Howdy,

We are having a problem cutting a circle with approximately 12" radius.  The item is a circular tool that needs to be reduced in diameter for better fit.  Our table has a y-axis travel limit of 15", so we are cutting a little more than half of the part at a time, then rotating 180deg and running the toolpath again. 

The toolpath begins at the proper radius (12.24"), but as reaches the midpoint (X0) the radius is reduced to 12.2137", as it reaches the end of the toolpath the radius is back to 12.24".  We have tried this with backlash comp. on and off, CV on and off, and even ran a sim on other computers.  The mechanical counters on our machine confirm our DRO's so we don't believe we are completely crazy. (yet)

%
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T239 M6
N106 G0 G90 X12.234 Y-.3823 S1069 M3
N108 H239 Z2.
N110 Z.35
N112 G1 Z-.005 F6.42
N114 G3 X-12.234 Y.3823 R12.24 F10.
N116 Y-.3825 R12.24
N118 G1 Z.095 F6.42
N120 G0 Z2.
N122 M5
N124 G0 X0. Y0.
N128 M30
%

Thanks in advance for any help.

Ok a couple of days ago you determened that your machine cut a circle to .0005" tolerance so we can assume that the machine can cut a good circle.

Are you cutting an already existing part??  Are you SURE you have it fixtured so that you are acutally cutting from the true center of the arc radius and are not slightly off center???

Did you measure the finished part to determine the error??

Just a thought (;-) TP

Yes, we are cutting an existing part.  It is used to locate multiple components, one of which is mounted in the center via a 1" hole.  We used this hole to center the part in our mill setup and the only time the part was moved, it was rotated at this point.  There was no more than a .001" of play at the center. The finished part was measured 180 deg apart on the x-axis. There was only .0006" error at these points. At the points on the y-axis the error was nearly .030".  There was no re-zeroing and the part was never removed from the mill.  To measure the part we use an edge finder and jog the table in .0001" increments.

Ok the next thing I would do is to reprogram the code from a radius format arc to a center format arc to see if it changes anything. 

Can you mount an indicator and spin the part slowly to double check runout?

(;-) TP

(;-) TP

Hi,

sorry to say its your code that,s wrong, your machine is probably fine, try this code.

%
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T239 M6
N106 G0 G90 X12.234 Y-.3823 S1069 M3
N108 H239 Z2.
N110 Z.35
N112 G01 Z-0.005 F6.42
N114 G03 X0. Y12.24 R12.24 F10.
N116 X-12.234 Y-0.383 R12.24
N118 G1 Z.095 F6.42
N120 G0 Z2.
N122 M5
N124 G0 X0. Y0.
N128 M30
%

Graham.

Graham did you ever publish your Gcode help manual. I have some students that I help from time to time to understand CNC (local High school)

My manual Gcoding is way too rusty (CAM) Your book would be helpfull.

(;-) TP

I am just in the middle of a re-write, I was asked by one of the model engineering mags to do a 12 to 24 month CNC set up and programming tutorial, it has to cover milling and lathe work with working examples for each issue. Starting off simple and working up to complex parts.  It is going to be much better than the original.

Graham.