LATHE G1 not doing a heck of a lot (resolved)

[Sparrowgun]

Hey guys, got a strange one here.

Short version:

Made a Gcode file, loads fine, starts fine, does the rapids and tool change but as soon as it comes to the first G1 move it stops. Says 302: moving.... and does nothing after that. Code below.
The sample files work fine.
In CNC12 bench mode with closed loop steppers hooked up and working (mostly).
I can rapid all over the place without limits (kitchen table doesn't have limit switches hooked up)
I can G0 all over the place using the MDI.
I can't do a G1 move in the MDI, same thing as above.
I can change all of the G1s in the file to G0 and rapid the whole toolpath which is amusing.

Any ideas? I would like to make sure I can actually run a basic home made file before I do the hardware changes to my lathe.

Long version:

I have got CNC12 hooked up in bench mode, MM dimensions and running reasonably well. Have run a few of the sample files and they run through fine, though a bit weird as they are mostly in inches. With that working it was time to make my own basic Gcode file to make sure I can run one I jimmied up.

After a bit of mucking around I managed to get it to load up in CNC12 without any errors. Had to take a bit from one of the sample files and change it up as the post processor in the CAM i used adds a few things in CNC12 doesn't like. Basically added the material parameters up the top and something down the bottom so it knew the program was done.

Running the file as per the others it changes the tool and starts fine until it gets to the first G1 movement G01 X6.35 Z-0.5 F50. I have tried a few variations of the feed speed F0050, F0500, F1000 etc and the G number G1 or G01, no G1s on the lines below the first G1 command, no line numbers etc. If I change all of the G1s to G0s, it runs through the file fine, although very quickly.

I have searched on here, google, printed the manual and read through a bunch of it, mainly the Gcode bits, but haven't had much luck. Thought CNC12 may be looking for a spindle speed to make sure it's actually spinning before it tries cutting but I have the encoder disabled in the wizard so it should be manual. And it has no probs with the other files that include G1 moves.

If anything obvious pops into mind, please let me know. In the mean time I will keep mucking about.

Cheers,

Sam

Gcode I have been tootooing with. Early stages of a .44cal slug for my air pistol I'm going to make in copper.

N100 G21 ; mm measurements
:::: --- Stock Dimensions ---
:::: X- = -6.35, X+ = 6.35
:::: Z- = -30, Z+ = 0.0
:::: ---
N110 G50 S1200 ; max CSS spindle speed
N112 G40 ; Cutter Comp Off
N114 G00 X0.0 Z0.0
N116 G00 T0101
N118 G97 S500
N120 G00 Z0.5
N122 G00 X6.5
N124 G00 X7.764 Z0.0
N126 G01 X6.35 Z-0.5 F50
N128 G01 X-0.4
N130 G01 X1.014 Z0.5
N132 G01 X7.35
N134 G01 X8.35 Z-0.4
N136 G01 Z-2.322 F50
N138 G01 X7.764
N140 G01 X6.35 Z-3.736 F1000
N142 G01 X5.35 Z-7.007
N144 G01 Z-9.966
N146 G01 X6.005 Z-10.576
N148 G01 X6.205 Z-10.809
N150 G01 X6.35 Z-11.08
N152 G01 X6.85
N154 G01 X8.264 Z-12.495
N156 G01 Z-5.593 F50
N158 G01 X6.764
N160 G01 X5.35 Z-7.007 F1000
N162 G01 X4.756 Z-8.951
N164 G01 X4.73 Z-9.125
N166 G01 Z-9.127
N168 G01 X4.752 Z-9.289
N170 G01 X4.817 Z-9.438
N172 G01 X4.92 Z-9.565
N174 G01 X5.85 Z-10.432
N176 G01 X7.764 F50
N178 G01 Z-12.205
N180 G01 X6.35 Z-13.62 F1000
N182 G01 X6.319 Z-13.692
N184 G01 X5.989 Z-14.4
N186 G01 X6.85
N188 G01 X8.264 Z-15.814
N190 G01 Z0.414 F0050
N192 G01 X1.414
N194 G01 X0.0 Z-1.0 F1000
N196 G01 Z-1.296
N198 G01 X3.365 Z-1.002
N200 G01 X3.4 Z-1.0
N202 G01 X6.464 F0050
N204 G01 Z0.414
N206 G01 X5.05 Z-1.0 F1000
N208 G01 X5.203 Z-1.03
N210 G01 X5.333 Z-1.117
N212 G01 X5.42 Z-1.247
N214 G01 X5.45 Z-1.4
N216 G01 Z-3.2
N218 G01 X5.433 Z-3.317
N220 G01 X3.8 Z-8.658
N222 G01 X3.734 Z-9.009
N224 G01 X3.748 Z-9.365
N226 G01 X3.84 Z-9.71
N228 G01 X4.006 Z-10.025
N230 G01 X4.238 Z-10.296
N232 G01 X5.323 Z-11.307
N234 G01 X5.417 Z-11.44
N236 G01 X5.45 Z-11.6
N238 G01 Z-13.1
N240 G01 X5.413 Z-13.269
N242 G01 X4.885 Z-14.4
N244 G01 X8.35 F0050
N246 G01 Z-0.4
N248 G01 Z0.0
N250 G0 T0303
N252 G97 S500
N254 G0 X9.35
N256 G0 Z-1.0
N258 G01 Z-16. F0050
N260 G01 X4.35 F1000
N262 G01 X4.75
N264 G01 X2.35
N266 G01 X2.75
N268 G01 X0.35
N270 G01 X0.75
N272 G01 X-0.8
N274 G01 X9.35
N276 G01 Z-0.0 F0050
N278 G01 X0.0
N280 M5
N282 G28
N284 ; End of Program

[frijoli]

Possible you're in feed per rev? G98/G99

[Sparrowgun]

Quite possibly, I'll chuck a G98 in there and see if that helps. Thanks for the tip!

[cnckeith]

viewtopic.php?f=60&t=1043

[Sparrowgun]

Sorry about that Keith, I did read that before posting, made a report, didn't take any pics as I had shut everything down, forgot to attach report...

But the good news is, chucking a G98 in there does indeed make it work. I would have never picked this up. Up the top of CNC12 it says mm/min but when I do a G1 in the MDI and it starts the move it changes to mm/rev. I didn't notice this before and wouldn't have clicked, pretty much ever. Even after doing a G98 in the MDI it sback to going into mm/rev when doing a G1.

Tried a G98 before my first G1 in my program and it ran through without a hitch.

Thanks Frijoli! Exactly what I was looking for.