Re: EMC and G28

["Matt Shaver" <mshaver-at-erols.com>]

> From: Stephen Tate <stephentate-at-email.msn.com>
> I am in the process of modifying the Fanuc Postprocessor in Mastercam for 
> use in EMC.  However, I am not sure how to handle the G28 command, which is

> generated by the Postprocessor and not supported by EMC.  I have modified 
> the Post Processor to Generate a G0 Z.0 then a G0 X.0 Y.0 on the next line 
> in the place of G28. This approach, however, seems to lead to problems when

> I change tools.  My BOSS always trips the Z+ limit switch.  I assume this 
> is caused by G43 calls which stack up on top of the current Z0. Reference 
> point.  Is there a way to implement a relative return to the last reference

> point under the limits of EMC?

I do a quill up with:

G53G0Z0

See skeleton.txt for an empty program template. Any other questions, just
ask!

Matt

P.S. Oh, why not, here it is (it's small anyway, and it'll save you trouble
if it's not in your distribution):

N5(SKELETON 00-00-00 1 filename, date, etc...)
(set up modal operators)
N10G17G20G40G49(XY plane select, inch mode, cancel diameter comp, cancel
length offset) 
N15G54G80G94G98(coordinate system 1, cancel motion, feed/minute mode, initial
level return)
N20M48
(The next 3 lines probably aren't needed anymore, they fixed an old bug)
N25G91
N30G0X0Y0Z0
N35G90
N40G53G0Z0(retract quill)
N45X0.Y0.(move X and Y to the tool change position, change as required)
N50M05M09(spindle and coolant OFF!)
(display a message for the operator)
N55(MSG,LOAD TOOL #1)
N60M00(don't move until the operator presses the S key)
(clear the message line, I don't think this is needed anymore either)
N65(MSG, )
N70T1M06G43H1(change to tool 1 and get its length from the tool table)
(start G0 lines with a .001 second pause to avoid motion blending problems)
N75G04P.001G0X1.0Y1.0S1000M3M8(rapid to the starting XY, spindle CW, coolant
ON, change as required)
N80G04P.001G0Z0.25(rapid to .25" above the part, change as required)
( )
(the program goes here, don't have blank lines)
( )
(PROGRAM END)
N980G0Z0.25(rapid to .25" above the part, change as required)
N985M05M09(spindle and coolant OFF!)
N990G53G0Z0(retract quill)
N995X0.Y0.(move X and Y to the tool change position, change as required)
N1000M2(end program)