Re: [CAD_CAM_EDM_DRO] Decent free G-code editor?

Why can't you do: G00 Z-5, instead of 'G01 Z-5 F<whatever>'? Since the G00
*is* the Rapid Command, you'd need to issue a G01 Z<b.bb> F<b.b>, unless
your F is modal, and was previously defined. Why are you stripping out the
G0's in the first place? Or are you trying to do 'plunge milling'?

That is a technique that I highly recommend for massive stock removal in a
small machine. What you basically do is, pretend you are 'drilling' (or even
peck-drilling) a series of closely spaced (about 10% of the cutter diameter)
holes, but with a milling cutter instead of a drill. Most good endmills can
remove stock much faster in a 10% cutter diameter vertical cut than a 10%
diameter depth cut in the horizontal plane. Anyways, you wind up with a
'bead-chain' looking profile cut that's (relatively) easy to clean up in a
single full-depth pass. BTW, the first 'hole' should actually be centered on
a pilot-drilled hole, so the mill doesn't have to plunge the full depth,
cutting 100%. Your biggest problem will be removing all those chips you're
generating so fast! Most programs would issue a string of commands (again,
assuming you'd already drilled the 1st pilot hole at X2 Y1) like:

G00 X0 Y0 Z2 , assuming you'd previously set the Z0 work plane to the
top of the work surface
G00 X2 Y1 Z0.1 , rapid to 1st 'hole' co-ord's & RAPID the cutter to a safe
work plane
G83..... (at this point, issue the required parameters that the drilling
command needs)
X2.05 , assuming you're using a 1/2" dia milling cutter,
and that the G83 is modal
X2.1 , first plunge at 10%
X2.15 , 2nd
X2.2 , 3rd
X2.25 , etc.
...... , if your CAM program allows incremental
looping, it would save lots of
...... , code here if you could use it
......
X(d.dd) , last roughing cut to be made
G80 , or, whatever, to cancel the drill code,
milling cutter will be at safe height
G00 Z-(e.ee) , RAPID to whatever your working depth was
G01 Z-(f.ff) F(g.g) , FEED down to cleanup depth) at F( whatever)
X2.05 F(h.h) , FEED back to the starting point if horizontal
feedrate different than Z-axis
G01 Z0.1 F(i.i) , FEED up, to achieve a good finish on the slot, if
required
G0 X0 Y0 Z2 , RAPID back to original position

Maybe, you want the 'cleanup depth' to be the exact depth of the pilot-drill
tip, and the 'roughing' series of cuts to be the 'flute depth' of the
pilot-drilled hole'...

RayHex

-----Original Message-----
Date: Saturday, September 03, 2005 5:30 AM
Subject: [CAD_CAM_EDM_DRO] Decent free G-code editor?

>Hi All,
>
>Is there a decent visual G-code editor out there?
>I dont want something to create my toolpaths (as I have these already)
>but something I can use to safely pull out unnecessary G0 X0 Y0's that
>seem to arise when I concatenate multiple toolpaths together. Also,
>changing things like "G01 Z-5 F<SNAILSPACE>" so they rapid down through
>what's already been cut first and then plunge what hasn't, rather than
>starting plunging slowly from my safeZ.
>
>Free, or very cheap would be good, too...
>
>Cheers!
>Abby