[turbocad6]

hey guys, first post here, I've been lurking and learning for a long while now. I'm def an admitted noob with cnc but I'm a big believer in searching for answers and reading, studying and learning instead of just asking questions, but this problem had got me stumped and I've been searching for hours but not finding anything like my problem so I figured I'd just ask

I'm working with a romaxx router and what I'm having a problem with is a simple little gcode that I wrote to profile 2 corners of a small wood panel. now where this problem gets strange is, I wrote the code and cut a few parts and it was working absolutely fine. the radius of my curve was good and it matched well to the part I need this to fit into, everything was good. then, all of a sudden, with nothing else changed (as far as I know), mach3 started to, instead of making a rounded corner, it just started to cut the corner at almost a 45 deg. angle. I'm running this real slow, at like 20ipm and again, it was working fine just a few minutes before.

I reloaded mach3 and even restarted the pc but nothing helps. what's even more strange is, it even shows this weird 45 deg. cut off corner in the tool path preview instead of showing the arc that the gcode should be??? this has me completely baffled because just minutes ago it was cutting this same arc just fine


here is the gcode for this part:

%
(main door)
g00 g20 g17 g90 g40 g49 g80 g61
x3y-0.95
m03 s15000
m08
g01 f20
z-2.45
x-0.65
g02 x -1.05 y -0.55 I0 J 0.4
g01 y 0.485
g02 x -0.65 y 0.885 I 0.4 J 0
g01 x3
z0
m30
%

here is what the curves should look like




but here is how it displays in mach3's tool path preview (don't know why it rotated sideways)




and here is the difference in the cut, I cut several like the one on the right and it was cutting perfect, and then all of a sudden it started cutting at an angle like shown on the left with the same exact block of gcode...






any help would be appreciated, thanks

[Jon.N.CNC]

That is wierd. Mach 3 supports radius's so you could use a pp that will use R instead of I,J.

Can't explain why your getting this issue tho. Has it switched from cv to exact stop mode?

[OlfCNC]

He is in exact stop mode already. G61 is in the beggining of his code.

[Jon.N.CNC]

He is in exact stop mode already. G61 is in the beggining of his code.

lol missed that, well there's his problem.

[ger21]

Looks like your IJ mode may have changed.

See if this code works:

%
(main door)
g00 g20 g17 g90 g40 g49 g80 g61
g91.1
x3y-0.95
m03 s15000
m08
g01 f20
z-2.45
x-0.65
g02 x -1.05 y -0.55 I0 J 0.4
g01 y 0.485
g02 x -0.65 y 0.885 I 0.4 J 0
g01 x3
z0
m30
%

[turbocad6]

thanks guys. I've been running exact stop mode because on some of the parts I'm making, fit-up to matching parts is critical so I wanted nice crisp precise corners, but I thought that even in exact stop mode, arcs would still be arcs, especially seeing as how it did initially work just fine even in exact stop mode, so I don't get how that in itself could be the problem.

Gerry thank you, I think you might have just hit the nail on the head although I have no idea what would have caused the IJK arc mode to change. I suspect that it may be in the code of a block generated by aspire that I may have run in-between the time it was working and the time it wasn't? so now I'm guessing that g90.1 and g91.1 are modal? yeah, guess I'm still learning something new every day this one only cost me 2 pieces of exotic wood, I guess it could have always been worse

anyway, I'll confirm this does work a bit later when I can get back to the router, but now even just in reading about the differences of g90.1 and g91.1 it certainly makes sense of something that made absolutely no sense to me before, so really thanks for that Gerry, I'll be sure to include a g91.1 in any new code I write with arcs in the future

stupid question but why would an aspire block of code even want to put the machine into a g90.1 mode(assuming it was indeed that)? I mean what is the reason or advantage to a g90.1 mode in the first place? and wouldn't it be good form, assuming that this is modal, to at least switch it back when finished excecuting the code?

[turbocad6]

well that was the problem, thanks again Gerry. I checked the code in the block I was running in-between when it was working and when it wasn't and it did not have a G90.1 in it, it actually had a G91.1 in the code so I still don't know what put the machine into G90.1 mode in the first place. I'm wondering if there might be a keyboard shortcut that activated it? I may have inadvertantly pressed a key or 2 on the keyboard vacuuming up chips, only thing I can think of...

[ger21]

Did you use any of the Mach3 wizards? Some of them use Absolute IJ mode.

[turbocad6]

nope, only thing I did was switch to resurface one panel at a different work co-ordanant then right back to these arcs. I did vacuum up some chips though, only thing I can think of is possibaly touching a key or 2 on the keyboard while doing that... def a mystery...

[ger21]

There are no shortcut keys to change IJ mode.
However, the default IJ mode is Absolute I think, unless you change it.
So unless you change it in General Config, any code with a G91.1 will run correctly, and any without it will not.

I mean what is the reason or advantage to a g90.1 mode in the first place? and wouldn't it be good form, assuming that this is modal, to at least switch it back when finished excecuting the code?

Just two different ways of writing code. I guess the advantage to absolute IJ mode is that it's a little easier to read. But, 99% of CAM programs use Incremental IJ.
You can't easily switch it back when finished, because the g-code doesn't know what mode you were in before it was loaded.