Hey

Is there a way (in format 2) to keep Z from going home (TC position) at the end of a program (M30 or M2)?

TIA

What's your scenario? Single tool program and trying to save time?

Hi Darebee

Show us what you have at the end of the program

Hi Guys,
If you want to avoid having the head going up to TC position after completing a part use M99P# (program jump). If you are only using one tool and don't want the spindle orient every time, set the P# for the line # after the T#M06 (this being the first line of the program. Write your program so after the operation is complete move Z to where you want it and then move to X&Y you want then M00. This will park the table and stop the spindle. No way to leave spindle running except by using a G04 with a huge P factor but this is not safe at all. When the next part is ready to go, one push of the button is all you need. This also works for you guys that hate to push start twice at the beginning of a program. I use only Format 1 but the M99 is supposed to work the same in both.
Give it a try. The P# = the sequence number you want to jump back to to start the program again.
Gary

Yes. single tool, really simple, put parts through.
Looking to save 44.5" of Z up and down.
Haven't got going on the machine yet today but the program looked like this Friday.

%
N2 G00 G40 G49 G80 G90 G17
N3 (Slot Mill - 5/16 T Slot cutter)
N4 G59 X18.25 Y2.
N5 S2300. M3 M8
N6 Z0. H9
N7 Y.35
N8 G1 Y.228 F20.
N9 X6.25 F30.
N10 Y.35 F40.
N11 G0 X18.25 Y2.
N12 M05 M9
N13 M30
%

I believe we have discussed this before.
Usually it works out that by the time I spend 1-2 hours "OPTIMIZING" a program that will be used once. I could have run my part (albeit inefficiently) ate my lunch and cleaned out the chips.
So - if it don't work right - I just do it the way it will work and forget about it.

G4P66000 will put the control in an endless dwell with the spindle and coolant still running. Resume operation with start or auto button. I use it and it works well. It will save you all that wasted Z axis motion on a single tool job.

That is not very safe.
Changing parts beside a running spindle while being blasted by coolant is not going to happen with me.

I was hoping for some stupid little idiosyncrasy that I had missed.

I could easily do a sub program call with many repeats and toss in a spindle off, coolant off and M00. (Next time)

I can hardly deburr the parts as fast as they are going through and am almost done the job.

I should have worded that a little differently. You have the option of leaving the spindle and coolant on. Obviously no one is going to stick their face(intentionally anyway) into a coolant bath. This should do what you were looking for. Spindle and coolant are both off and restart is one push of the start button.
%
N2 G00 G40 G49 G80 G90 G17
N3 (Slot Mill - 5/16 T Slot cutter)
N4 G59 X18.25 Y2.
N5 S2300. M3 M8
N6 Z0. H9
N7 Y.35
N8 G1 Y.228 F20.
N9 X6.25 F30.
N10 Y.35 F40.
N11 G0 X18.25 Y2.
N12 M05 M9
N13 G4P66000
N14 M99P2
%



Dave

Another way is with the L routine...(I'm in Format 1)
example I'm using to face a part, L100 to M17 is the subroutine, and L101.1 at N215 tells the sub to repeat till the cows come home.

The Y10. at N170 brings the table to me for loading after the spindle and coolant have shut off.

N5 O476(FACE PART)
N10 G80G90G49G40G17M5M9
N15 L100
N20 M3 S1200
N25 G0 X1.5 Y5. E1
N30 G0 Z.2 (.200 OVER Z0)
N35 G1 Y-5. F20.
N40 G0 Z.5
N45 Y5.
N50 G0 Z.16 (.16 OVER Z0)
N55 G1 Y-5. F20.
N60 G0 Z.5
N65 Y5.
N70 G0 Z.12 (.12 OVER Z0)
N75 G1 Y-5. F20.
N80 G0 Z.5
N85 Y5.
N90 G0 Z.1 (.1 OVER Z0)
N95 G1 Y-5. F20.
N100 G0 Z.5
N105 Y5.
N110 G0 Z.06 (.06 OVER Z0)
N115 G1 Y-5. F20.
N120 G0 Z.5
N125 Y5.
N130 G0 Z.02 (.02 OVER Z0)
N135 G1 Y-5. F20.
N140 G0 Z.5
N145 Y5.
N150 G0 Z.005 (.005 OVER Z0)
N155 G1 Y-5. F20.
N160 G0 Z0. M8 (FINISH CUT AT Z0)
N165 G1 Y5. F18.
N170 G0 Y10. Z.5 M9
N175 M5
N180 M1
N185 M17
N190 M30
N195 T2 M6 (2.5 SS FACE MILL)
N200 M3 S1200
N205 G0 G90 X0 Y0 E1
N210 H2 D2 Z1.
N215 L101.1
N220 M2

Thanks Dave.
I must save that to try on my next similar type programming need.

Fizz - maybe my terminology is wrong but when I mentioned sub program earlier an "L routine" is what I meant.

DareBee,
Figured that's what you meant...I was just throwing out an example. That seems to be how I learn best, so was just trying to help.

thanks bud
I didn't mean anything negative (if that is how I came across).

Loving all the examples of how to do this. I like some of these better than what I'm doing now. (Format 2)

G20
G0 G17 G40 G80 G90
T1 M6
M3 S2000
G90 E1 X0.28 Y0.28
G43 Z2.5 H1
#:LOOP
M8 D1
Z0.1
G1 Z-0.75 F50.
G41 X0 F15.28
Y-3.28
G40 X0.28
G0 Z0.1
M5 M9
Z2.5
Y9.
M0
( LOAD NEXT PART )
M3 S2000
G90 E1 X0.28 Y0.28
#GOTO :LOOP

Dammit guys

I didn't want to spend time on this, but you have forced my hand ;-)

Here is what my loop would have looked like (it is the same program (unless I made a mistake)).

%
N2 L200
N3 G1 Y.35 F99.
N4 Y.228 F20.
N5 X6.25 F30.
N6 Y.35 F40.
N7 G0 X18.25 Y2.
N8 M05 M9
N9 M00
N10 M3 M8
N11 M17
N12 M30
N13 G00 G40 G49 G80 G90 G17
N14 M6 T9 (Slot Mill - 5/16 T Slot cutter)
N15 G59 X18.25 Y2. (Datum Y Back - X Left)
N16 S2300. M3 M8
N17 Z0. H9 (Tool Zero at Cut height)
N18 L2100
N19 G0 G90 H0 Z.0
N20 E0 X-5. Y9.8
N21 M05 M9
N22 M30
%


Daves is shorter, I will try it the next time I need this functionality.

I believe we have discussed this before.
Usually it works out that by the time I spend 1-2 hours "OPTIMIZING" a program that will be used once. I could have run my part (albeit inefficiently) ate my lunch and cleaned out the chips.
So - if it don't work right - I just do it the way it will work and forget about it.

I just caught this part of your post.

I'm with ya on that. I've got 3 machines so I try not to sweat small things too much. There's almost always one sitting anyway waiting for a new part so optimizing only helps on very long programs.

Darebee--
Look at line 18. I don't think you mean to define subroutine #2100. I think you mean to say L201.

Neal

Thanks Neal, we are both wrong (so far).

It SHOULD be L201.1

sorry

I am running these again.

Program works perfect.

Thanks