Yes I do use the G10 but I use it to change the values in our fixture offsets when we require more then 6 fixture offsets I'll investigate further. Thanks. -----Original Message----- From: Dave Coupar <[EMAIL PROTECTED]> To: Michael Senack <[EMAIL PROTECTED]>; '[EMAIL PROTECTED]' <[EMAIL PROTECTED]> Date: Saturday, July 08, 2000 7:22 AM Subject: RE: [mfg-smartcam] Cutter diameter for Fanuc OM Series control
>Michael, > >I don't have a 0M manual handy, but the other Fanuc controls use G10 with an >Lnn and Pnn to specify which type (Tool Length, Tool Diameter, Work >Coordinates) and which number to modify, i.e. G10 L2 P2 X-1.2340 Y-2.345 >would set G55 registers to those values. > >Also, you can use G10 G90 to set the values or G10 G91 to increment the >values. > >Dave > >-----Original Message----- >From: [EMAIL PROTECTED] >[mailto:[EMAIL PROTECTED]]On Behalf Of Michael Senack >Sent: Friday, July 07, 2000 4:00 PM >To: '[EMAIL PROTECTED]' >Subject: [mfg-smartcam] Cutter diameter for Fanuc OM Series control > > >Below is a sample from our Bostomatic milling machine. In it we can change >the cutter diameter that is entered in by the operator anywhere in the code >using a G39 code followed by a D register with the diameter you want to use >in 4 place decimal format. Lets say the operator sets T4=1.0 FINISH E/M to >1.0 diameter in the control and it profiles the outside of a cam follower >using a subroutine. We can enter G39D1.1 and run the subroutine and it will >leave .05" mat'l/side or .1" on diameter of the cam follower for a roughing >pass then we can say G39D1.0 and run the subroutine again at finish size. >Neat... > >Sample Bostomatic code > >% BO0708.M 3501G-1150-005 REV.AB OP.1 >% >% ****************************** >% SET ALL TOOL DIAMETERS TO ZERO >% ****************************** >% >N40M0 T2 1-1/2 FINISH E/M L >N41T2 >N42G39D0.0 THIS SETS ANY PREVIOUS G39D TO ZERO BECAUSE IT IS A MODAL >COMMAND >N43G1M3S27F1.0 >N44G4X6. >N45X3.45Y0.0R >N46G48R >N47Z0.1R >N48ZM8 >N49G39D-0.025 SEMI-FINISH PASS 1.574-1.5=.074 .074/2=.037 .037-.025=.012 >MATL/SIDE >N51Z-.9R >N52Z-1.010 >N53G94D100 >N54G39D-0.037 FINISH PASS 1.574-1.5=.074 .074/2=.037 .037-.037=0 FINISH >PROFILE CAM TO SIZE >N56Z-1.010 >N57G94D100 >N58Z4.0RM9M5 >N59G49R > > >Now we have a Hurco milling center with an OM Series Fanuc control, and I'm >reprogramming the above job sample from the Bostomatic which uses G39's >codes to the Hurco. >My question is...does the Fanuc OM Series control have any way of >programming cutter diameter in the code? > >Thanks >====================================================================== >To find out more about this mailing list including how to unsubscribe, >send the message "info mfg-smartcam" to [EMAIL PROTECTED] >====================================================================== > >====================================================================== >To find out more about this mailing list including how to unsubscribe, >send the message "info mfg-smartcam" to [EMAIL PROTECTED] >====================================================================== ====================================================================== To find out more about this mailing list including how to unsubscribe, send the message "info mfg-smartcam" to [EMAIL PROTECTED] ======================================================================
