Autoleveller

Thanks again for an awesome addition to the GCode / CNC / PCB field !

I've only recently started using a CNC and this probing technique, but wanted clarification on the optimal way to use the Z height settings. Here's what I did.....

Load up my GCode file - it's in millimetres. "Probe Depth" setting defaults to -1, so I assume that this is -1mm (correct assumption?)

I then create the levelled GCode.

Load that up in Mach3 - check the probe setup is working, and then get my piece ready to etch. I get my X and Y cords properly zeroed relative to the work piece. I then lower the probe to around 6-8mm of the work surface, and zero Z. I then start Mach3's execution of the file.

Things appear to work correctly - in that I can see the machine probing across the matrix of locations set, and I think the probe is contacting the copper clad, but I can't watch the Digitize setting to see if it's recording a hit or not.

I have had a much better success rate than pre-levelling but I did have a couple of issues - one I suspect was the chuck worked loose and the bit could move, that I'll discount as error on my part. The other one is that I suspect my etch depth on my particular PCB material was not sufficient - I'm using PCBs from Jaycar (a local Australian brand ) and I suspect the material is, well, not manufactured to the highest of standards, and I suspect there's some variation that my etch depth wasn't able to account for; so I'll definitely take that into account in the future but I wanted to make sure that the probing should have been successful.

Is there any error when the probe does not touch before the Z height travel limit has been met? Or is there a way to prompt feedback through the message after probing (where perhaps it shows the "depth" below Z=0 that the last probe detected)

Any other thoughts/suggestions are greatly appreciated !

Edit: oh yeah, I really wondered if the Probe Height of -1 should have been -10? That would somewhat make the 3/8" or 10mm suggested starting height make sense, I guess.

Hi Poundy,

Great to hear you like the autoleveller

Load up my GCode file - it's in millimetres. "Probe Depth" setting defaults to -1, so I assume that this is -1mm (correct assumption?)

Correct. The autoleveller will read the GCode file you browse for and check for G20 and G21 commands which signify inches or millimeters then display inches or millimeters in the 'units' box at the top. In fact, if there is no G20/G21 in the file, it will prompt you for the units. All the values in the 'probe settings' will be for the stated unit type, in your case, millimeters. Feel free to change these values to whatever you want. The initial values are defaults which work well in most cases.

Is there any error when the probe does not touch before the Z height travel limit has been met? Or is there a way to prompt feedback through the message after probing (where perhaps it shows the "depth" below Z=0 that the last probe detected)

I mainly use LinuxCNC myself and in that, if the probe does not touch the surface before the Z limit is met, it pops up with a box which say something like 'the 'probe in' value did not change before Z depth reached' and it probably says something similar in Mach3. Mach 3 users can either confirm or deny this.

Edit: oh yeah, I really wondered if the Probe Height of -1 should have been -10? That would somewhat make the 3/8" or 10mm suggested starting height make sense, I guess.

You mean 'probe depth'? This value tells the probe how far below 0 to check. So, with -1, it will stop probing when Z reaches -1 before giving up trying to find the surface. -10 would probably be fine but if you forget to attach a wire to the probe or something, it would never find the surface and would continue to probe until Z is -10, which would probably destroy your work-piece, your bit and probably some of your table as well. -1 will probably not be so disastrous. However, having said that, if your work-piece is particuarly uneven, you may want to adjust the 'probe depth' to a bigger number (-2 or -5 for example).

Hi James, thanks for the reply.

Yes, I meant "depth" not "height" (even though technically a "depth" of -1 would imply above the surface, and a "height" of -1 below ). I have never seen Mach3 pop up a dialog, but nor have I tried it with the Z height well above the surface - I'll test that out and confirm that it does that when I'm next near the CNC.

So do you think that the approach I have used, which zeroes Z at ~8mm above true surface, is the way you intended this to work?

This piqued my interest in what the GCode looks like - here's a snippet from a sample board.

(begin initial probe and set Z to 0)
G0 X-2.3032 Y-2.3032 Z0
G31 Z-10 F100
G92 Z0
G0 Z2
G31 Z-1 F50
G92 Z0
G0 Z2
G0 X-2.3032 Y-2.3032
G31 Z-1 F100
#500=#2002
G0 Z2

So what this looks to me like is that it always assumes a Z height of the first probe to be 10mm or less, which matches your guidance of 3/8" or less. It does a probe for that -10mm with speed as set in the parameter supplied in the interface, then resets the Z to 0; then probe returns to Z=2, probes at half speed with a limit of z=-1 (which should never come into play, we haven't moved the probe's location), and resets Z again. Then finally it moves to the same XY cords (not sure why - probably this is a function of generating GCode in a loop) and probes at full speed and stores the offset in #501.

So I think everything will be fine in the way I've documented this - get to within 10mm and zero Z, then start the probe code execution. -1 for "depth" will be fine too since we're talking about 1.6mm PCB material that should never be that far out

OK, now I have learnt my one thing for the day I can sleep easy (later - it's morning here )

Thats pretty much exactly right and yes, your approach looks exactly the way I intended

It probes the first point twice, once fast and once slow to ensure Z0 is correctly set. Since all other points are offset to this first point it is arguably the most important point.

Yes, it probes the initial point a 3rd time because, as you say, its part of the (probing / offset) loop in the code.

technically a "depth" of -1 would imply above the surface, and a "height" of -1 below

technically, yes

Thanks again James for the reply - and a big thanks again for the software.

I wonder if the value of doing the 2nd probe is at all realized when the third probe is the one that is recorded and used in offset calcs, and perhaps it'd be better to store the zero value obtained by that 2nd probe and ignore the (0,0) index point? Certainly less "clean" but if the final read gave anything other than 0 I'd expect there's potentially a machine variability that needs looking at

The 2nd probe is indeed half the feedrate of the 1st and is therefore a bit more accurate than the first. However, the difference between a feedrate of 100 and 50 for the probe is fairly neglegable and really not worth me making any changes to this part of the code (I like 'clean' code ).

Actually, the difference between the Z0 index point and the offset is never 0, at least on my machine, but always very close, certainly nothing to be concerned about.