I'll jump in. I have the Fanuc 18m manual out. G65 = custom macro call. The P word calls the macro. All other addresses relate to variables in the macro. IE: Z#26 in the macro = Z in the G65 block; X#24 in the macro = X in the G65 block. M98 = simple sub call
I think Dave may be looking for a G68 coordinate rotation call: G68 X=center of rotation Y=center of rotation R=angle of rotation M98 P G69 (cancels G68) repeat as needed. Benz -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of John Gent Sent: Thursday, March 18, 2004 11:36 AM To: 'SmartCam Forum' Subject: RE: [mfg-smartcam] SUB ROTATION Hi Dave, I don't remember if it's G65 or M98 for subs with an OM, so I'll use G65 for the example. I'm not positive, but I think the R in the G65 does the transformation (plane rotation). @GOSUB G65 P#SNAME L#SREPT R#ROT2 This is supposed to do the first call and where ever the last position of that sub is, starts the first position of the next repeat, rotated around the handle by the incremental angle. The way I remember it is that if you use any absolute stuff in the sub, it will certainly screw up. I'm not sure how to use #ROT1 other than if you want to call the sub once, rotated (?). I also don't have a Fanuc programming manual here so it is hard to confirm any of what I just typed. Hopefully someone can jump in and fill in the blanks or correct where I might have blown it. Anyone? - John Gent McKenzie River Software Your Exclusive Source for SmartCAM -----Original Message----- From: Dave Wolfgang [mailto:[EMAIL PROTECTED] Sent: Thursday, March 18, 2004 5:35 AM To: John Gent; 'SmartCam Forum' Subject: Re: [mfg-smartcam] SUB ROTATION Thank you John for your responses on the #ROT1 and #ROT2 code words. I understand the purpose of the code words my question I was trying to ask was were in the TMP does it get used. And most of all there has to be a G code outputted to tell my OM control the plane has rotated. If I program my subs in incremental moves and my first move would only be a X+. At #ROT1 I rotate my sub +45^ the control now has to move X+ and Y+ with the same sub program. To better under stand my thought if I would generate a sub at 0^ then rotate the same sub call at 180^ the same sub would read X+ but my machine would be moving X- something would have to tell my control to reverse the plane moves and same would hold true for radius moves. Dave Wolfgang CNC Programmer/Supervisor www.hrindustries.net ----- Original Message ----- From: "John Gent" <[EMAIL PROTECTED]> To: "'SmartCam Forum'" <[EMAIL PROTECTED]> Sent: Wednesday, March 17, 2004 11:32 AM Subject: RE: [mfg-smartcam] SUB ROTATION > Hi Dave, all. > > #ROT1 is how much to rotate the first call to your sub (absolute). > (#ROT2 is > for incremental rotations of multiple calls) > > To cut a diamond shape with a single line sub, for example. > > The sub consists of a single line 1 long at zero degrees from X0Y0. > The handle is at X.5Y.5 (also the point to rotate around). > > The sub call will rotate repeats 3 times (4 total) rotated 45 degrees > (the initial rotation). Note that the repeat angle is given at 90 > degrees, based > on the handle of the sub - it is the only angle that will make the end > of one meet the start of the next. > > So code will set $ROT1 = 45 and #ROT2 = 90 ($SREPT = 3) > > Sub is called and the initial rotates the first line 45 degrees > (around the > handle) - cuts - incrementally rotates 90 degrees - cuts - and repeats > the incremental thing 2 more times. > > I tried to keep this simple, but something tells me the murk may be > defeating my intent <grin>. Still, I hope this helps. > > - John Gent > McKenzie River Software > Your Exclusive Source for SmartCAM > > > -----Original Message----- > From: [EMAIL PROTECTED] > [mailto:[EMAIL PROTECTED] On Behalf Of Dave Wolfgang > Sent: Monday, March 15, 2004 8:54 AM > To: SmartCam Forum > Subject: [mfg-smartcam] SUB ROTATION > > > I do sub programming and when I define a sub, I would like to do a > #ROT1 (rotation). Can someone explain how and where #ROT1 is used. > > > Dave Wolfgang > CNC Programmer/Supervisor > www.hrindustries.net > > > > ====================================================================== > 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] ======================================================================
