Can't get a loop programmed

We have a little simple job that we just can't figure out how to do it with a Centroid control.

The part is only .032 thick and about 2" dia.and we have a .062 cutoff.
The material is 2" X 11" and we can make a good part but we want to do a loop and
and keep cutting about 100 pc per length. We give it a w-.095 (.062 cutoff+ .032 part) but it will go back to the beginning.
It seems like we can't mix Inc/Absolute programming.
We could do similar parts on the old fanuc 5t no problem.
Any help would be appreciated,
%

G99 G54
N10 G50 S1000
N20 G97 S900 F0.006 M44
N30 G00 T101
M03
M08
N40 G00 X2.02 Z0.1
N50 G94 X-.06 Z0
N60 G00 X2.02 Z0.1
N70 G00 X1.9138
N80 G01 X1.848 Z0
N90 G03 X1.942 Z-.0475 R.047
N100 G01 Z-.095
N110 G01 X2.02
N120 G00 X11.Z 5.M05
N130 T0100

N140 G50 S1200
N150 G97 S800 F0.002
N160 G00 T0505
M04
M08
N170 G00 X.0 Z0.1
N180 G01 Z-.12
N190 G00 Z0.0
N200 G01 X-.6
N210 G01 Z-.12
N220 G00 Z0.0
N230 G00 X.0
N240 G01 Z-.121
N250 G01 X -.660
N260 G01 Z0.01
N270 G00 X-11.9 Z 5.
N280 G00 T0500


N290 G50 S1200
N300 G97 S800 F0.006
N310 G00T0606
N320 G00 X-1.59 Z.1
N330
N340 G00 X-1.54
N350 G01 X-1.656 Z0
N360 G03 X-1.562 Z-.0475 R.047
N370 G01 X-1.5087 Z-.0472
N380 G01 Z-.095
N390 G01 X-1.656
N400 G02 X-1.562 Z-.0475 R.047
N410 G01 X-1.506 Z-.0466
N420 G00 Z.0848
N430 G00 X-11. Z 5.
N440 G00 T0600
N450 G00 M05

N460 G50 S1200
N470 G97 S800 F0.006
N480 G00 T0303
M03
M08
N490 G00 X2.0214 Z.0431
N500 Z-.095
N510 G01 X1.848
N520 G02 X1.942 Z-.0475 R.047
N530 G01 X2.02
N540 G00 X 11. Z 5.
N550 G00 T0300

N560 G50 S1200
N570 G97 S800 F0.002
G00 T0404
M03
M08
N580 G00 X2.148 Z-.095
N590 G01 X1.65
N600 G00 X2.1467 Z.1126
N610 G00 X11. Z 5.
N620 G00 T0400
N630 G00 Z-.095
N640 G00 M01
N650 M99 P10
%

Couldn't you shift over in G91, then back to G90?

i WILL TRY THAT Monday
Thanks

G90 G91 are for Mills only

Does the Centroid control have a G10 code like a Fanuc? If so, you could do something like G10 P0 W0.095 to shift the work coordinates over 0.095" after every part is made. You'd have to look at the exact syntax for your controller.

mc3608 said:

G90 G91 are for Mills only

Click to expand...

In what universe?

mc3608 said:

G90 G91 are for Mills only

Click to expand...

Mtndew said:

In what universe?

Click to expand...

Saying they are mill only is an absolute statement that isn't totally accurate as there are lathes that use them. That said I have a lathe with a Fanuc that G90 is a turning cycle

I tape cheat sheets to the side of each machine since all the builders refuse to get on the same page

Can you make your Z moves a #500 variable instead? Start #500 at .095", put the whole program in a do/while loop, and at the end of the loop increment #500 by .095", and set the loop to repeat until #500 is Greater Than 9.500"?

Not familiar with centroid controls, but I assume they can handle variables.

Centroid does have variables, but not a #500 series. Centroid's static variables (maintained indefinitely between jobs) are #150 - #159. Variables #100 - #149 are also available; they are reset to zero at the beginning of every job.

For this purpose, you could also do an incremental G50 to move your Z axis part zero. For example, "G50 W-2" would shift the Z axis part zero location left two inches.

You could also use CNC system variable #2600, which is the Z axis work offset (aka fixture offset, part zero). For example, "#2600 = #2600 = 2.0" would also shift the Z axis part zero location left two inches.

In either case, it is probably necessary to precede the coordinate-shifting code with the parse-pausing idiom: a separate line, with "IF [#50001]" if your control runs CNC11 or CNC12 software, or "IF [#6001]" if your control runs CNC7 or CNC10 software. This will ensure that the control does not change the part zero location during read-ahead in the job file, but instead does so only once the actual cutting has caught up to that point.

The G50 W-.095 does work
Thanks for everyone's input.