Hello all!   [I originally posted this mistakenly to the Mach4 area]
I built an Ox CNC machine controlled with Probotix PBX-RF Isolated Breakout Board and Mach3.  Nema23 motors 2 on Y, 1 on X and 1 on Z.
I run the simulations in both Autodesk Inventor 2015 and Mach3 and the tool path is followed correctly.  When I run a test cut (using whiteboard material, with very little load on the machine) the drill portions runs fine, but when it begins cutting circles in the material it will start correctly, them 2/3 through the circle it cuts across the middle.  I searched the forum earlier today and found a post that had optimized settings for Win XP, so I followed the suggestions on stopping all processes except those needed by OS to run Mach3.

After optimizing and restarting XP, I ran the same G Code file and it ran a bit faster, but when it started the first circle it "stair stepped" about and inch, then began a circle... it was off by the distance of the stair step portion.

I am in the shop writing this and wanted to at least get a thread started.  I have images and uploaded YouTube video to show the behavior.  I really would like to get to the bottom of this as I have a project that needs to be completed (doesn't everybody???).

I appreciate any insight and yes, I have a licensed copy of Mach3.  Thanks again for any help and I will provide any files that can be used to narrow this issue down.  I will post images shortly.

Info:
Mach3 Version R3.043.066

Dell E7300 2.66Ghz Intel Core Duo CPU
2GB Ram
Windows XP Pro SP3

The PC runs very well and is not a bottom of the barrel PC.  No driver issues.

Sully

Check that your cam source and mach agree on the IJ Mode.

If your cam program is outputting arcs with IJ in absolute mode, you will get all kinds of wild tool paths unless the GCode also specifies G90.1 for absolute IJ mode
Normally Mach is configured for incremental mode. This can be set in general configuration or in GCode with G91.1

Either may be used but the way the GCode is generated (absolute or incremental) MUST match the Mach settings

Don't beat me up... this is my first attempt at CNC:

On the first two attempts, I overlayed the file using Photoshop.  This is for reference purposes and was done to better describe the issue.

See image.

Thanks Graham.  I was not aware of this and will learn it and correct it if needed.  I do know Autodesk's Cam plugin has a Mach3 profile when generating G-Code.

Here is the section of the output:

(2D CONTOUR2)
M9
G0 X4.4752 Y-0.0125
Z0.6
Z0.2
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G18 G2 X4.4877 Z-0.2106 R0.0125
G1 X4.5002 F39.4
G17 G3 X4.5127 Y0. R0.0125     <-------------------------------------- I think this is the first large circle
X2.7873 R0.8627     <-------------------------------------- I think this is the first large circle
X4.5127 R0.8627     <-------------------------------------- I think this is the first large circle
X4.5002 Y0.0125 R0.0125
G1 X4.4877
G18 G3 X4.4752 Z-0.1981 R0.0125
G0 Z0.2
X-0.7 Y1.7498
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-0.6875 Z-0.2106 R0.0125
G1 X-0.675 F39.4
G17 G3 X-0.6625 Y1.7623 R0.0125
X-1.0375 R0.1875
X-0.6625 R0.1875
X-0.675 Y1.7748 R0.0125
G1 X-0.6875
G18 G3 X-0.7 Z-0.1981 R0.0125
G0 Z0.2
X-1.325 Y1.7498
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-1.3125 Z-0.2106 R0.0125
G1 X-1.3 F39.4
G17 G3 X-1.2875 Y1.7623 R0.0125
X-2.4125 R0.5625
X-1.2875 R0.5625
X-1.3 Y1.7748 R0.0125
G1 X-1.3125
G18 G3 X-1.325 Z-0.1981 R0.0125
G0 Z0.2
X-2.7 Y1.7498
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-2.6875 Z-0.2106 R0.0125
G1 X-2.675 F39.4
G17 G3 X-2.6625 Y1.7623 R0.0125
X-3.0375 R0.1875
X-2.6625 R0.1875
X-2.675 Y1.7748 R0.0125
G1 X-2.6875
G18 G3 X-2.7 Z-0.1981 R0.0125
G0 Z0.2
X-1.325 Y-1.7748
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-1.3125 Z-0.2106 R0.0125
G1 X-1.3 F39.4
G17 G3 X-1.2875 Y-1.7623 R0.0125
X-2.4125 R0.5625
X-1.2875 R0.5625
X-1.3 Y-1.7498 R0.0125
G1 X-1.3125
G18 G3 X-1.325 Z-0.1981 R0.0125
G0 Z0.2
X-0.7 Y-1.7748
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-0.6875 Z-0.2106 R0.0125
G1 X-0.675 F39.4
G17 G3 X-0.6625 Y-1.7623 R0.0125
X-1.0375 R0.1875
X-0.6625 R0.1875
X-0.675 Y-1.7498 R0.0125
G1 X-0.6875
G18 G3 X-0.7 Z-0.1981 R0.0125
G0 Z0.2
X-2.7 Y-1.7748
G1 Z0.0394 F39.4
Z-0.1981 F13.1
G2 X-2.6875 Z-0.2106 R0.0125
G1 X-2.675 F39.4
G17 G3 X-2.6625 Y-1.7623 R0.0125
X-3.0375 R0.1875
X-2.6625 R0.1875
X-2.675 Y-1.7498 R0.0125
G1 X-2.6875
G18 G3 X-2.7 Z-0.1981 R0.0125
G0 Z0.6
G17

Digging a bit...

// user-defined properties
  useRadius: true, // specifies that arcs should be output using the radius (R word) instead of the I, J, and K words.

1. Your code looks fine in my Mach3.
2. If you are using radius mode for arcs, then my previous comments are not relevant for this job
3. I am not too clear about your picture but it looks to me as if you have some mechanical problems or are losing steps.
Check your backlash, loose belts/pulleys/something....
Have you checked that your steps per unit are correct? 3" movement on DRO is 3" on the table?
Have you done the repeatability test in the Mach User Manual Section 5 I think around page 15.
If the steps per unit are OK and you find no significant mechanical issues, go to motor tuning and cut you speed down by 75% and your acceleration to 10% of the new speed and try again.
Graham

Graham, you did point me in the right direction and I really appreciate it!!!  The issue was my General Config > Distance Mode > Inc and I tightened my X axis belt.

These are my third attempt (first attempt after the change) and what a blast... CNC is going to be really interesting moving forward.

Thanks again for taking the time to help me.

Sully

Sully,
Thanks for the update. Glad it is working out.
Graham