Need Help!- Macro for changing Z depth on a facemill

[banshee1a]

I have a part that going to run on our Okuma horizontal mill with a 16i-MA control, that is over 220,000 bytes in size. The control can only store approx. 100,000 bytes so you can see my problem. The the tool paths for the first 1-1/2" are the same, so I was thinking of putting the tool path in a subprogram and writing a macro that would change the Z depths in the sub until it reaches a certain depth, but I don't have a clue on how to write macros, and they want to run these parts in a few days so I don't have a lot of time to learn what I need. Now the tool also retracts and moves to a different position several times for each depth of cut. Could somebody give me a hand on trying figure this out if its possible? I can set up a mobile pc that we have to drip feed the program, but the higher ups don't want this because of some problems that could arise if the operator has to stop and bail out to index the inserts or something. I have thought of also using a G10 to change the work shift, which we have done before, but there again they're worried the operator could mess something up.
Any help or ideas would be appreciated.

[psychomill]

Sounds like a good candidate for a macro loop or a "WHILE/DO" statement. I use this alot for tools that have many repetitive cuts that only change in Z. It could be a bit sketchy though if you're not used to some macro writing.

You're on a Okuma? Doesn't Okuma have a way to do internal subs? You can loop this as well.

Another way is to seperate your actual XY cuts into a sub. Strip any Z outputs in the sub except for the last retract to a clearance plane. Then you just sub program it all with M98:

XxxYyy
G1Z-.25F200.
M98P100

XxxYyy
G1Z-.5F200.
M98P100

XxxYyy
G1Z-.75F200.
M98P100


In case you're wondering... a While/Do loop is kind of like this:

#520=.25 (1st cut and each Depth of cut)
#521=.25 (Z Depth Counter)
WHILE[#521LE1.25]DO1
Xxx.xxYyy.yy (START POINT)
G1Z-#521 (Z DEPTH OF CUT)
M98P100 (SUB CALL)
#521=#521+#520 (ADDS Z FOR NEXT PASS)
END1

<REST OF PROGRAM>

This is a simplified one and doesn't have much for safety in it but maybe you'll get the idea. You have to be careful which variable numbers you choose because the machine may already be using them for various things like probes, machine base macros, etc. You could actually do this with only one variable but I like to keep things seperated somewhat for clarity and better adjustability.

[stevo1]

Psychomill has it hit right on the head. I would use a “while” statement for this. I like to add a bit more flexibility to mine that way if you do bail in the middle you can just change the Z-start depth(#1) and it will continue through. Ex. if your last pass was at Z-.12 then change #1=.12. I also like to use the local variables so you do not overwrite any variables that the machine may be using as suggested above.

Now this does not run a sub program. Depending on how many XY moves at each Z depth you have should dictate that. If there is only a few moves then I would use the below suggestion as is. Now if there are extensive amount of movements in the same Z then I would put those movements into a sub as Psycho suggested. All you would have to do then is put the M98 call right after the G0Z-#1 line in place of the XY Position to cut.

#1=0(Z-START )
#2=.354(FINAL DEPTH)
#3=.03(PICK)
G0X0Y0Z3.-----XY POSITION OF CUT, Z SAFE
WHILE[#1LT#2]DO1
#1=#1+#3
IF[#1GE#2]THEN#1=#2
G0Z-#1
G1X0Y0F.01M8---XY POSITION TO CUT
G0Z3.
X0Y0-----XY POSITION OF CUT
END1
M0

Stevo