[loedward22]

If I run a simple program (example below) that cuts the same circle in clockwise and counterclockwise directions, the result is a shift on the y axis like the illustration I have drawn. I've been stumped on this problem for weeks and have narrowed it down to this simple problem. I've considered many possible causes but am beginning to think its the way the control interprets the code (Centroid M39). Has anyone encountered anything like this before?

example G-Code:

%
N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T1 M6
N130 G0 G90 G54 X4.8943 Y2.5 S3000 M3
N140 G43 H0 Z.25
N150 Z.1
N160 G1 Z-.25 F6.
N170 G2 X.1057 R2.3943 F12.
N180 X4.8943 R2.3943
N190 G1 Z-.15 F6.
N200 G0 Z.25
N210 Z.1
N220 G1 Z-.25
N230 G3 X.1057 R2.3943 F12.
N240 X4.8943 R2.3943
N250 G1 Z-.15 F6.
N260 G0 Z.25
N270 M5
N280 G91 G28 Z0.
N290 G28 X0. Y0.
N300 M30
%


Resulting Shift:

[littlerob]

I don't know where your offsets are or what diameter your tool is, but the first thing I would try is using "I" and "J" commands instead of "R". The best reason for this is you can complete an entire circle with one line of code.

Hope that helps, I think it will, Robert

[loedward22]

I've tried switching to I and J and had the same issue. The tool is 1/4" end mill, but the problem is the same with other tools. Oh, and I'm not using diameter offsets.

[Runner4404spd]

i think your problem is backlash. how round is the hole to begin with? also cut it alot slower and see if it helps. i had a similar problem on my IH mill. apparently the bearing housing had loosened up and as long as i was going in one direction it was fine but as soon as i moved backwards the entire pattern would shift from the backlash. similar to what your seeing.

[loedward22]

i think your problem is backlash. how round is the hole to begin with? also cut it alot slower and see if it helps. i had a similar problem on my IH mill. apparently the bearing housing had loosened up and as long as i was going in one direction it was fine but as soon as i moved backwards the entire pattern would shift from the backlash. similar to what your seeing.

Backlash is one problem I've banged my head on the table about as well, but I don't think it would cause this. I may be wrong, but backlash will only shift the entire coordinates of the piece. So if you're cutting in to uncut metal the location will be slightly off from where you want it, but for any operation you perform it will be the off by the same amount. That being said, I haven't entirely ruled it out as the culprit.

[Runner4404spd]

in this particular case i think it is backlash. i don't know how your approaching the hole, but if you come in with just an x move, you never preload the y screw, so before the move is made to make the circle the backlash has to be taken up. same goes for the reverse cut. i would adjust the gibs and check your ball screw and bearings on the wy axis.

[littlerob]

With the blue pattern you are climb cutting, and with the red you are conventional milling. Could rigitity in the tool holder be the problem?

[loedward22]

in this particular case i think it is backlash. i don't know how your approaching the hole, but if you come in with just an x move, you never preload the y screw, so before the move is made to make the circle the backlash has to be taken up. same goes for the reverse cut. i would adjust the gibs and check your ball screw and bearings on the wy axis.

I'll look at it closer. The funny thing is I have more backlash on the x axis than the y axis so you'd think it would shift on the x axis as well, but only the y...

[loedward22]

With the blue pattern you are climb cutting, and with the red you are conventional milling. Could rigitity in the tool holder be the problem?

I've went down that path too and don't believe that's the cause. I've checked for motion/movement after I have the piece down and get none. The convention and climb mill is a good observation, and that's why I'm doing this. Conventional milling for a roughing pass and then climb milling for the finishing pass.

[littlerob]

I'm with runner then I would say "backlash". Sorry couldn't be more help.

[mrainey]

You only specify a Y coordinate one time. You're assuming that the tool is at Y2.5 at the start of each half-circle, but have you verified that? I'd try sticking Y2.5 in each circular move just as a test.

[EPTech]

I have had the same problem milling a rectangle. I had artifacts on the contour walls when milling with incremental depth. I do not know the deviation in your case but mine was severe (about 0.5mm). That's more then just backlash. In my case the four bolts that hold the housing of the lead-screw to the X-table were loose. Tightened them... problem solved.

[niggle]

Why do you have two G2 / G3 lines after each other, why not use I / J values?

It could be how you're just specifying an X Coordinate for the G2/3 codes, if I'm using a G2/3 code like that I always put an X and Y in there. And how you're using a G2/3 as modal (not specifying G2/3 on the line after) looks dodgy to me. I always put the G2/3 infront of it.

I'd write this as; (in metric)

G15H--
T-- (6 E/M)
M6
M1
N1
T-- (?)
S--M3
G0X25Y0
G56H--Z25M8
Z1
G2I-25Z-6F--
G2I-25
G3I-25
G0Z10
G0Z100M9
G30P2
M2

[Kool Parts]

This is the way surfcam spits it out. 2 inch circle... 1/4 endmill.. Circle center is X0.0 Y0.0.
Gary

G17 G40 G80 G90
T1 M6
S6112 M3
G0 G90 G54 X0.875 Y0
G43 Z1. H1 M8
G0 Z0.1
G1 Z0 F2.2
G3 I-0.875 J0 F4.4
G0 Z1.
Z0.1
G1 Z0 F2.2
G2 I-0.875 J0 F4.4
G0 Z1.
G0 G49 G90 Z0 M9
G28 G91 Y0 Z0
M30

[loedward22]

Why do you have two G2 / G3 lines after each other, why not use I / J values?

It could be how you're just specifying an X Coordinate for the G2/3 codes, if I'm using a G2/3 code like that I always put an X and Y in there. And how you're using a G2/3 as modal (not specifying G2/3 on the line after) looks dodgy to me. I always put the G2/3 infront of it.

I'd write this as; (in metric)

G15H--
T-- (6 E/M)
M6
M1
N1
T-- (?)
S--M3
G0X25Y0
G56H--Z25M8
Z1
G2I-25Z-6F--
G2I-25
G3I-25
G0Z10
G0Z100M9
G30P2
M2

I think you are dead on. The code I posted was directly from Mastercam, and I went back to double check everything again and have FINALLY found the solution. To do this series of checks I just loaded a sharpie in a chuck and set the height so it barely made a mark, and the output gave me a very nice fine line. Okay, then I was just trying different code and wiping the mark after each iteration. Bottom line, I change the control parameter of Mastercam's Arc setting to ABSOLUTE vs. radial and the problem is gone (this gives output in I and J instead R). I now believe the problem is on Mastercam.... and in the future am only using ABSOLUTE. I hope this thread saves others this same headache.