Originally Posted by
Deano7/11
I did notice the y only move but as this is a knee mill with z on the quill having the vice and job way out the way of me manually changing tools appeals to me at the moment.
when you say to alter the tc program i assume cause i dont have a auto tool changer this is not needed.??
- So what does the M6 do in your machine ???
the M6 should be calling up a little macro, or just have a Z return (G0 G91 G28 Z0.) with a program stop ( M00 )
so how would you suggest i have my end of toolpath/program outputting???
were would i put the g80?
something like
g91 g28 z0
g28 x0 y0
g90 g80
a0
not sure what you mean about the g94 tho. what will that do?
The G94 would be used as a safety code, so if you did any machining with a feed per revolution ie tapping, it would be changed back to your normal setting for milling
I have mine output after any drill cycles, just to be safe
- the * before the postblock actually forces the output to the NC file, even if it is a modal code.
Code:
pcanceldc$ #Cancel canned drill cycle
result = newfs(three, zinc)
z$ = initht$
if cuttype = one, prv_zia = initht$ + (rotdia$/two)
else, prv_zia = initht$
pxyzcout
!zabs, !zinc
prv_gcode$ = zero
pcan
pcan1, pbld, n$, *sg80, *sg94, strcantext, e$
#if drillcyc$ = 3, pbld, n$, sg94, e$
pcan2
IMO, the required output NC code before each toolchange you need is
- I placed the modal G codes so you can see whatis actually active
Code:
G80 G94 ( this line outputs after any drill cycle )
M5
M9
G0 G91 G28 Z0.
G0 G91 G28 X0. Y0.
G0 G90 A0. ( the A0. can be omitted if you only have 3 axis )
M1 ( optional stop, good for when proving off, or wanting the program to stop to inspect the cut, tool, part size etc.- by just flicking the OPT. STOP switch to ON )
I would also NOT have the G49 ( cancel tool length ) output on the toolchange line, it doesn't do anything, as the next G43 will reset tool length