Manual Probing

[vadim]

Hi guys,

I was wondering if it is possible to do manual probing without having physical probe.
Pretty much what I want to do is at the probed locations jog until material is hit and set probed Z to zero at that location.

To illustrate my problem a little more:
The CNC I have doesn't have a probe and to get it in will require modifying what now works quite well for me.
I'm engraving in plastic about 4.5mm thick. The piece is relatively flat to start with, however across the distance of about 150mm z is ~0.2-0.4mm off. I'm sure that can be corrected with just about 4 or 5 probe points at the edges(+ or or few in the middle).

I can more or less see how this can be achieved by setting first probed point z to 0, and then the others to the offset relative to that(say +0.1 or -0.2 etc). I'm not familiar with gcode commands per se, but I can sortof see what's going on in the file with probe locations.
I was wondering of doing something like so:
1) Generate new gcode file from AutoLeveller
2) Manually probe at the probed locations
2) Open up the gcode file and manually put Z coordinates for probe locations, but I'm not sure how to assign the right value and what format to use


Since if I'm the only one interested in such feature it's unlikely it will be developed just for me, but if someone could point me in the right direction please..

[vadim]

Just to continue my thought process. Is the following possible.
1) Have GCode that positions the mill at the probe location but does not move along Z axis. It just awaits probe signal.
2) I remap the e-stop to be probe and after manually locating the 0 of the surface, hit the e-stop indicating that probe has touched

[daedelus]

I think I see what you mean,

First of all, to manually set the Z, you can just jog down to the surface and touch off the Z axis to 0.22 or -0.14 or whatever. This will set the Z for all locations however so you will not get any AutoLevelling effect like you need.

There is a planned update where Z values are persisted and written to a separate file. The idea here is that this probe process is kept separate from the milling process so that the probe values can be re-used many times without physically re-probing. In your case, you could manually edit the values in the probe output file and then feed the probe output file back into AutoLeveller which will generate a "levelled" GCode file from these values. This would do what you need I think?

As for when this update will be done, I really wouldnt like to guess.

[Country_Bubba]

To continue what James is saying, when you probe; your not setting z=0 but are setting a variable to what the Z value is. Then you go to the next probe point and set another variable to its Z value.
Then when running your program, it checks against the various variables to adjust the Z height.

What control program are you using? Mach3 and Linuxcnc have the necessary software to handle the probing and variable assignment.

[daedelus]

Art is correct of course and has made me realise something.

If you run code through the AutoLeveller, you will see lines like this:

Code: Select all

#500=#5422
G0 Z2
G0 X-72.3148 Y-66.8981
G38.2 Z-1 F100
#501=#5422
G0 Z2
G0 X-62.1816 Y-66.8981
G38.2 Z-1 F100
#502=#5422
G0 Z2
G0 X-52.0484 Y-66.8981
G38.2 Z-1 F100
#503=#5422

#5422 is the variable which holds the current Z position and #500 onwards is the variable which the AutoLeveller refers to in milling later. So what you could do is replace the #5422 variable with you own number. You can then remove the probe lines before it. So the above code would become:

Code: Select all

#500=0.012
#501=0.056
#502=0.023
#503=0.034

for example. I think this will do what you want.

[vadim]

Hi guys,

Great answers! Thanks!

for example. I think this will do what you want.

Yes, that's exactly what I've been thinking about doing, I just wasn't entirely sure what the format of the variable(and variable assignment) was. Now, I do So that's precisely what I need. I can just manually run through a few probe points, note the position and assign them correctly. Will give that a go!

Mach3 and Linuxcnc have the necessary software to handle the probing and variable assignment.

I'm with Mach3. Are you saying there's an automatic way I can get Mach3 to do this assignment where I myself jog the Z axis? That would be great... means no manual file editing for me

Code: Select all

#500=${currentZ}
#501=${currentZ}
#502=${currentZ}
#503=${currentZ}

The idea here is that this probe process is kept separate from the milling process so that the probe values can be re-used many times without physically re-probing. In your case, you could manually edit the values in the probe output file and then feed the probe output file back into AutoLeveller which will generate a "levelled" GCode file from these values. This would do what you need I think?

Yep, that would also do the trick. It's very similar to just assigning probe Z variables in the GCode file itself; just much more flexible when you have and reusable.

[vadim]

Just a follow up:
Did manual measurements and assigned the 4 corner variables to the right values and everything worked beautifully!
Thanks for your help guys.

[Country_Bubba]

Fantastic, glad it worked for you!!!!

[paulnd]

Hi,

I'll be very grateful if someone could explain how to do this with Linux CNC please?

Paul

[Country_Bubba]

If you haven't done so, go to:
http://www.autoleveller.co.uk/autoleveller-guide/

and the instructions are there. I think this is what your asking. If not, please refine your question and we will try to help.