My Program Skips Lines

[DroopyPawn]

I'm not sure why this code is skipping depth passes after the stops at the beginning. I'm trying to run the same contour code over and over and incrementing the depth by 0.02" each pass. For whatever reason, it goes from -0.02, to 0.06 to 0.10, to 0.14. It's skipping 4, 8, 12 etc. Did I do something wrong or is this a limitation of the Mach3 demo?

(File created using FlashCut CNC DXF Import)
(Import File: Dekley Bellcrank.dxf)
(Import Date: 11/20/2007)

(3/8" hole)
G00 Z0.20000
G00 X1.5525 Y0.3775
M0

(1/4" hole)
G00 Z0.20000
G00 X1.0775 Y0.3775
M0

(1/4" hole)
G00 Z0.20000
G00 X0.7575 Y0.3775
M0

(1/4" hole)
G00 Z0.20000
G00 X0.4375 Y0.3775
M0

(1/4" hole)
G00 Z0.20000
G00 X0.1175 Y0.3775
M0

(insert 1/8" endmill)
M0

G00 Z0.20000
G00 X0.00000 Y0.06300
G01 Z-0.02000 F1.00 M98 P1
G01 Z-0.04000 F1.00 M98 P1
G01 Z-0.06000 F1.00 M98 P1
G01 Z-0.08000 F1.00 M98 P1
G01 Z-0.10000 F1.00 M98 P1
G01 Z-0.12000 F1.00 M98 P1
G01 Z-0.14000 F1.00 M98 P1
G01 Z-0.16000 F1.00 M98 P1
G01 Z-0.18000 F1.00 M98 P1
G01 Z-0.20000 F1.00 M98 P1
G01 Z-0.22000 F1.00 M98 P1
G01 Z-0.24000 F1.00 M98 P1
G01 Z-0.26000 F1.00 M98 P1
G01 Z-0.28000 F1.00 M98 P1
G01 Z-0.30000 F1.00 M98 P1
G01 Z-0.32000 F1.00 M98 P1
G01 Z-0.34000 F1.00 M98 P1
G01 Z-0.36000 F1.00 M98 P1
G01 Z-0.38000 F1.00 M98 P1

G00 Z1
G00 X0.00000 Y0.00000
M30


O1
G03 X0.06300 Y0.00000 I0.06300 J-0.00000 F18.00
G01 X1.67800 Y0.00000
G03 X1.67800 Y0.75600 I0.00000 J0.37800
G01 X0.06300 Y0.75600
G03 X0.00000 Y0.69300 I0.00000 J-0.06300
G01 X0.00000 Y0.06300
M99

[DroopyPawn]

Also, my Z-axis never seems to go deep enough with I run the program. But I've checked it while not running a program and the distance is true to what the DRO reads.

[Mitsui Seiki]

Try to put one or two "blind blocks" between the Z passes.

G00 Z0.20000
G00 X0.00000 Y0.06300
G01 Z-0.02000 F1.00 M98 P1
;
G01 Z-0.04000 F1.00 M98 P1
;
;
G01 Z-0.06000 F1.00 M98 P1
;
;
G01 Z-0.08000 F1.00 M98 P1

[DroopyPawn]

Yeah, that seems to have fixed it. But why would I need to do that?

[HuFlungDung]

I suppose it is difficult to say why, because it could be a result of the way the gcode is being interpreted. Special syntax rules may be required because the controller software may not have logic to correctly return to the main program using your syntax.

For example, to alter the syntax, try putting the subroutine call on a seperate line beneath each Z move.

You might also put the Z movement into the subroutine:
O1
G91 G01 Z-.02 F1.
G90
etc.

This would then permit you to write the main program with a single line calling for repeats, something like:
G00 Z0.20000
G00 X0.00000 Y0.06300
M98 P1 L19

[Mitsui Seiki]

Originally Posted by DroopyPawn Yeah, that seems to have fixed it. But why would I need to do that?

The control read more than just one block.It stays ahead and sometimes you need blind blocks to "force" it to read everything.

[Mitsui Seiki]

Originally Posted by DroopyPawn Also, my Z-axis never seems to go deep enough with I run the program. But I've checked it while not running a program and the distance is true to what the DRO reads.

Is your Z workzero set right?Tool lenght?Tool length comp. set to zero?

[DroopyPawn]

The tools are zeroed to the top of the workpiece. No compensation. I don't think I'd be losing any steps on the z-axis.

[Mitsui Seiki]

Is it working now?Or do you still have problems with the Z depth?

[DroopyPawn]

Well, it's not skipping from 2 to 6 to 10 anymore. I haven't checked the other yet but I will soon.

[Mitsui Seiki]

Ok.

[Paul_S]

Just place the subprogram call on a separate line. I always place subprograms or subroutines calls on a separate line.

So:
G00 X0.00000 Y0.06300
G01 Z-0.02000 F1.00 M98 P1
G01 Z-0.04000 F1.00 M98 P1
Would become:
G00 X0.00000 Y0.06300
G01 Z-0.02000 F1.00
M98 P1
G01 Z-0.04000 F1.00
M98 P1