Well I kept cutting my code down from 1300 lines to what I have shown here.  There is a problem somewhere (maybe a bug within Mach3?).  When I load this, my toolpath shown in the window shows two large sweeping arcs for parts 3 & 4.  Anything after the use of a G52 (I also tried it using fixture offsets G55, G56 etc.) causes it.  What am I doing wrong?

G0 G49 G40.1 G17
G80 G50 G90 G98 
G20 (Inch)

(***** Remove material before cutting threads part 1 *****)
(***** Reset Z zero at this time *****)
M6 T1
M03 S4000
M9
G00G43 H1 Z0.1
G00 X1.125 Y0
G41 P0.25
G01 X0.432 F15
G02 X-0.432 Y0 R0.432 Z-0.025 F24
X0.432 Y0 R0.432 Z-0.05
X-0.432 Y0 R0.432
X0.432 Y0 R0.432
G00 Z0.1
G40

(***** Remove material before cutting threads part 2*****)
G00 Z0.1
G00 X4.125 Y0
G41 P0.25
G01 X3.432 F15
G02 X2.568 Y0 R0.432 Z-0.025 F24
X3.432 Y0 R0.432 Z-0.05
X2.568 Y0 R0.432
X3.432 Y0 R0.432
G00 Z0.1
G40

G52 X3

(***** Remove material before cutting threads part 3 *****)

G00G43 H1 Z0.1
G00 X6.125 Y0
G41 P0.25
G01 X5.432 F15
G02 X4.568 Y0 R0.432 Z-0.025 F24
X5.432 Y0 R0.432 Z-0.05
X4.568 Y0 R0.432
X5.432 Y0 R0.432
G00 Z0.1
G40

(***** Remove material before cutting threads part 4 *****)
G00 Z0.1
G00 X9.125 Y0
G41 P0.25
G01 X8.432 F15
G02 X7.568 Y0 R0.432 Z-0.025 F24
X8.432 Y0 R0.432 Z-0.05
X7.568 Y0 R0.432
X8.432 Y0 R0.432
G00 Z0.1
G40
G52 X0

M5 M9
M30

Radioactive, I don't know anything about this specific fixture offset problem, but there are unfortunately other problems with fixture offsets in Mach3.

If you do a feed hold and then start in G code with fixture offsets you're asking for a big crash (and this got me pretty bad), Mach will often apply the wrong fixture offset when the Start is hit.

A workaround for this problem is to put a dwell operation right before the fixture change, ie:

G4 P1 (Fixes Mach3 Feedhold problem)
G59 P#101 (Change to Specified fixture offset)

I don't know if this workaround will help with your problem, but its worth a try, let us know if it helps.

I really hope this gets fixed in the new release, as far as I'm concerned this is "Class A" critical bug that shouldn't be present in a Mach release version, a machine or a finger can really get hurt with problems like this.

Paul T.

Hi Radioactive (and all others),

concerning the G52 (temporary offset) I got the recommendation to wait for Mach3 Rev. 4.   


My experience with G52 was as follows:

- Using G52 just with linear and circular interpolation looks weird on the toolpath display, but works correctly on the machine.
- Using G52 together with G41/G42 (cutter radius compensation) leads to crash. There seems to be an error in code.

--> So, I decided that using the G52 temporary offset is not an option for me until release of rev. 4.

But, if you are just cutting the entirely same part two times, you could check wether using G54...59 (work / fixture offset) could be an alternative for you .?.



have fun
Konrad

Well, at least I can stop pulling my hair out trying to figure out what I was doing wrong.  It seemed to me Mach3 was having trouble with it, but I wanted to make sure it wasn't my error.

Sounds like to be on the safe side I shouldn't use G52 at all until Rev. 4 comes out (when is it supposed to be released?)

I'll just rewrite the code to use fixture offsets (G54...59) for everything.  The same problems don't exist within Mach3 using those does it?  I will have code using G41/G42 within it.

Thanks for the help guys.