Prompt CNC machine operators to QC parts!
All we need is a sub routine for the Haas control and a direct line of G code for PathPilot. This video covers how to use manual NC pass throughs instead of modifying the post processor. This can also be used to incorporate photos, videos, and even probing routines!
Haas Instructions & Sample Code
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 | To run this 10th part check as a subroutine + alias code 1) Manual NC pass through in the CAM file: IF [[#3901 MOD 10] EQ 0] M157 2) Copy program 9005 below: % O09005 N30 M109 P10501 (Press Y when 10th Part QC complete) ; IF [ #10501 EQ 0. ] GOTO30 (Wait for a key) ; IF [ #10501 EQ 89. ] GOTO40 (Y) ; GOTO30 (Keep checking) ; N40 (A Y was entered) ; GOTO50; N50 M99 % 3) Set 9005 as alias 157 (Resource for Alias: https://nyccnc.com/using-haas-alias-codes-to-center-machine-over-vise/ |
Tormach Sample Code
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 | % O01007 (Using high feed G1 F650. instead of G0.) (T16 D=0.4219 CR=0. TAPER=118deg - ZMIN=-1.1767 - drill) N10 G90 G94 G17 N15 G20 G4 P1 o177 IF [[#5650 MOD 5] EQ 0] (msg, Press Cycle Start when 5th Part QC complete); M0; o177 endif N80 M5 N85 M9 N105 M30 % |