Strange preview for circular arc (G2/G3)

Hello,

I was planning to bore out a disc yesterday and thought I'd handwrite the code. The circular path would be 105 mm in diameter with the center at G54 X0, Y0, and starting at position X-52.5 Y0. Because of my lack of experience, I wrote is as a small program so I could get a preview. But the preview is not what I expected for the:The arc is started from position X-52.5, Y0.

As you can see in the screenshot, the preview shows a strange linear movement and a counter clockwise helix. But when I run the code, the machine makes a 105 mm circle in the XY plane, just as I wanted. The path from this run is visible as well (the red line). I'm guessing I'm doing something wrong, but what?
 

The complete code was visible in the screenshot, but for clarity I include it here:
I made a new test with the code you used, and for that the preview is working properly. But if I comment out the G0 move, then the preview is again strange. See the two situations below.
 
 

The complete code, with G0 commented out is below:
Maybe this is expected behavior? It certainly wasn't what I expected, but that doesn't mean much. I use LinuxCNC 2.9.2 by the way.

Thank you for having a look. With that the issue is now pinpointed.

Just in case you want helix milling, you need to set z value for start and end. P is the amount of turns, if z-10 P5, it could look like that, pitch 2


 


 

Yes, helix milling was the end goal. But I was trying to build the program as simple as possible to start with, because I have little experience with anything else than G0/G1. But I got stuck because the preview did not show what I expected for an in-plane (XY) circle.

Thank you for the explanation and test you provided!

This toolpath is at centerpoint, so don't forget cuttercompensation. If G41/ / G42 makes trouble, whats not unusual, it can be solved like that. Parameter #5410 is tooldiameter of loaded tool. 
 

Maybe the result depends on the starting position, or some other unknown factor(?)

As such, this is okay for me. I was thinking that maybe a have some strange more or similar enabled. But it appears the preview may require a linear move before arcs.

So maybe a bug in the preview code...

I just quickly tested it. That's a bug in gmoccapy. In axis, it works.

In axis, you have to reload the gcode after each other move, so the initial position of the circle is updated.

G2's I and J parameters are relative to the last position:
linuxcnc.org/docs/html/gcode/g-code.html#gcode:g2-g3

Now if you don't have a G0 or G1 command before, the preview in gmoccapy looks funny. I think the preview interpreter is not initialized with the actual position in the UI. The real machine interpreter has no issues afterwards.

For the first command, X,Y and Z has to be specified to work. G0 X0 Y0 is not enough, G0 X0 Y0 Z0 does the trick.

I suggest writing a bug report.

BTW: Not having a absolute move before a relative move is probably not anything a CAM software would ever do, but it's also not illegal.
However, a "normal" preview tool not knowing where you machine is could not show you anything in that case.