will stop (ID ten T) errors......(change ten to 10 )