I have this working fine on a Fanuc 16i with one exception. The manual says I can use canned cycles while in this mode, but when I program a G83 for instance, it works fine except that it rapids rather than feeding, and there is no peck. So basically, it makes the move in and out of the hole, but at the rapid feed.
E.G.
Coordinate rotation of X about Y on a VMC
G18 G90 X0 Y0
G68 X0 Y0 R-45.0
G91 G83 Z-4.0 F5.0 Q.05 (This moves in the X+, Z- direction at a 45° angle)
Any help appreciated,
Thanks,
Dave
Similar Threads:
The G18 is required to get the rotation I need. Without it, the machine won't move on the correct plane.
I think you have to have the G68 in the same block as the G83. Here is an example of a similiar code on a Haas Machine: G72 G Code Explained
www.WebMachinist.Net
The Ultimate Online Source for Machinist Related Stuff!
Your example program shows the Centre of Rotation in the X Y plane and your G83 code is in the Z plane. The plane selection should be G17 for your example. If you're wanting to do something other than your example code indicates, then that's something else.
Regard,
Bill
Sorry, let me try to make this clearer.
My original description was not accurate. The drill cycle line doesn’t drill at all, it merely rapids to the Z depth on that line, moving at the 45° angle. Rapid moves and linear feed moves work great on the rotated plane, just not canned cycles. Here is the current code I'm testing.
G18 G90 G0 X0 Y0
G43 H96 Z0.
G68 X0 Y0 I0. J1.0 K0. R-45.
S200 M3
G98 G83 Z-4.0 R0. F50. Q1.0
G80 G0 Z2.0
G69
G17 G90 X0 Y0
M30
Attached is a sketch of what I’m trying to do.
Thanks,
Dave
P.S. I'm beginning to think this is a parameter setting. (BTW, I do have parameter 5101.0 set to 1)
Yes, I tried that as soon as I read it. What happens is the machine reverts to the XY plane and therefore drills only moving the Z axis. You must be in G18 mode for both axis to move simultaneously and perpendicular to the rotated plane.
I'm to the point where I'm going to have to use a macro I found on this site that uses only linear feed moves and rapids to peck drill the hole.
...not sure where that leaves me when it's time to tap the holes.
Thanks,
Dave
you need 1 of the following functions/options,
3-dimensional coordinate system conversion, A02B-0282-J713 (16i-MB)
or
Tilted working plane command, A02B-0282-S676
My manual does not show IJK in G68 block???
Try R45. instead of R-45.
Edit: I am sorry. R-45. is correct. Counterclockwise rotation is taken positive. One has to view from the positive side of the third axis, y-axis in this case.
Last edited by sinha_nsit; 01-28-2013 at 11:11 PM. Reason: correction
Fanuc G68 rotate co-ordinate system for milling program
G68 Command is used to project the operation on an angle .
G68 command parameters ,
XY - Center of rotation (co-ordinate used to measure distance )
R- Angle of rotation (operation projection angle )
In following fig . we assume corner offset co-ordinate (0 ,0) , In these fig we project the drill of 20 diameter at 45 degree only once a time and depth of drilling is 15 .
O1423
N10 M06 T05 ;
N20 G00 G90 G40 G80 G17 G21 ;
N30 M03 S1500 ;
N40 G54 X25 Y0 ;
N50 M08 ;
N60 G43 Z100 H4 ;
N70 G81 Z-15 R5 G98 F300 ;
N80 G68 X25 Y0 R45 ;
N90 X50 ;
N100 X75 ;
N110 G80 G69 ;
N120 G00 Z100 ;
N130 M05 M09 M30 ;
More examples..........!!!!
DESCRIPTION OF PROGRAM :_
O1423- Name of main program
N10- Tool change command , select tool no 5 ,
N20- Rapid command , program in absolute co-ordinate ,tool radius compensation cancle , canned cycle command (if we used) , XY plane selection command , metric input ( all dimension in mm)
N30- Spindle ON clockwise , speed is 1500 rpm .
N40- Work co-ordinate system command ( set XY value of co-ordinate) , where X25 and Y0
N50- Coolant is ON
N60- Tool height offset compensation Z100 and H4(we set tool height of z axis )
N70- Simple drilling cycle command , drilling depth is -15 , R5 is reference leave (it means tool up 5 mm and then it convert into feed for start next drilling ) , feed rate per minute is F300
N80- Rotate co-ordinate system command , where X25, Y0 at an angle 45 degree (1st drill)
N90- Next drill along X distance is 50 .( 2 nd drill)
N100- Next drill along X distance is 75 .( 3rd drill)
N110- Cancel canned cycle command , cancel co-ordinate system rotation command .
N120- Rapid action , tool goes above 100
N130- Spindle off , coolant off , main program end .
my link is
www.hdknowledge.com
Fanuc G68 rotate co-ordinate system for milling program example
August 08, 2018 - FANUC G68 ROTATE COORDINATE SYSTEM [M]
G68 Command is used to project the operation on an angle .
G68 command parameters ,
XY - Center of rotation (co-ordinate used to measure distance )
R- Angle of rotation (operation projection angle )
In following fig . we project the drill of 20 diameter at 60 degree six time and depth of drilling is 10.
O1424
N10 M06 T05 ;
N20 G00 G90 G40 G80 G17 G21 ;
N30 M03 S1500 ;
N40 G54 X15 Y0 ;
N50 M08 ;
N60 G43 Z200 H4 ;
N70 G81 Z-10 R5 G98 F300 ;
N80 X15 ;
N90 X30 ;
N100 G68 X0 Y0 R60 ;
N110 X15 ;
N120 X30 ;
N130 G68 X0 Y0 R120 ;
N140 X15 ;
N150 X30 ;
N160 G68 X0 Y0 R180 ;
N170 X15 ;
N180 X30 ;
N190 G68 X0 Y0 R240 ;
N200 X15 ;
N210 X30 ;
N220 G68 X0 Y0 R300 ;
N230 X15 ;
N240 X30 ;
N250 G68 X0 Y0 R360 ;
N260 X15 ;
N270 X30 ;
N280 G80 G69 ;
N290 G00 Z200 ;
N300 M05 M09 M30 ;
my linlk is
http://www.hdknowledge.com/2018/08/f...m-example.html
dr dave, curious to know if you could mill a basic profile using this g68 or was it just drilling in linear movements you achieved?
yes im wondering if i could achieve profiling in and x znd z axis @45deg using this way? I see you could linear drill this way which got me wondering about profiling too.