Rotate G68

[cadman@teluspla]

Can anyone provide a detailed sample of a program using G68
I can get my profile cut with no problem but when I try to rotate about
X0.0 Y0.0 I get alarms

[Donkey Hotey]

Do you have the Coordinate Rotation & Scaling option on your control? What are the alarms you're getting?

[pit202]

with error you get ? maybe you doesn`t have rotation ?
typical use of G68:

G59
G00 G90 X0 Y0 Z0
M98 P1 ( some shape ) 
G90 G0 X0 Y0
G68 R60 ( optionally X and Y )
M98 P1 ( some shape ) 
G69 G90 G0 X0 Y0
M30

[cadman@teluspla]

We do have rotation & scaling and parameter is turned on
I managed to get rid of the alarms however when the program is run it loops around twice in the same location, I have missed something
%
O00091
(GRIZZLEY)

T4 M06
(.5 HANITA)
G54
G90 G00 X0. Y0.
M88
S2250 M03
G43 H04 Z1. M08
M98 P93 L2
G00 Z2. M09
M89
G91 G28 Z0
G90
M30


093
G91 G68 R45
G90 M98 P1
G90 G00 X0 Y0
G00 X4.882 Y-0.3155
G90 G42 G01 X5.5908 Y0.25 D04 F10.
G01 X5.591 Y1.3 F20.
G03 X5.316 Y1.575 R0.275
G01 X5.157
G03 X4.882 Y1.3 R0.275
G01 Y-1.3
G03 X5.157 Y-1.575 R0.275
G01 X5.316
G03 X5.591 Y-1.3 R0.275
G01 Y0.
G00 Z0.5
G40 G01 X5. Y0.5
G90 G00 X0.0 Y0.0
M99

[cadman@teluspla]

The problem has been solved with the help of Haas factory Answer Man
in the code G91 G68 R45
there is a decimal point missing behind the R45
It should read G91 G68 R45.
Thanks to those who tried to help

[Donkey Hotey]

DOH! Thanks for following up with us. Yes, the ol' missing decimal point problem. That's easy to miss. I've done it too many times.

[Zak@CWS]

I'm also having an issue with Mastercam X2 and a VF-3: we're using the X2 haas post, G68 incremental is enabled. When we first load the program, we'll get a line like:
G90 Xxx Yyy G68 X.0 Y0. G91 R-72. Haas doesn't like this and throws a "multiple code" error. I can understand that, it doesn't like the G90 and G91 in the same line. If I split the block at the G68, we wind up with very strange tool paths, rapids with some details in the cycle being skipped over and others being "cut" twice. Is this a post problem, operator error, or maybe parameters in the machine?

[I_flungdung]

I use the G68 a lot and the following works for me. Put it in a line by itself. Also check out your parameters/settings. In my case, the part is rotated a positive 28 degrees from 0 degrees. It is in the X Y plane and is in inches. The last line is the first move for some face milling.

M06T1
M08
M88 (through spindle coolant)
G00 G90 G154 P1 X0. Y-1.5 S1200 M03
G43 H01 Z2.72
G68 G17 X0. Y0. R28.
G01 Y-3.5 F30.

[Frank_S]

I'm also having an issue with Mastercam X2 and a VF-3: we're using the X2 haas post, G68 incremental is enabled. When we first load the program, we'll get a line like:
G90 Xxx Yyy G68 X.0 Y0. G91 R-72. Haas doesn't like this and throws a "multiple code" error. I can understand that, it doesn't like the G90 and G91 in the same line. If I split the block at the G68, we wind up with very strange tool paths, rapids with some details in the cycle being skipped over and others being "cut" twice. Is this a post problem, operator error, or maybe parameters in the machine?

Are you cutting the part using G91 or just using G91 to increment the angular rotation? I always try to avoid using G91 unless I absolutely have to. You might want to try using a positive angular rotation rather than negative. It would aslo help if you posted more lines of code.