Autoleveller

Hi,

I'm a first time user of AutoLeveller software. Using the software modified gcode, the cuts are way too deep (~.5-.9mm). I have dug as deep as I could into the problem, but I'm stuck as to why this is happening.

Looking over the linuxcnc documents, i found and used (PROBEOPEN probelog.txt) along with (LOGOPEN, log.txt) & (LOG) commands to dump out what is going on in the probing section of the gcode. What i found is that all the probed value z is positive (.2 to .3 range), while the saved #50X values are negative (-.5 to -1mm). If I stop the program after the initial z setting @ 0,0 and give g0 z0 command, I get an warning that the probe has tripped on non probe command, so I think the values in the probelog.txt is correct.

It seems to me, the problem is the cnc machine is stopping way past the probe contact on the G38.2 command instead of at the probe contact. I see little holes where the probe points dig in, so I have tried to reduced the max velocity and acceleration, and now the machine stops at the -1mm (setting I used for max z depth). All the #50x values are -1! (It made the problem worse.)

Any idea what I can do? Any settings in linuxCNC that I can try to get the machine to stop at probe contact? Is there too much delay on one of the settings? Do i have some persistent g code that is active, that shouldn't be?

One workaround I'm thinking of trying next is to try to save the probe z value(#5063) instead of the current z values(#5223). If this works, I guess I can do a global search and replace on the gcode.... I'll have to live with the holes left by the probing since I do a indent on the pcb on the spots that was probed...

Any help / ideas would be appreciated.

Thanks,

Rob

My setup:
Linuxcnc 2.6.7 on Ubuntu 10.04.4 with AutoLeverller .77, JRE 1.8.
Metric (mm) units, 30degree .1mm vbit, zentoolworks 7x7 cnc with f8 on x,y and standard(f1.25) on z axis.
TB6560 based parallel port to 3 axis controller.

Checked to make sure i'm not missing Z steps, and i have turned way down the max acceleration and max velocity for that axis way down in the .ini file. I'm using 200step/rev stepper, full step, 1.25mm/rev so my step settings are 160 steps/mm.

Oops, typo: #5223 should be #5422

I hand edited the gcode file so that it does a G0 Z#5063 before setting the Z0:

G38.2 Z-1 F100
G0 Z#5063
G10 L20 P1 Z0

G38.2 Z-1 F50
G0 Z#5063
G10 L20 P1 Z0

I did a search and replace for all #5422 to #5063 for the rest of the files.

This sets the Z0 and all probe point saves to be the probe contact value instead of what the machine stops at. I got my first clean PCB isolation mill using my small test layout!

AutoLeveller software worked great!

I now have a workaround, but I'm still interested in hearing back from anyone who may have ideas on how I can fix LinuxCNC setup and/ or hardware issue.

Thanks and regards,

Rob

Hi Rob,

looks like you have done some good and extensive testing yourself. This is interesting because you should not, and I have never needed to add any extra #5063's to the gcode and I too would be interested if anyone else has this problem and if Robs workaround worked for you?

The membership version uses improved algorithms for leveling and should improve accuracy if needed. Plus it has a lot of other improvements. The probe log open and close lines are also built in to the membership version which should help for diagnosing any issues.

This latest version is open-source and can be downloaded and compiled from my bitbucket repository, or you can become a member and get hold of the pre-compiled .exe or .jar. I am also working on the new AL8 which members will be the first to get their hands on.

Hi

I'm new to AutoLeveller too. i an having a similar problem with AutoLeveller and Mach3.

My Setup:
CNC 6040z (a well made one)
Lisenced Mach3 R3.043.066
AutoLeveler 0.7.7
Bit: 60 deg v-bit

The probing seams to probe fine with no marking on the surface of the PCB.
In my cam I set depth of cut to 0.035mm which is the thickness of my copper layer. The actual cut is a lot deeper then just the copper layer so i tried in the cam changing the depth of cut to 0mm (just touching the surface) it cuts 0.45..mm deep.
I am still learning how to CNC mill, if anyone have any ideas I would be very grateful.

I've attached the 0mm deep g code and generated AutoLeveller g code if someone wants to have a look at it.
During probing it dose the following:

G0 X0 Y0 Z0
G31 Z-10 F100
G92 Z0
G0 Z3
G31 Z-1 F50
G92 Z0
G0 Z3
G0 X0 Y0
G31 Z-1 F100
#500=#2002
G0 Z3
G0 X3.03258 Y0
G31 Z-1 F100
#501=#2002
G0 Z3
and so on....

One thing to check is whether or not your pcb is solid to the spoilboard or if there is any flexure if you place your thumb on the board.
I found in some original testing with crumpled aluminum foil that probing would not deform the foil. However if your have any flex to your pcb, it will cut to deep. This "could be" a be a fixture problem an not software.

My .02