Probing - error with the post processor for a smoothieboard

[bertrandletot]

Hello, 

I've got the post processor 
https://cam.autodesk.com/posts/post.php?name=smoothie

I' would try to probe my model before milling it.
But fusion always return me an error -> Error: Spindle speed out of range.
I suppose this post processor doesn't support a probing sequence ?
Can i change something ?

Regards, 

Bertrand

Information: Configuration: Smoothie Mill/Laser
Information: Vendor: Smoothie
Information: Posting intermediate data to 'C:\cnc\gcode\gravitrax\spacer-10.nc'
Error: Failed to post process. See below for details.
...
Code page changed to '1252 (ANSI - latin I)'
Start time: Sunday, March 29, 2020 12:50:18 PM
Code page changed to '20127 (ASCII - ɉ-U.)'
Post processor engine: 4.5633.2
Configuration path: C:\Users\bertr\AppData\Local\Autodesk\webdeploy\production\edf0a409d74cbc712b7f97f98853d005413e965e\Applications\CAM360\Data\Posts\smoothie.cps
Include paths: C:\Users\bertr\AppData\Local\Autodesk\webdeploy\production\edf0a409d74cbc712b7f97f98853d005413e965e\Applications\CAM360\Data\Posts
Configuration modification date: Sunday, March 29, 2020 12:47:05 PM
Output path: C:\cnc\gcode\gravitrax\spacer-10.nc
Checksum of intermediate NC data: fecb14329e350526d139fbe58b7be604
Checksum of configuration: 65bf86b4cedf542d9955c06a38e0bb0e
Vendor url: http://smoothieware.org
Legal: Copyright (C) 2012-2020 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.7824
...

###############################################################################
Error: Spindle speed out of range.
Error at line: 516
Error in operation: 'Probe WCS1'
Failed while processing onSection() for record 315.
###############################################################################

Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Sunday, March 29, 2020 12:50:18 PM
Post processing failed.

[Richard.stubley]

Hi @bertrandletot,

What probe have your got installed?

And do you know what macros you call manually to do use the probe normally?

[bertrandletot]

Hi richard, thanks for your time

For the moment i'm just trying with this kind of probe more a edge finder
My cnc machine is an hobby.
And after that with a real probe https://drewtronics.org/s5000led

A don't have a macro now. That was just my idea to see what fusion use to do xy probing, what's the best gcode to do it ?

But maybe i'm taking the wrong direction ?

Bertrand

[bertrandletot]

Hi Richard, thanks for your time, 

Now i'm using a basic probe like this one, kind of edge finder

And after https://drewtronics.org/s5000led

For the moment i don't use a macro, the idea was to see what code fusion 360 would create to do the job.
But maybe i'm taking the wrong direction ?

Regards

Bertrand

[Richard.stubley]

Ok, this isn't going to be easy but who says I don't like a challenge 🙂

This is going to need a fair amount of testing from yourself to get it to work, I will of course be helping along the way but just need to check you are ok to spend the time on your end also.

Basically we re going to have to write our own macros to run on your machine. As standard set does not currently exsist, hence the post error.

From what I can see it should be possible. 

This is what I ave found so far.

The smoothe does support probing see probing section. http://smoothieware.org/cnc-mill-guide

This takes you to here http://smoothieware.org/zprobe

Which for more detail takes you here http://linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G38-probe

So my question to you is do you currently have your probe wired to the controller?
Do you know if i currently works?

If so try this 

G91

G38.2 X10.0 F50.0

This should just incrementally move the probe 10mm in the X direction.

Try this first where the probe will not touch anything, you should get some kind of error saying the move has finished and you didn't touch anything.

Next, run that code again where you know the probe will trigger and see what happens, do this very carefully the machine should stop when the probe triggers.

Now try this 
(LOGOPEN,probe-results.ngc)

G91

G38.2 X10.0 F50.0

(LOGCLOSE)

This should create a log file with the coordinates the machine was at when it triggered.

I have no idea where this log file will be saved. 

Finally try this

G91

G38.2 X10.0 F50.0

#5221 = #5061

This should set the G54 X value to the X triggered point.

Please read through the links I have sent over before running anything as they describe procedures in setting up the probe. Also please note this is development work so you are doing it all at your own risk, I will help as much as I can but I can't be responsible for any damage to the machine.

If you don't want to spend the time on this then that is fine but I'm more than happy to help work on this together. 

[bertrandletot]

Hi richard, 

Sorry for the delay, my last two messages just did not want to appear in this post.
I've found the notification in my spam folder.

So, yes my probe is connected
probe in z -> G30 Z19 -> working
probe in x -> G38.2 X10.0 F50.0 -> return me a distance

I' will try tomorrow the #5221 = #5061

I've found

5221-5230 - Coordinate System 1, G54 for X, Y, Z, A, B, C, U, V, W & R. R denotes the XY rotation angle around the Z axis. Persistent.

5061-5069 - Coordinates of a G38 probe result (X, Y, Z, A, B, C, U, V & W). Coordinates are in the coordinate system in which the G38 took place. Volatile.

Next step ?
Move the probe to get the y axis
G38.2 Y10.0 F50.0
#5222 = #5062
?

I've a bad sciatica, my movement are limited 😞
But i certainly want to spend time on this.

Thanks Richard

Bertrand

[bertrandletot]

Hello, 

Taddaaaa, i've made my macro and it's working well for the moment.
;probe z
G38.2 Z-10 F50.0
G10 L20 P1 Z19.4137 ;height of the probe
G0 Z25
G91 ;relative
G0 X-20
G90 ;absolute
G0 Z18.5
G4 S1 ;pause 2s needed avoid error with the probe
G38.2 X20.0 F50.0
G10 L20 P1 X0
G0 X-4
;probe y
G91 ;relative
G0 Y-20
G0 X20
G90 ;absolute
G4 S1 ;pause 2s needed avoid error with the probe
G38.2 Y20.0 F50.0
G10 L20 P1 Y0
G0 Y-4
;home G54
G0 X0 Y0 Z19.4137
M2

;still need to remove the with of the probe

Working in progress
Bertrand

[Richard.stubley]

Hi @bertrandletot,

Excellent work I will start to out this in the post processor so we can get automatic output. 

Another thing we will have to look at is calibration. but one step at a time. At the moment where we are just finding the centre position of a part which is fine but if you touch 1 edge then we will be out by the radi of the styli.