C-Axis Resolution

[Josh Kinney -Elite Engineering]

I'm having finish issues doing a c-axis face contour on a Mori Lathe (no Y-Axis), it appears the code is outpout without enough resolution and I'm getting notches in the finish.

 

Anyone have any ideas?

 

G20

(TOOL - 2 OFFSET - 2)

(0.750" INCH FLAT ENDMILL)

G54

G0 G53 X-.5 Z-6.0

N2 G0 T0202

G98

M45

M69

G28 H0.

G0 C136.437

G0 X1.5742 Z.25

G97 S814 M14

Z.1

G1 Z-.8 F6.42

X1.5251 C136.362 F19.92

X1.4768 C136.035 F86.88

X1.4301 C135.437 F158.68

X1.3861 C134.554 F234.03

X1.3458 C133.38 F311.19

G41 X1.3103 C131.92 F387.58

X1.2281 C127.451 F452.58

X1.1553 C122.443 F513.39

X1.093 C116.876 F576.87

X1.0427 C110.761 F639.22

X1.0055 C104.161 F695.14

X.9827 C97.192 F737.49

X.975 C90.028 F760.92

X.9825 C82.87

X1.0051 C75.921 F738.02

X1.0419 C69.348 F695.85

X1.0916 C63.267 F640.64

X1.1393 C58.839 F585.23

X1.1933 C54.792 F535.38

X1.2497 C51.279 F488.36

X1.3104 C48.078 F444.21

X1.3458 C46.622 F387.45

X1.3861 C45.448 F311.39

X1.4301 C44.565 F234.71

X1.4768 C43.967 F158.99

X1.5251 C43.64 F86.83

G40 X1.5741 C43.566 F19.72

G0 X1.5742 Z-.55 C43.563

Z.25

C-43.563

Z.1

[FP1]

On my Mori Lathes I like to use G112. It can be turned on through the misc values button on the tool path parameters page. This will cause the c-values in the g-code to represent Y values rather than degrees. Your cnc control will then interpolate these values to make a smoother path. You don't need a Y-axis machine to do this. My machines are C-axis only and it works just fine. It will also be considerably less lines of g-code.

(edit) - I am using the mpmaster post to do this. When I used the generic fanuc post it did not work.

[Josh Kinney -Elite Engineering]

I'm using an eval version of the InHouse Mori Post. I'll look for the G112. Looking at the MPLMaster its Mi4.

 

Thanks.

[Turn Master]

Go into your control def. In tolerances change the chordal deviation from .0001 to .0005. Should help your finish quite a bit.