[corpse]

I'm learning how to use some stuff in OneCNC 2000 pro, and some simple pocketing is causing me great grief. I'm drawing a circle in a circle, 2" dia and .5" dia, both centered at x2y2.

I create the pocket, plunge only with climb milling, .375" end mill, 0 offsets (as my My T Mill cnc software for my sherline mill doesnt support it)...
rapid Z plane .15, plunge clearance .11 (still not sure what this is for anyways), material z = 0, final z depth = .5". roughing not enabled, .2 step over 0" leave for finish.

When it creates the code, it seems to create some pretty crazy stuff.. the toolpath appears to be ok in onecnc, but the code is not jiving in the tiniest bit with my My T Mill s/w, when I read the code as normal is seems to be creating a crummy toolpath.. Below is the code is creates..

N10 X1.3125 Y2. Z0.15 
N20 Z0.11 
N30 G01 Z-0.5 F6
N40 G02 X2.6875 Y2. I0.6875 J0. F12
N50 G01 X2.8875 
N60 X3.0875 
N70 G02 X0.9125 Y2. I-1.0875 J0. 
N80 X3.0875 Y2. I1.0875 J0. 
N90 G01 X2.8875 
N100 G02 X1.1125 Y2. I-0.8875 J0. 
N110 X2.8875 Y2. I0.8875 J0. 
N120 G01 X2.6875 
N130 G02 X1.3125 Y2. I-0.6875 J0. 
N140 G01 Z0.11 F6
N150 G00 Z0.15 
N160 X3.8125 
N170 Z0.11 
N180 G01 Z-0.5 
N190 X3.6125 F12
N200 X3.4125 
N210 G03 X0.5875 Y2. I-1.4125 J0. 
N220 X3.4125 Y2. I1.4125 J0. 
N230 G01 X3.6125 
N240 G03 X0.3875 Y2. I-1.6125 J0. 
N250 X3.6125 Y2. I1.6125 J0. 
N260 G01 X3.8125 
N270 G03 X0.1875 Y2. I-1.8125 J0. 
N280 X3.8125 Y2. I1.8125 J0. 
N290 G01 Z0.11 F6
N300 G00 Z0.15

edit:
oh yeah, in my nc post output settings...
I'm using absolute coordinate with Incremental I J for G2/G3 circular, full circular movement. My MY T Mill software uses the Incremental I J codes, as per an example from them:

Example
G2 X-1.535 Y0.469 I0.500 J0.000
Description
Move in a clockwise arc from the current position to location (-1.535, 0.469) using a center point located 0.5 units in the X direction from the current position.

But the problem with the above OneCNC code (the first big code snippet), is that it doesn't seem to properly factor in the starting positioin when doing the circular motion, so its result is creating mostly half circles.

[HuFlungDung]

If you don't define your coordinate system in your gcode program, your control may not be interpreting it correctly. You should always tell the cnc whether you are working in G90 (absolute mode) or G91 incremental mode. This should be near or at the beginning of your program.

Most cnc's will have a default if this distinction is not defined, and the default may be to the last used mode (because these two gcodes are modal or permanent in effect until power off), or else, the control may default to either G90 or G91 when powered up.

[kdoney]

Not much help here. It looks good in Mach2.
Kevin

[corpse]

its definitely in absolute mode for basic xyz coordinates, and the ij coordinates are relative.

What I noticed is wrong with the onecnc code, which is why I'm posting here, is that in this code:

N10 X1.3125 Y2. Z0.15 
N20 Z0.11 
N30 G01 Z-0.5 F6
N40 G02 X2.6875 Y2. I0.6875 J0.

In onecnc, this is supposed to make a circle, but instead it starts at the 9 oclock position (x2y2 is the center of the circle), and finishes the circle at 3 oclock (moving clockwise) The onecnc code seems like it should be doing:

N40 G02 X1.3125 Y2. I0.6875 J0.

And this creates a complete circle.

And based on the reading I've done with the g-codes, onecnc's code seems to be outputting wrong.. please explain..

In OneCNC, I'm using the default.cfg file.. The g-codes I have to use are shown on this page http://www.acumotion.com/gcode.shtml, this is the controller setup I'm using for my sherline mill.

