C - Axis Face Contour w/ Mastercam

[rexster_001]

I'm using MasterCam X2 and I'm programming a 1.720 X 1.720 square. The CNC Lathe I'm using is a Mori Seiki SL-200 with live tooling. When MasterCam spits out the code it looks a little something like this. (No I don't have Y - Axis)

%
O0033
(PROGRAM NAME - SQUARE TEST)
G20
(TOOL - 5 OFFSET - 5)
( 5/8 FLAT ENDMILL)
( ROUGHING THE 1.720" X 1.720" SQUARE )
G0 T0505
M45
M91
G0 G54 X4.9827 Z0.
C-49.033
G97 S750 M13
M8
G98 G1 Z-.5 F20.
X4.7261 C-49.252
X4.472 C-49.494
X4.2202 C-49.763
X3.9707 C-50.063
X3.7235 C-50.4
X3.4784 C-50.782 F31.
X3.2968 C-51.101
X3.1151 C-51.459
X3.075 C-51.594 F66.35
X3.0361 C-51.831 F115.66
X2.9993 C-52.168 F164.97
X2.9652 C-52.603 F212.83
X2.9347 C-53.13 F257.99
X2.9082 C-53.742 F299.09
X2.7729 C-57.748 F333.39
X2.6529 C-62.125 F365.53
X2.5501 C-66.869 F397.52
X2.4663 C-71.96 F427.66
X2.4034 C-77.351 F453.83
X2.3628 C-82.97 F473.77
X2.3456 C-88.722 F485.47
X2.3523 C-94.498
X2.3826 C-100.185
X2.4357 C-105.68 F463.57
X2.5103 C-110.902 F439.93
X2.6046 C-115.794 F411.35
X2.7167 C-120.324 F380.02
X2.8087 C-123.393 F352.27
X2.9082 C-126.259 F329.14
X2.9446 C-127.324
X2.9761 C-128.432
X3.0028 C-129.578 F350.16
X3.0242 C-130.753
X3.0405 C-131.95 F366.1
X3.0513 C-133.164
X3.0568 C-134.387
C-135.613
X3.0513 C-136.836
X3.0405 C-138.05
X3.0242 C-139.247
X3.0028 C-140.422
X2.9761 C-141.568 F350.16
X2.9446 C-142.676 F338.95
X2.9082 C-143.741 F325.43
X2.7728 C-147.747
X2.6528 C-152.124 F365.53
X2.55 C-156.869 F397.53
X2.4662 C-161.959 F427.67
X2.4033 C-167.351 F453.84
X2.3628 C-172.97 F473.78
X2.3456 C-178.722 F485.48
X2.3522 C-184.498
X2.3825 C-190.185
X2.4356 C-195.681 F463.58
X2.5102 C-200.903 F439.94
X2.6045 C-205.794 F411.35
X2.7167 C-210.324 F380.03
X2.8087 C-213.393 F352.27
X2.9082 C-216.259 F329.06
X2.9446 C-217.324
X2.9761 C-218.432
X3.0028 C-219.578 F350.16
X3.0242 C-220.753
X3.0405 C-221.95 F366.1
X3.0513 C-223.164
X3.0568 C-224.387
C-225.613
X3.0513 C-226.836
X3.0405 C-228.05
X3.0242 C-229.247
X3.0028 C-230.422
X2.9761 C-231.568 F350.16
X2.9446 C-232.676 F338.95
X2.9082 C-233.741 F325.43
X2.7728 C-237.747
X2.6528 C-242.124 F365.53
X2.55 C-246.869 F397.53
X2.4662 C-251.959 F427.67
X2.4033 C-257.351 F453.84
X2.3628 C-262.97 F473.78
X2.3456 C-268.722 F485.48
X2.3522 C-274.498
X2.3825 C-280.185
X2.4356 C-285.681 F463.58
X2.5102 C-290.903 F439.94
X2.6045 C-295.794 F411.35
X2.7167 C-300.324 F380.03
X2.8087 C-303.393 F352.27
X2.9082 C-306.259 F329.06
X2.9446 C-307.324
X2.9761 C-308.432
X3.0028 C-309.578 F350.16
X3.0242 C-310.753
X3.0405 C-311.95 F366.1
X3.0513 C-313.164
X3.0568 C-314.387
C-315.613
X3.0513 C-316.836
X3.0405 C-318.05
X3.0242 C-319.247
X3.0028 C-320.422
X2.9761 C-321.568 F350.16
X2.9446 C-322.676 F338.95
X2.9082 C-323.741 F325.43
X2.7728 C-327.747
X2.6528 C-332.124 F365.53
X2.55 C-336.869 F397.53
X2.4662 C-341.959 F427.67
X2.4033 C-347.351 F453.84
X2.3628 C-352.97 F473.78
X2.3456 C-358.722 F485.48
X2.3522 C-364.498
X2.3825 C-370.185
X2.4356 C-375.681 F463.58
X2.5102 C-380.903 F439.94
X2.6045 C-385.794 F411.35
X2.7167 C-390.324 F380.03
X2.8087 C-393.393 F352.27
X2.9082 C-396.259 F329.06
X2.9446 C-397.324
X2.9761 C-398.432
X3.0028 C-399.578 F350.16
X3.0242 C-400.753
X3.0405 C-401.95 F366.1
X3.0513 C-403.164
X3.0568 C-404.387
C-405.613
X3.0513 C-406.836
X3.0405 C-408.05
X3.0242 C-409.247
X3.0028 C-410.422
X2.9761 C-411.568 F350.16
X2.9446 C-412.676 F338.95
X2.9082 C-413.741 F325.43
X2.7945 C-417.049
X2.7748 C-417.786 F360.49
X2.7604 C-418.579 F387.65
X2.7518 C-419.409 F406.3
X2.749 C-420.259
X2.7521 C-421.109
X2.7612 C-421.937
X2.8401 C-426.561 F386.26
X2.9367 C-430.916 F363.13
X3.0495 C-434.983 F338.16
X3.1769 C-438.754 F312.56
X3.3176 C-442.233 F287.28
X3.4701 C-445.431 F262.99
X3.6129 C-448.021 F241.47
X3.7624 C-450.408 F222.67
G0 Z1.0
M9
G28 U0.
G28 W0.
M05
M46
G99
M91
T0500
M30
%


