Aircuts on Mach3 USB NcUsbPod

[steamer]

Hello,

I'm currently having problems with aircuts (Z 280mm) with AutolevellerAE v0.8.4 where Autoleveller 0.7.7 works without a problem with the same setup.

I've generated a probe set:

-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
-549.96875,-337.49063,180.48438
....

Am I doing something wrong?

Greetings,
Emile

[Country_Bubba]

Emile,
I don't use Mach, so this is just a guess.
By any chance do you have an offset for your tool??? I have seen where others have had an unknown offset for a tool and it will show the same problem.
Again, just a guess

Art
Country Bubba
Moderator

[steamer]

Hello,

My mach3 controller seems to ignore the Z-1 part of the G31 Z-1 F100 probe command, it stops when it reaches Z0 and goes to the next point, only when the level is positive, it triggers the probe correctly.

Strange because I use the probe a lot with tool changes and there it functions correctly.

I wonder if it has something to do with the G92 Z0 command.

Greetings,
Emile

[steamer]

I've made some progress and cut my first pcb with AutolevellerAE.

Changes in the AL output file:

Replace both of the G92 Z0 entries with G52 Z0, with G92 the controller won't move the Z lower than Z0.

After each G31 command add call to macro routine M2002. (Got that idea from gskular on cnczone.com, the controller won't put the correct values into 2002 on it's own)

Add a macro routine containing "SetVar(2002,getoemdro(802))" to the active macro directory of mach3 and call it M2002.m1s
This gets the correct value from the controller and stores it in 2002.

Would be nice if a setting could be added for Mach3 controllers that use the NcUsbPod.dll driver. (XHC MACH3 IV USB and several clones of it)

Greetings,

Emile

G90 G21 S20000 G17

M0 (Attach probe wires and clips that need attaching)
(Initialize probe routine)
G0 Z25 (Move clear of the board first)
G1 X-0.28 Y-0.28 F1000 (Move to bottom left corner)
G0 Z2 (Quick move to probe clearance height)
G31 Z-1 F100
M2002
G52 Z0 (Touch off Z to 0 once contact is made)
G0 Z2 (Move Z to above the contact point)
G31 Z-1 F50 (Repeat at a more accurate slower rate)
M2002
G52 Z0
G0 Z2

G0 Z2
G1 X-0.28 Y-0.28 F1000
G31 Z-1 F100
M2002
#500=#2002
G0 Z2
G1 X9.81333 Y-0.28 F1000
G31 Z-1 F100
M2002
#501=#2002
G0 Z2
G1 X19.90666 Y-0.28 F1000
G31 Z-1 F100
M2002
....

[daedelus]

Hey, Great work finding a workaround for this issue, very helpful post, thanks. I only have a parallel port on my CNC PC so I would never have found the problem without a USB interface myself.

I am currently working on having a custom controller option in AE, Where you should be able to add commands like G52 in place of G92 and M2002, this will help you and others I think. Should be with you in the next update, cant give a date on that yet though

Edit: The custom controller options have been added now. Since v0.8.5 of AE

[steamer]

That would be a great addition, I'm looking forward for it!

Greetings,
Emile

[stephan]

Just wanted to add a little bit of info to this thread, given that my issues with aircuts and probing on a USB cnc mill (6040z) on Mach3 led me here.

What I've noticed is that "G31 Z-1 F100" sometimes ignores the probe contact and crashes into my PCB . To resolve this issue I just had to increase the probing depth, i.e. "G31 Z-5 F100". Once I made this change the over-probing and crashing was resolved. It appears that the USB controllers for these chinese cnc machines act weird if the G31 command limit (i.e. Z-1) is not far enough beyond the workpiece/PCB/Probe. Whether the #2002 variable was saved properly is not something I checked for.

Another note to add, start the variable count at #601, as #601-#999 are reserved for user variables in Mach3.

Also, make sure you have high quality bits. This will also help resolve aircutting issues, as the cheaper V-shaped engraving bits (from eBay or Amazon) tend to bend or break during the milling process. A small ball or square end mill produces much more reliable results. I personally use Melin Ball End mills, at sizes 0.016" and 0.009".

Hope this helps someone else out there with a similar issue.

[Renato]

Hi,

I´m having the same issue, but for me the solutions above didn't worked. (Sorry for my poor English)
I made some tests here.
1 - When I type the command G31 Z-1 F100 in the MDI field the machine works.
2 -When the machine is moving along the path, if the probe contact is closed (digitize LED on), the machine stops at the next probe position. If I open the probe contact the machine execute the G31 command correctly, and while the Z axis is going down, if I close the probe contact again the machine recognize like if the PCB surface was hit and move back and goes to the next probe point.

I don't know how to program but I believe that this information can help you guys to find one solution for this problem.

I'm using a chinese USB board and Mach3.

[Renato]

Hi James,

As I said I'm bring our conversaton to here.

As you told me The solution was to create a line before de command G31 Z-1 F100

Like this:

G4 P1 (alts the gcode for 1 second)
G31 Z-1 F100

This way the zero axis worked fine. The Mach 3 (or the USB controller) does not accept floating numbers. So the times has to be 1, 2, 3... seconds.

As I told you on the e-mail, the problem is I did not find an easy way for to fill the Gcode with the command G4 P1. Would be nice if the next version come with this improvement.

Thank you.

Renato Ferreira

[daedelus]

I was not 100% sure that pausing with G4 would work but it seems to work for some and i'm glad it works for you. Yes, it would be nice if you could add a smaller delay that 1 sec but I guess thats part of the GCode specification or Mach3 / USB controller as you say. Cant be helped.

As for adding the G4 command for each line. Does this not help?
Change controller to custom as shown here:

Now change the custom controller options in the options menu to something like this:

This should be the same settings as for Mach3 but with the added "G4 P1" probe command.