[HuFlungDung]

Where is the G90 or G91 defined in your program? Its not only the settings in the post that have to be correct to match your controller, but your controller also has to read a G90. If it is in incremental mode, you'll get a series of non-concentric half-circles.

In some instances, the cnc controllers cannot perform complete circles properly. In this case, you should set up your onecnc post to output 1/4 arcs maximum per movement. This will take 4 lines to move around a complete circle, but will eliminate all chance of ambiguity.

Did you know also that you can get a free update to OneCNC 2003? You should contact OneCNC for the link.

Note: I backplotted your code and it is okay, so it is most likely the lack of reading a G90 instruction that has your controller off track.

[corpse]

My stuff defaults to G90, so that is why I didn't have it in my code. I put it in the first line and it made no difference. When I put on G91, then it draws the circles like a chain-link, so that just confirms G90 is default.

And like I mentioned, the circle commands works if the starting point is on the same xy point as reference in the circle.. the onecnc code is placing the xy of the circle (xy to draw the circle to) at 180* of the starting point. If I change the code to simply make the xy of the circle command be equal to the current xy, it works fine and draws a complete circle.

[HuFlungDung]

I drew your pocket (which is centered at X1.75 Y2. ) and generated the following code with quarter circle maximum arc output:
N10 G00 X1.3125 Y2. Z0.15
N20 G00 Z0.11
N30 G01 Z-0.5 F6
N40 G02 X1.75 Y2.4375 I0.4375 J0. F12
N50 G02 X2.1875 Y2. I0. J-0.4375
N60 G02 X1.75 Y1.5625 I-0.4375 J0.
N70 G02 X1.3125 Y2. I0. J0.4375
N80 G00 Z0.15
N90 G00 X2.5625
N100 G00 Z0.11
N110 G01 Z-0.5 F6
N120 G03 X1.75 Y2.8125 I-0.8125 J0. F12
N130 G03 X0.9375 Y2. I0. J-0.8125
N140 G03 X1.75 Y1.1875 I0.8125 J0.
N150 G03 X2.5625 Y2. I0. J0.8125
N160 G00 Z0.15

So, from looking at the jumble in your code sample, I would say that your drawing must have at least one duplicate entity. This causes the tool to jump around as it attempts to machine every visible entity. Try checking your drawing, to make sure it is free of duplicate entities.

[OneCNC]

I have created two screen shots that displays your posted toolpaths on your PC based controller software. The problem is the post settings, it has nothng to do with G90 or G91. The issue is your controller requires an active G Code on everyline. This can be changed by unselecting G-Codes as Modal in NCSetup > General Settings:

Provided Sample:
N50 G01 X2.8875
N60 X3.0875
N70 G02 X0.9125 Y2. I-1.0875 J0.
N80 X3.0875 Y2. I1.0875 J0.

Should be:
N50 G01 X2.8875
N60 G01 X3.0875
N70 G02 X0.9125 Y2. I-1.0875 J0.
N80 G02 X3.0875 Y2. I1.0875 J0.

There is a Free Update to 2003 Mill Professional for all 2000 Series users: Please contact us for that update at (877) 626-1262

The image below is what appears on your controller screen based on your posted G code, the lower image is with the code edited to reflect Non Modal G -Codes:

OneCNC USA

[corpse]

Thanks a bunch onecnc - that was the fix..

I'll let my buddy know about the updates, hopefully he'll get it updated soon - I'm learning on his machine until I can figure out how to use all this stuff

huflungdung - thanks a million for your time on this, very appreciated!

[Kmed]

I know my machine will not do arcs above 359.9999xxxx degrees. In my post (not one cnc) I have a setting for arcs less than 180 and have to have this enabled. Now some machines use absolute positions with incremental IJ positions, some are incremental-incremental, and still others are absolute-absolute. I am not familiar wiht your control but this may be the problem. I dont know about all controls, but I have never seen one that required a G91 for incremental arcs. as Hu suggested, (normally embedded in the PLC). But I guess it could be a problem as he mentioned at the beginning of the program you do not have a G90, as some machine plcs ar notorious for leaving modal commands active even if the program is changed and they are not reset. (I know my Bostomatic does this when executing a new program. I dont have a G00 available so I have to use a G01 with a feedrate. This took some time to correct in the post without having to tag each line with a feed rate. which just eats up program space).... Let us know how it turns out.

should have read every ones response first whoops.. lol.