can anyone help me out with these codes maybe asample program
Printable View
can anyone help me out with these codes maybe asample program
On a Fanuc control G68 is coordinate rotation "On" and G69 Coordinate rotation "Cancel". On your line with G68 supply the X & Y value for the position of rotation and an "R" in degrees of rotation. A negative number will rotate CCW.
G68 X0 Y0 R90.
At the end of the run use the G69.
I found some more info but the string you gave me was helpful. On the mazatrol m plus its G17 G68 X0 Y0 R5 for example. But my machinist here has raised the issue of whether this code only has to be inserted at the beginning of the program or at each tool change. Can you shed some light on this for me?
Eric
Don't know much about mazatrol but on the controls I have programmed if you want to rotate the entire program you just put it at the start. If you want to rotate parts of the program you turn it on and off as needed.Quote:
Originally Posted by ebragdon
Also if by chance you are also using local work offsets G52, in my experience mixing the two can sometimes be unpredictable.
On most controls including Mazatrol, there are some commands that won't work in G68 mode and you probably wouldn't want it to anyway. So, things like tool change commands, G28/G30 commands, etc won't generally work. This means you need to turn G68 on/off for each tool in the program.
You also cannot randomly change work offsets in G68 mode so on some controls, using G53 as a retract may become a problem (Since this is viewed as an offset for some machines).
You can use it in G52 mode and it's not that it becomes "unpredictable" but you certainly need to visualize it enough to follow it.
A wise thing to do is after picking up your work offset, turn on G68. At the end of the tool (before tool change), turn off G68 (G69). Next tool do the same thing....
Syntax:
G17 G68 X_ Y_ R_;
as already described.
If you omit XY words, the current tool position becomes the center of rotation.
FANUC G68 ROTATE COORDINATE MAIN PROGRAM & SUB PROGRAM EXAMPLE
August 08, 2018 - FANUC G68 ROTATE COORDINATE SYSTEM [M]
MAIN PROGRAM
N10 G54 X0 Y0 ;
N20 M06 T05 ;
N30 G43 H5 ;
N40 M03 S1500 ;
N50 M08 ;
N60 G98 F300 ;
M98 P034321 ; sub program call
N70 G00 Z100 ;
N80 M05 M09 M30 ;
SUB PROGRAM
O4321
N10 G91 G68 X10 Y10 R22.5 ;
N20 G90 X30 Y10 Z5 ;
N30 G01 Z-5 ;
N40 X47 ;
N50 G00 Z5 ;
N60 M17 ;
DESCRIPTION OF PROGRAM
Main program
N10- Work co-ordinate system command ( Offset point) , where X0 and Y0
N20- Tool change command , select tool no 5
N30- Tool height offset compensation H5(we set tool height of z axis )
N40- Spindle on clockwise at speed 1500 rpm
N50- Coolant on
N60- Feed rate per minute F300
M98- Sub program call , P03- no same operation repeat ,4321- no. of sub program.
N70- Rapid command , where Z100 [ tool up ]
N80- Spindle off , coolant off , main program end
Sub program
N10- Incremental co-ordinate command , rotate coordinate system command where X10 , Y10 and angle of rotation R22.5
N20- Absolute co-ordinate command , X axis distance count from 0 to starting position ,Y at same place 10 and tool is 5 mm up.
N30- linear interpolation command , cutting depth is 5
N40- Operation end position 47 along X
N50- Rapid command , tool up 5 mm
N60- Sub program end .
my link is
FANUC G68 ROTATE COORDINATE MAIN PROGRAM & SUB PROGRAM EXAMPLE - CNC PROGRAMMING TUTORIAL