After I machine the part the part comes out with a bad finish. Its not tool chatter or part chatter. The finish looks wavy. Can somebody tell me why the finish is coming out like that and is there a fix?

Many Thanks!

[cnc-king]

never worked on a Mori but on our Daewoo, MasterCam X2 spits out G112 at the begining and G113 at the end on face contour ops for the X and C moves which is for polar coordinate interpolation. you may want to check your misc integer 4 to see if it is turned on

[CNCRim]

Bad finish is come from the little segment from the output of the program.......try program different.

[chuy]

i've been on a kia ,but i'm just seeing the feedrate and it looks really fast and all over the place can't you slow that down? and make it an even feed rate.and kick your spindle speed up.

[Mike Mattera]

The feedrate for rotary is in Degree's per min or inverse time.

Mike Mattera

[Mike Stevenson]

I suggest you start with the basics:

1. How rigidly are you holding the part in the chuck?

2. How long is part?

3. How far is it extended from the chuck?

4. How long is the end mill you are milling with?

[wine]

i want to learn mastercam lathe c axis so much but i can not find it on net... if you have, please send. Thank you so much.

[CNCRim]

Originally Posted by wine i want to learn mastercam lathe c axis so much but i can not find it on net... if you have, please send. Thank you so much.

F1 in the help section should have few example you can learn from it.

[danhaskell]

Post it in polar cords. g112/g113

[Stebedeff]

This is what you need to do.
For C-axis with spindle on left side always have your contour on the right plane. In the first parameter page choose C-axis for Rotary axis and in miscellaneous change the 0 to a 1 to activate G112/G113 Third or 4th line I guess.
The best is to use radius compensation to better understand what machine is doing and what's going on. Don't forget to put the 1/2 diameter of you mill in your machine offset and set your comp. type/point to "0" .

You might find out that the G113 is called up before G40 in the posted programm. If your using FANUC this will give a alarm. G113 must be after your G40 block.

Good luck!