Using cutter comp eia/iso on M2
Hello,
I'm using EIA/ISO/ format on M2 controller. I want to offset (G41) my cutter, when I go to the tool offset page and put -.005 it just goes that much deeper with z axis. I see that one cannot put a negative value in the tool data page. Does anyone know how to offset on the x and y plane? Thanks in advance.
Re: Using cutter comp eia/iso on M2
Hello
I have changed the parameters but i still dont get the tool offset lenght correct.. my tools go below the Z surface..
O1001
(T4 D=10. CR=0. - ZMIN=-1. - FLAT END MILL)
N10 G90 G94 G17 G49
N15 G21
N20 G53 G0 Z0.
(BORE1)
N25 T4 M6
N30 S6000 M3
N35 G54
N40 M8
N45 G0 X32.678 Y-119.177
N50 Z100.
N55 G0 Z22.
N60 G1 Z20. F500.
N65 G41 X31.778 Y-113.177
N70 G3 X25.778 Y-119.177 I0. J-6.
N75 X39.578 Z19. I6.9 J0.
N80 X25.778 Z18. I-6.9 J0.
N85 X39.578 Z17. I6.9 J0.
N90 X25.778 Z16. I-6.9 J0.
N95 X39.578 Z15. I6.9 J0.
N100 X25.778 Z14. I-6.9 J0.
N105 X39.578 Z13. I6.9 J0.
N110 X25.778 Z12. I-6.9 J0.
N115 X39.578 Z11. I6.9 J0.
N120 X25.778 Z10. I-6.9 J0.
N125 X39.578 Z9. I6.9 J0.
N130 X25.778 Z8. I-6.9 J0.
N135 X39.578 Z7. I6.9 J0.
N140 X25.778 Z6. I-6.9 J0.
N145 X39.578 Z5. I6.9 J0.
N150 X25.778 Z4. I-6.9 J0.
N155 X39.578 Z3. I6.9 J0.
N160 X25.778 Z2. I-6.9 J0.
N165 X39.578 Z1. I6.9 J0.
N170 X25.778 Z0. I-6.9 J0.
N175 X39.578 Z-1. I6.9 J0.
N180 X25.778 I-6.9 J0.
N185 X39.578 I6.9 J0.
N190 X33.578 Y-113.177 I-6. J0.
N195 G1 G40 X32.678 Y-119.177
N200 G0 Z50.
N205 X33.178 Y-118.177
N210 Z1.
N215 G1 Z0. F500.
N220 G18 G3 X32.178 Z-1. I-1. K0.
N225 G17
N230 G1 G41 X31.678 Y-113.177
N235 G3 X25.678 Y-119.177 I0. J-6.
N240 X39.678 I7. J0.
N245 X25.678 I-7. J0.
N250 X31.678 Y-125.177 I6. J0.
N255 G1 G40 X32.178 Y-120.177
N260 G18 G2 X33.178 Z0. I0. K1.
N265 G0 Z100.
N270 G17
N275 M5
N280 M9
N285 G53 G0 Z0.
N290 M30
Re: Using cutter comp eia/iso on M2
ok so i got it to read diameter offset. but not lenght... i still need to put tool lenght into the EIA offset page.
Re: Using cutter comp eia/iso on M2
Quote:
Originally Posted by
MrMazak
Check parameter OP2 and set it for what you need
OP2 bit 0 Tape Puncher (0=EIA 1=ISO)
bit 1 Tool Length Offset (0=Only Z axis 1=Any axis)
bit 2 Tool Offset (0=D code 1=H code)
bit 3 Tool Dia Offset (0= Diameter in TOOL DATA is active 1 = not active)
To use Mazatrol Tool Data in EIA programs set all to 0 and delete any G43 and D or H callouts in your program just use T01 to call tool #1 and it will use the Tool length and Actual Dia. from the TOOL DATA page.
Mr. Mazak,
Hi. I did what you said and OP2 for me is 224 right now. Deleted all the G43 H and G42 D codes (a hard thing for a G-code guy to do!) and yes the machine magically uses the Mazatrol tool length.
I must be violating another fundamental rule though, as I try to take a .125 endmill in to open up a .178 semi-finished (without comp) milled hole to .188. I get "512-Tool Diameter Offset Impossible". I would think it IS possible to get tool comp working in such small hole.
Thanks for your reply!