G2 - G3 Command Bug with G68

[jmchris]

All,
I seem to have sumbled on a bug that has some very odd behavior.  While the following code is exactly the same line for line two different circles are created.  My IJ is set to incremental.  I'm attempting to cut a spiral hole so I don't burn up my endmill drilling straight down in .25 stainless.  I need the G68 as I'm milling a single part and will be reversing it for every other part cut so as to use my stainless in the most efficient manner possible.  I've removed all other part G-code to ensure it wasn't causing an issue.  The two pieces that appear to conflict are the G68 and G2/G3.

First my original code that revealed the issue.  You'll notice that the only difference between line 4 and 5 is deeper Z.  But instead a different and much larger hole is created:
G68 A0 B2 R180
G0 x0 y0 z0
G1 X.280 Y.432 F.6
G2 x.280 y.432 Z-.15 i.036
G2 x.280 y.432 Z-.25 i.036
G2 x.280 y.432 Z-.35 i.036
G40
M30

Second a block of IDENTICAL lines of code that create two different size holes.  Each identical line of G2 code creates an alternating different size hole.
G68 A0 B2 R180
G0 x0 y0 z0
G1 X.280 Y.432 F.6
G2 x.280 y.432 Z-.15 i.036
G2 x.280 y.432 Z-.15 i.036
G2 x.280 y.432 Z-.15 i.036
G2 x.280 y.432 Z-.15 i.036
G40
M30

Any assistance would be greatly appreciated.
Thank you,
Jeff

[BR549]

I can confirm that .  Cuts a large circle then does a small circle at the start point then another correct circle and another small circle.

(;-) TP

[BR549]

Instead of full circle arcs try it with half circle arcs

(;-) TP

[BR549]

OK testing shows this work fine. So lets take apart your code and see where it fails.

G90 G80 G54 G69 G0
G68 A0 B2 R180
G0 x0 y0 z1
G1 Z0
G2 x0 y0 Z-1 I.5 J0
G2 x0 y0 Z-2 I.5 J0
G2 x0 y0 Z-3 I.5J0
G2 x0 y0 Z-4 I.5 J0
G0 X0 Y0 Z0
G40
G69
M30
%

[BR549]

OK add on the J 0.000   Mach is trying to justify the absence of the reference point when rotated.

Mach does NOT need the reference without it being rotated that is why it cuts ok when NOT rotated.

BUG ?  Quirk ??  More quirk than bug.

(;-) TP

[jmchris]

Sooo.  How do I G68 rotate my part?

Jeff

[jmchris]

BR549 - Firstly, thanks for the help.  I had hoped someone from Mach3 would be on the form to look into the bug.

The code you pasted in doesn't work properly.  Instead of alternating a correct and incorrect circle, now it only makes incorrect circles.  You can add a line G1 X1 Y1 to create a one inch reference point for the proper size of the circle.  In your example the radius should be .5 inches, but when adding the reference point of 1 inch you can see the circle is really over two inches instead of 1/2.

Jeff

[BR549]

YOU are correct, I was testing the geometry of the circle and did not verify the diameter.

BUT I know for sure that the Radius method works correctly. Try this, the diameters are correct here(;-)

Also you may want to give the IJs a try using  arcs instead of the circle method.

I don't think you will have much luck on getting the G68  fixed so I was looking for a workaround


G90 G80 G54 G69 G0
G68 A0 Y1 R180
G0 x0 y0 z1 F100
G1 x0 Y-.5 Z0
G2 x0 y.5 Z-.1 R.5
G2 x0 Y-.5 Z-.2 R.5
G2 x0 y.5 Z-.3 R.5
G2 x0 y-.5 Z-.4 R.5
G0  Z0
G40
G69
M30
%

[BR549]

OK testing shows that radius arc method AND absolute IJK mode works BUT inc IJK method is broken with a G68 command. I think I see the problem BUT Brian will have to fix it.

(;-) TP