[lew90nicis]

Hi folks,

Does anyone know where I can find a hole centre finding macro? I've scoured Google but haven't managed to come across any yet.

I'm no g code wizzard so unable to create my own.

Any help would be great.

John.

[tinmancarving]

Hi John, I don't know anything about Linux based systems but I did run across this web page while looking at probing systems for my machine. The code on this page if for finding a corner but if you decipher the macros you can modify it to perform probing of a bore.

7xCNC - Minilathe CNC :: Probe Corner (NGCGUI)

I'm sure someone will come along with just what you need.

Much Luck,
Rob

[NitroCH3NO2]

John,

There has been a post on the LinuxCNC forums about just such a program that is an add in for the GUIs.

Here is a link to the post.

LinuxCNC :: Topic: Work with probe (1/2)

It has all types of probing macros built into the program. I have not used it yet but I plan to when I get my machine converted to LinuxCNC in the near future.

[askjerry]

Have you found your solution? If not... I have a few that I have been using... and I've learned to write a few. Once you understand the concept it isn't too bad.

Are you running AXIS 2.6 or better? After 2.5 they made it so it can share variables between the pyVCP panel ad G-Code... and that opened up a lot of doors!

This is one I use... I call it from a button in my pyVCP panel.

O  sub
(Idea Stolen from Pete Mills http://petemills.blogspot.com/2014/04/diy-pick-and-place-machine-part-2.html )
G20 F10
(MSG, Probing..stand by...)
#1000=2 ;max radius
#1015=0.066 ;Probe Tip DIA in inches

G91 G38.3 Z.00001
#1001=#5061
#1002=#5062

G91 G38.2 X#1000
#1003=#5061
G90 G0 X#1001
G91 G38.2 X[0-#1000]
#1004=#5061
#1001=[[#1003+#1004]/2]
G90 G0 X#1001

G91 G38.2 Y#1000
#1005=#5062
G90 G0 Y#1002
G91 G38.2 Y[0-#1000]
#1006=#5062
#1002=[[#1005+#1006]/2]
G90 G0 Y#1002


G91 G38.2 X#1000
#1003=#5061
G90 G0 X#1001
G91 G38.2 X[0-#1000]
#1004=#5061
#1001=[[#1003+#1004]/2]
G90 G0 X#1001

G91 G38.2 Y#1000
#1005=#5062
G90 G0 Y#1002
G91 G38.2 Y[0-#1000]
#1006=#5062
#1002=[[#1005+#1006]/2]
G90 G0 Y#1002

(MSG, SLOW PROBING...)
F0.1

G90 G0 X[#1003-0.02]
G91 G38.2 X0.025
#1003=#5061
G90 G0 X[#1004+0.02]
G91 G38.2 X-0.025
#1004=#5061
#1001=[[#1003+#1004]/2]
G90 G0 X#1001

G90 G0 Y[#1005-0.02]
G91 G38.2 Y0.025
#1005=#5062
G90 G0 Y[#1006+0.02]
G91 G38.2 Y-0.025
#1006=#5062
#1002=[[#1005+#1006]/2]
G90 G0 Y#1002

#1007=[#1003-#1004+[#1015]]
#1008=[#1005-#1006+[#1015]]
#1009=[[#1007+#1008]/2]
#1010=[atan[#1002]/[#1001]]
#1011=[sqrt[[#1001*#1001]+[#1002*#1002]]]

(Xdia #1007 Ydia #1008 Dia #1009 Ang #1010 Dist #1011)

G17    (Machine to XY Plane)
G20    (Inch Mode)
G40    (Cutter Compensation OFF)
G90    (Absolute Movement Mode)
G94    (Speed in Inches per minute)
G54    (Use Coordinate system P1 G54 Default)
G49    (Cancel any tool length compensation)
G91.1  (Arcs set to default units and method)
M5     (Stop Spindle)
M9     (Stop Coolant)
M48    (Allow Speed Override)

G10 L20 P1 X0 Y0 (Set current location to ZERO X and Y only.)
(DEBUG, PROBE DONE. DIA X:#1007. DIA-Y:#1008)
O  endsub
M2

I hope that helps.
Jerry