Nomad: tool probe gcode? (linux)

Software
1

Hey all,

I have paired a raspberry pi 3 up with my Nomad 883. On the rpi, I am running bCNC.py as the gcode sender.

So far for homing/probing, I have $H to home, but I am unsure what to use for tool length probing.

I suspect Carbide motion sends $H, then some G0 command to jog to the height sensor, then maybe some G38.2 command…

Could anyone tell me what the actual gcodes that are used for the nomad home/probe?

Thanks!

2

I believe it is the standard measure tool command.

3

These are the supported G Codes:

http://carbide3d.com/docs/list-of-supported-gcodes

I’ve had a question outstanding to C3D for some time - Edward specifically - about what the native G codes are on the Nomad. I have good reason to believe the list is seriously out of date and/or incorrect.

mark

4

There’s some documentation on this on the Shapeoko wiki: Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable

I believe the command which you want is:

G38.2 Z-26 F100

where G38.2 is the command, Z-26 indicates that you are less than 26mm above the point you wish to measure (adjust that number as needed to match your machine position and stock size), and F100 is the speed at which you wish to move (adjust depending on your patience or sense of safety and reaction time).

5

@WillAdams have it right. This is the G38.2 command. bCNC drives this perfectly.

For G38.2 to work, one has to tap into the tool length probe wires (the “button” on the bottom, left of the Nomad to help with tool change). One wire has to be extended to the surface you are probing (assuming it is conductive) and the other wire has to be connected to the probe (usually a tool or a 1/8’’ metal pin).

Tool change also uses G38.2 to work and this pair of wires is the only way to report contact back to GRBL.

6

I found this sequence worked ok…
$H; g21; g91; g0 x-216; G38.2 Z-70 F100; g0 z+10

it ends 1 cm above the probe tip button

7

I’ve captured command their Carbide Motion app sends to the device for this.

Here is the sequence:

N0G0X-2.500Z-5.000
N0G0Z-35.000
N0G38.2Z-105.000F800.0

N0 G4P0.005
N0G0Z-79.675
N0G38.2Z-182.675F200.0

N0 G4P0.005
N0G0X-8.000Z-5.000
1 Like
8

any chance you also have the x y motions it uses?

9

X is included in the first line. Y is taken from the last position after $H. Which is -5 I believe.

10

Ah, how strange, I was just looking at pictures and it appears on the website that the tool probe point is now on the far right where on my nomad it is on the far left. That would explain the large difference in X for probing we have.

11

Yes, in mine the probe point is on right, close to the homing area.

12

Were you able to get this working on your Nomad? I am trying to set up bCNC for my Nomad now and I am running into the same issues. How do you configure bCNC to do the tool probe at the start of each g-code file run? Do you have to manually alter the .nc file or can the program be configured with the parameters? Any information you can share about how you got yours working would be appreciated.

Thanks

13

bcnc works great. I do not end up using the nomad tool probe button feature.

I usually just: home, then zero X/Y, then do the paper drag technique for my zero Z.

I do have to re-zero on tool changes.

1 Like
14

All of the tool probing logic is in Carbide Motion, so it won’t work in bCNC (except as a normal probe input).

-Rob

15

Thanks Rob, I appreciate the reply.