Non-conductive material levelling

[ansenseale]

Is there any way in the software to provide an additional offset for the use of a touch plate for non-conductive materials? I'm thinking of hanging a small touch plate below the bit and connected to the probe to travel with the bit as it does it's measuring.

[daedelus]

If you see the second video on my site, the surface of the case is non-conductive. This was not done by myself but the guy who did it, laid a this piece of tin foil on top (squirt the surface with water first to give some surface tension and brush the foil with a small paintbrush) for probing then removed it before milling started. You could also paint on some conductive paint.

This might be a better option for you?

[yioryos]

Hi all,

its my 1st post here and all the best to the AutoLeveller creator !!

I am getting ready 2 do my first autolevelling, and it will be on anodised aluminium. So, I made and tested a probe to do the probing.

When probing finishes, I replace the probe with the engraving bit and attach clip, position the ground plate (x,y of 1st point, #500 var).

Press cycle start and my g-code file prompts for tool change

Then, I do AutoToolZero after having found a script for this button in Mach3 and updated it regarding plate thickness and feed. (See attached file).

After, the AutoToolZero execution, I press cycle start and the AL-ed program does its magic.

Haven't tested it yet but I will let you know the following days..

I have read the "Practical question during use" post and have not understand this=


"If you mean "adjusted the Z" means you moved the head or tool up or down, then yes, you will have to re-probe"

So, if somebody jogs the mill in z or even in xy prior to hitting "cycle start" the probing must be repeated? If I understand correct, then my too optimist approach described above, cannot be implemented...

Well, why? I haven't clarified it yet.. The assigned variables of the probed z trip points are reset if the mill is jogged prior to g-code execution?

I 'd be grateful for your feedback... All the best

[yioryos]

Well, just an update:

I tested the AL with my probe and AutoToolZero and the #500 did not change.(Used the GCode Var Monitor at operator menu of mach3). Though, Mach3 halted (no-estop, just no x-y-z movements but the spindle fully on, at the highlighted line:

(The original mill file is now rewritten with z depth replaced with a)
(bilinear interpolated value based on the initial probing)

%
O1
G80 G40 G17
G0 Z30. M9
T3 M6
(TOOL 3)
(OPERATION 1)
M3 S18000
G0 G90 G54 X-30.4961 Y13. A0 M3 S18000
M8
G0 Z0.5
#102=#685
#101=[#686+0*#685-0*#686]
#100=[#102+0.13361*#101-0.13361*#102]
G1 Z[#100 + -0.1] F250
.......code continues here


The previous part of the program was just assigning variables and this is why I am guessing it did not affect my system, but the G1 command has a variable USAGE in gcode execution and it is the first it encounters!!

Mach 3 stopped without e-stop and no x,y,z movement! just the spindle remained ON at 18000 rpm at 0.1mm below z0.

I think this must be a problem related to my SmoothStepper and I wrote them an email. Will c their reply......

Also, during probing, there is a delay between z-trip and beginning of G31. I think, the smoothstepper seems to be again the cause.....

[daedelus]

Hi, and welcome to the forums

For the line you highlighted from another post, I think we were mainly we were referring to LinuxCNC and turboCNC when we said that as probed values do not seem to be persisted in those software tools.

You may well have more luck with Mach 3 as I believe the variables between #500 and #1000 are indeed persisted there.

I do not use Mach 3 myself so it is great to know the Autoleveller for Mach 3 is working as expected.

Good luck with the smoothstepper.

[yioryos]

Hi Daedalus !

Well, I have to say I have good news. I found out the cause for having the Mach halting. My G-Code post processor issues dots in places they shouldn't be and after "cleaning" the file from these dot-bugs, nothing halted. No relation with the smooth stepper.

I did engravings both in plastic and anodised aluminium and used both methods: 1) 0.02mm thick aluminium foil adhered through water induced surface tension and with the probe.

With the foil:

As you described

With the probe:

After probing the surface with the probe, I changed it with the engraving bit and used the autotoolzero. Just keep in mind though, that the plate's area may obstruct registering the actual trip point the tool would have have, acting as a "peaks integrator". Thus, it could be a good idea to use a small piece of foil instead of the plate and to update its thickness to the autotoolzero script. But, then again we come with the original foil method, proving it is very good, simple and reliable, as long as you ensure adherence throughout probing which was easily done in my try with the aluminium panel. The probe could be an alternative in cases this adherence cannot be easily or satisfactorily be achieved. Of course, it is meant that your probe should have a repeatability much lower than the minimum variations you 're autolevelling.

Another important note is to properly adjust probe spacing according to your warp estimation. I had 2 bolts holding the aluminium fixed and I adjusted probe spacing to avoid them during probing. Well, this was a bad criterion for probe spacing adjustment since, these 2 bolts were bending locally the aluminium at the space between two probe points. So, if you design a line between these 2 points you loose the extra depth of the bend! In other words, you do not say AL to measure this variation and you end up without autolevelling.

Finally, if the probe depth is 0.01" higher that the programed trip point in G31, Mach3 will halt after the trip. That gave me a headache for 2 hours until I re-assembled the gcode through AL with an increased depth and no halts.

Again thanks Daidale for this s/w!!!

yioryos