My new Shapeoko 3 is it just me?

[ArtF]

Wow, thats really curious. It looks to everyone so far as if its ignoring that line, but it shouldnt.. I wonder if maybe it doesn't like comments, or a tool change command, perhaps you should remove all the unimportant lines at the start to see if its that..

How about we change this..

G20 (Imperial Mode)
M5
M6 T5
M3 S1750
G0 X3.445  Y3.307  Z0.250  A0.000
G1 Z-0.050  F20.00

to this

G20
M3 S1750
G0 X3.445  Y3.307  Z0.250  A0.000

  If you zero your table with Z 1" in the air, and run the above 3 lines, does the tool end up .25" in the air, at a
point 3.445 " to the right and 3.3" back? If not, where DOES it move to?

Art

[Joakim]

Art:

Interesting to see if it works without the unimportant lines.
From the GRBL github Wiki I see, that M6 is unsupported and the A parameter in moves.

Joakim

[Richard Cullin]

if you make your gear in millimeters , does that cut properly on the shakeopo

[Rocket]

if you make your gear in millimeters , does that cut properly on the shakeopo

No, I tried that also.

[kit]

Rocket: This machine seems to be causing some serious trouble! I've recently got my DIY CNC router up and running using LinuxCNC and a cheap Chinese control board and stepper drivers from eBay. It works without any problems with the G-code from Gearotic Thoughts as long as I remove the 'A0.000' from the initial G0 line of code. Good luck with getting your machine working as you want it.

Art: Please explain how to prevent the A axis command being produced.

Kit

[Richard Cullin]

is it possible the console program that sends the gcode to the shakeoko has a "safe work height" or a "clear height"  or a "tool change height"
that's set to 0 or a negative value that mucks up the first move .

[ArtF]

Kit:

  There is a file int eh Gearotic folder called "DefaultMill.pst" , this is the post processor.
I dont recommend changing it, BUT, I do recommand copying it to "MyPoster.pst" which
you then select as your default post processor.

Open that file and youll see..

!X%.3f !  -- This is the X coordinate letter and precision
!Y%.3f !  -- Same for Y
!Z%.3f !  -- Same for Z
!A%.3f !  -- Same for A

  Change it to

!X%.3f !  -- This is the X coordinate letter and precision
!Y%.3f !  -- Same for Y
!Z%.3f !  -- Same for Z
!          !  -- Same for A

  And the A will go away.  Changing the X%.3f to x%.4f would give you 4 decimals points for example..

Art

[ArtF]

Rocket:

I have to say, in answer to the tagline of this post, its the shapeoko.. lol

 In truth it seems not a terrible machine, but its software interface leaves a whole
lot to be desired. I suspect someone from shapeoko may have to explain why that
first line keeps getting ignored.
  Excellent suggestions from folks, but iot seems nothing we try gets it to run properly,
what did it do on that 3 line test I listed.. did it move at all?

G20
M3 S1750
G0 X3.445  Y3.307  Z0.250  

 If you zero your table with Z 1" in the air, and run the above 3 lines, does the tool end up .25" in the air, at a
point 3.445 " to the right and 3.3" back? If not, where DOES it move to?

[endquote]

Art

[Nate]

It looks like the shapeoko uses grbl.  If it does, these -

http://www.shapeoko.com/wiki/index.php/ ... ds.5B33.5D

In particular the "?" and "$#".  Might be helpful in figuring out what's going on.

[ArtF]

Nate

looking at the software thats sending it Im not sure he can query it.. but I guess
thats more a question for whoever supports Carbide.. Have to say I had never heard of it,
I must be sheltered...

Art

[Rocket]

Art,

When I run this command:
G20
M3 S1750
G0 X3.445  Y3.307  Z0.250  A0.000

The spindle does not move at all, it just says job finished and nothing happens.

So I removed the A0.000 and the spindle moved left and back about
3.5 inches with NO change in up or down.....!!!!!

G20
M3 S1750
G0 X3.445  Y3.307  Z0.250.........................works.......................!!!


RRRRR

[ArtF]

Rocket:

Perform the post I wrote on removing the "A" output from gearotic, and add a "G20" to your prologue
and youll probably be fine then.. :)

Art

[Rocket]

Art,

I just went back  to the file I posted on page 8 of this thread:

File:  999straight from Gearotic.tap. (1078.63KB)
I removed the A0.000 and added G20.

No luck, the same as before, Z drops down and cuts before it should cut...

RR

[ArtF]

Rocket:

Remove the line with M3 and the one with M5 and the one with the T on it,, any difference?

( if your spindle is automatic this means it wont turn on by itself.. or off)

Art

[Rocket]

Art,

This Post is finally Toast!!!

We got it!!!

Attached see file that works without dragging cut to start area.

I moved the line:  G0 X3.445  Y3.307  Z0.250
under G20..............just a wild guess....................>>>>>>>>>>>>>>>

(yes...Yes...Yes...)
(This really works...)
(Art is a Wizard)

G20
G0 X3.445  Y3.307  Z0.250 
M3 S1750
G1 Z-0.050  F20.00

Also see attached file that shows simulation of start (green line is finally
above the drawing!!!

Wow.......................

RRRRRRRR