-
Helical Help
Just started working at this new place and we're upgrading cutters. We jumped from 12 IPM to 194IPM, Now here's the kicker, Step is .05 from .200, so the guys are having to reprogram all the programs. The way they were doing it was say with a XYIJ and z-.2 then next line z-.4 and so on till the pockets cut thru. Now we are doing .05 depth, and in a 3" plate that's adding a lot of lines and that's a mistake waiting to happen. I know you can use a L word and G91 but can't remember how to do it(been doing CAM for to long ) Can someone give me and example that I can follow that will work on a Fanuc 18i and or a Mazak? Thanks in advance....
-
This is quick and dirty but it give an idea to start with.
Uses macro B not simple loops.
Code:
#100=.5(RADIUS)
#101=0.01(START DEPTH)
#102=-1.5(END DEPTH)
#103=-0.05(STEP SIZE)
(----------)
#104=#101(SET CURRENT DEPTH)
(DO A G52 LOCAL WORK OFFSET HERE)
(IF YOU WANT TO MAKE A HOLE SOMEPLACE)
(OTHER THEN THE CURRENT WORK OFFSET)
(ZERO POSITION)
G0X#100Y0.0
G0Z[#104+0.1]
G1Z#104F200.0
#104=[#104+#103]
WHILE [#104 GT #102] DO1
G3I[-#100]Z#104F100.0
#104=[#104+#103]
END1
G3I[-#100]Z#102F100.0(LAST STEP)
G3I[-#100]F100.0(CLEANUP)
G1X0Y0Z[#102+0.01]
G0Z[#104+0.1]
G52X0Y0
