Newbie- how do i program for incremental depths?

[mathewepperson]

i have about 4 month of machining experience and im working on a haas tm3. its kinda embarrasing to ask that question but i dont know. Im looking through the manual for the machine and the only thing i found is a L code that can be used with g91. But i dont know how to program the L code with anything. I read something on subroutines too. maybe that could be a way to solve my problem. The way i program it now is to copy and paste the first couple lines of code that i wrote and change the z depth, which takes alot of time. is there a way to do this quicker with other codes. and will it work with cutter comp?

[Pondo]

G91 changes the distances to incremental mode. That is, if you input X-3. it will move X 3" from wherever it is now. G90 needs to be in the next line to switch it back to Absolute mode (G91 and G90 are modal and will remain active in all following lines until the other is read).
An Example:

O3002 ( DERBY OP2 )
( T5 - .5C RESHARP - .46-.47- )
G17G40G80G90G0G54
N5
T5M6
( TOOL 5; .47 FINISH ENDMILL )
( .5C RESHARP - .46-.47- )
S1600M3
G90G0G54X-1.375Y0.
G43Z1.1H5M8
G0Z.1
G1Z0.F12. POSITIONS TOOL AT START POINT
M97P100L10 CALLS INTERNAL SUB STARTING AT N100 AND RUNS (LOOPS) IT 10 TIMES
G0Z1.1
M9
G91G28Z0.
G91G28Y0.
T1M6
M30 THE M30 DOES NOT NEED TO BE AT THE END
N100 SUBROUTINE START
G91Z-.01F12. FEEDS DOWN INCREMENTALLY .010
G90X1.375F24. FEEDS TO X ABSOLUTE POSITION OF 1.375
G91Z-.01F12. FEEDS DOWN .010 MORE
G90X-1.375 RETURN FEED TO START POINT
M99 END OF SUBROUTINE - RETURNS TO M97 LINE
%

The program is for cutting an undersize 1/2" slot .200 deep. It cuts .010/pass, .020 total for each sub. The M97 calls up an internal sub, the L tells it how many times to loop it (if no L, then it is 1). The code between the N100 and the M99 would be your toolpath.
It comes in handy for depth cuts and also if you rough and finish a profile with different tools. You can program the contour as a sub and then call it up for each tool. You can start off the part, move near the part while activating cutter comp, then do the profile. Clear the part, then G40. That way you can use different size tools.
This was useful for a couple years of fingerpecking programs at the control. The quick code is real handy, but once I went to a CAM system I'd never fingerpeck again.

[mathewepperson]

another question. is there a way to make the rapid on the machine faster? because it seems like it goes slow to me.

[offsetxyz]

The L in a HAAS is a loop command. In a canned cycle an L2 (no period) will repeat the line two times. If it is a hole position in a canned cycle it will drill twice or bore twice in the same spot. Usefull for when you want to run a boring bar in twice to eliiminate push off for a close finish. An L0 will make it skip that hole.

In incremantal mode G91 loop command can be used to drill a series of holes; for example every 1 inche by programing a canned cycle in a line that causes a 1" move in a certain direction then drills a hole and comes out then L# and it will repeat with move and all. See examples in HAAS operator's manual under canned cycles.

What you want for depth, in say milling down in hole, you would program a G02 or G03 circle with a z move. All must be in G91 incremental and a loop command a the end. The circle will repeat as many times as the L commands. This is common for cumputer generated thread milling programs.

Remember for a loop command to work right you must be in G91 or a canned cycle or the begining and ending point of the program line must be the same, as in a circle, for the L to function prorperly.

Do not try to take the L loop command to other machines because for example a Hyundia Kia KG63 uses a K loop comand in a cannned cycle.

[offsetxyz]

Yes loop commands work with cutter comp because maost computer generated thread mill programs assume a center line useing no tool diameter and CDC must be used to compensate for tool diameter

[mathewepperson]

imma try it and see how it goes. i guess ill do a dry run above the part so i dont crash. i got alot to learn about cnc but ill get there soon. it kinda sucks being the only cnc guy in the shop and having to learn everything by trail and error. but thats what it takes some times.

thanks for your replies and help.

Matt