G92 support

[Bertho]

I bought CutViewer and I have been happily using it but I have been pulling my hair out trying to test some code yesterday.

It appears that it will accept a G92 command (For example G92 X0 Y0) but it will not restore the offsets with a G92.1. Is that correct or am I doing something wrong?
How about G52? I have not tried it.
Best Regards

[Randy]

Bertho, welcome to the forum (are you the same Bertho from the Mach forum?)

It looks like CutViewer doesn't implement G92.1.

I wrote a little test program:

(Filename: g92test.nc)
G20 (Units: Inches)
G17 G40 G80 G90
(STOCK/BLOCK,4.0,4.0,0.5,0.0,0.0,0.5)
(TOOL/MILL,0.25,0,0.5,0)
G00 X0.5000 Y0.5000 Z0.1000
G01 Z-0.1000 F12
G01 X1.5000
G01 Y1.5000
G01 x0.5000
G01 Y0.5000
G00 z0.1000
G92 Y-1.500
G00 X0.5000 Y0.5000 Z0.1000
G01 Z-0.1000 F12
G01 X1.5000
G01 Y1.5000
G01 x0.5000
G01 Y0.5000
G00 Z0.1000
G92.1
G00 X2.5000 Y0.5000 Z0.1000
G01 Z-0.1000 F12
G01 X3.5000
G01 Y1.5000
G01 x2.5000
G01 Y0.5000
M30

and ran it through CutViewer:

g92test_cutviewer.gif (4.64 KiB) Viewed 1184 times

and then loaded it into Mach3:

g92test_mach3.gif (4.66 KiB) Viewed 1184 times

Mach3 processes the G92.1 but CutViewer doesn't.

I've never used G52, but with a little playing found that CutViewer doesn't process it at all.

It looks like, for CutViewer to correctly show your gcode intent, you'll need to (in the above example) replace the

G92.1

with

G92 Y2.5000

i.e. explicitly change the coordinate that was changed originally (I made a -2.000 change in the Y coordinate with the first G92 so I need to make a +2.000 change with the second G92).

Randy

[Bertho]

Hi Randy,
Yes, that is me on the Mach forum.
It is disappointing that CutViewer is not processing the G92.1 properly. It accepts the G92 X0 Y0 and properly sets them to zero but it does not restore them afterward. The G92 makes really nice subroutines for "randomly" placed patterns:
----------------
S12000 M03 M08
G00 X-6.400 Y-11.085
M98 P1001
G00 X-12.800
M98 P1001
G00 X-9.600 Y-5.543
M98 P1001
G00 X-3.200
M98 P1001
G00 X0.000 Y-11.085
--------------------------
G00 Z60.0
M5 M9
M30


O1001 (Sub: ===== Hex Recess====)
G92 X0 Y0 (set current location to 0/0)
G00 Z1
X0.000 Y1.353
G01 Z-0.850 F60
X1.172 Y0.677 F120
Y-0.677
X-0.000 Y-1.353
X-1.172 Y-0.677
Y0.677
X0.000 Y1.353
Z-1.700 F60
X1.172 Y0.677 F120
Y-0.677
X-0.000 Y-1.353
X-1.172 Y-0.677
Y0.677
X0.000 Y1.353
G00 X0 Y0 Z2
G92.1 (restore the old X & Y)
M99
%

What are the possibilities to fixing/adding the proper G92 processing?
Thanks,
Bertho

[Randy]

That is a neat application for G92, Bertho. The only time I've used G92 is in a program I did for my Tormach mill, which has a clamp-on mount for a Proxxon high-speed hand tool as a secondary spindle. I machined a control panel with the main spindle for the cutouts, then used G92 to offset the origin to the Proxxon and do the text engraving.

You could write to Stan (CutViewer's developer) at support [at] cutviewer [dot] com and request G92.1 implementation. I wrote to him near the beginning of last month to ask about corner-rounding endmill support, but haven't received an answer yet.

Randy

[Bertho]

Great News:

Stan emailed me an updated version of CutViewer and it now works great with the G92 G92.1
Thank you very much Stan!!

That is fantastic service: An update in 6 hours after the request!
A very happy Bertho

[Randy]

Great, Bertho. Confirmed it here too. That is a great response time!

Randy