[Steve Seebold]

This is the code created by the "generic Tormach post" on hsmxpress. It works on the machine!
Trouble is, this post fails for general machining giving "radius too small" errors at certain points.

%
(DRILL1)
(T1 D=0.25 CR=0. TAPER=118DEG - ZMIN=-0.8651 - DRILL)
N10 G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
N20 G20
N30 G28 G91 Z0.
N40 G90

(DRILL1)
N50 M998
N60 T1 G43 H1 M6
N70 S1000 M3
N80 G54
N90 G0 X-0.2865 Y0.
N100 M9
N110 G0 Z0.6
N130 G0 Z0.2
N140 G98 G73 X-0.2865 Y0. Z-0.8651 R-0.34 Q0.0625 F40.
N150 G80
N160 G0 Z0.6

N180 M9
N190 G28 G91 Z0.
N200 G28 X0. Y0.
N210 M30

(DRILL1)
(T1 D=0.25 CR=0. TAPER=118DEG - ZMIN=-0.8651 - DRILL)
N10 G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
N20 G20
N30 G28 G91 Z0.
N40 G90

What the heck is G64, G94 and G94.1?

I know G20 is IPM, but in Mach, once you program a G20, it stays that way until you change it. I have been running my machine for nearly 4 years, an I have NEVER used G20. NOT EVER.

My drilling programs start out:

G54
S3500M3
T1M6
G90G0X1.0Y.5Z1.G43H1M8
Z.1
G83G99X1.Y.5R.1Q.15F15.
X2.
X3.
X4.
Y1.5
X3.
X2.
X1.
G80M9
M5
M998
T2M6
S3500M3
G90G0X1.0Y.5Z1.G43H2M8
Z.1
And so on for the rest of the program.

I don't use line numbers because in long programs, line numbers take up take up way too much program space and I have run programs on my machine that are as large as 300,000 lines long.

[widget_maker]

(DRILL1)

And so on for the rest of the program.

I don't use line numbers because in long programs, line numbers take up take up way too much program space and I have run programs on my machine that are as large as 300,000 lines long.

But Steve, this was created with a mach3 post program.

[SCzEngrgGroup]

(DRILL1)
(T1 D=0.25 CR=0. TAPER=118DEG - ZMIN=-0.8651 - DRILL)
N10 G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
N20 G20
N30 G28 G91 Z0.
N40 G90

What the heck is G64, G94 and G94.1?

G64 sets the path blending tolerance, which helps you tune the program for best performance on your machine.

G94 sets "units per minute" mode, rather than "units per rev" or "inverse time" modes.

G94.1? No idea.

I know G20 is IPM, but in Mach, once you program a G20, it stays that way until you change it. I have been running my machine for nearly 4 years, an I have NEVER used G20. NOT EVER.

Standard good coding practice, regardless of language, dictates setting ALL persistent modes at the start of any program, to be certain they are in the expected state. This recommendation is followed be nearly all CAM programs. This prevents problems if someone comes along and sets G21 when you're not looking, then you run one of your programs written for G20. Some people also do some jobs in G20, some in G21, and should not have to depend on their memory to remember to set the correct mode manually before each job. It's a safety, and strongly recommended. Cost is $0, and it can easily save a part or tool.

I don't use line numbers because in long programs, line numbers take up take up way too much program space and I have run programs on my machine that are as large as 300,000 lines long.

Space? Who cares? You have gigabytes of memory and storage, and Mach3 is perfectly happy running programs millions of lines long, with line numbers. It makes absolutely no difference in performance, and, for some people, makes the code more readable.

Regards,
Ray L.

[shred]

LinuxCNC is overall much more strict about G-code than Mach. Mach tends to ignore things it doesn't understand while that will throw errors in LinuxCNC. Btw, the error line numbers are those of the file and not the N-numbers. Those are largely optional.

G64 is something anybody doing engraving will want to pay attention to. In some cases it can round off corners quite severely.

[hall6ppc]

LinuxCNC is overall much more strict about G-code than Mach. Mach tends to ignore things it doesn't understand while that will throw errors in LinuxCNC. Btw, the error line numbers are those of the file and not the N-numbers. Those are largely optional.

G64 is something anybody doing engraving will want to pay attention to. In some cases it can round off corners quite severely.

Can you edit the values for G64 ? I though I read or heard somewhere you could ?

[SCzEngrgGroup]

Can you edit the values for G64 ? I though I read or heard somewhere you could ?

Of course. Either modify the post, or hand-edit the g-code.

Regards,
Ray L.

[hall6ppc]

Of course. Either modify the post, or hand-edit the g-code.

Regards,
Ray L.

What would some example code look like? I have never tried to use this setting ?

Thanks

[SCzEngrgGroup]

What would some example code look like? I have never tried to use this setting ?

Thanks

That depends on what CAM you're using. The POST is the part of the CAM that actually writes the g-code file. It is not part of PathPilot.

Regards,
Ray L.

[hall6ppc]

That depends on what CAM you're using. The POST is the part of the CAM that actually writes the g-code file. It is not part of PathPilot.

Regards,
Ray L.

Using Mastercam X8 . I might be able to edit my post or I can get my reseller to do it. Just not sure exactly what I am looking for as far as a value goes . Also not sure of what the value would represent either. I have never thought about editing the G64 value in MACH because I thought you could not .

Again Thanks for your help !

[shred]

G64 P0.005

for example will keep the tool within 5 thou of the programmed path.

LinuxCNC manual page: G Codes

Note that G64 - without P means to keep the best speed possible, no matter how far away from the programmed point you end up. I've seen it round corners 1/8" or more when blasting through plastic in G64-without-P mode.

[hall6ppc]

G64 P0.005

for example will keep the tool within 5 thou of the programmed path.

LinuxCNC manual page: G Codes

Note that G64 - without P means to keep the best speed possible, no matter how far away from the programmed point you end up. I've seen it round corners 1/8" or more when blasting through plastic in G64-without-P mode.

Thanks very much

! I believe I got it