Re: G76 format?

Thanks Andrew!

So, that's the two line form, eh? Neat. Thanks for taking the
time to look it up and post it.

Questions: Are Q, R, I, and the second P always in the implied
decimal format? Since Z, X, and F are decimalized, it seems kind of
strange to mix the two in the same code - doubly so since retrofits
have all kinds of different resolutions.

I'm a bit unclear the effect of the chamfering amount in the second
two chars of the P word. Is the thread chamfered with the threading
tool explicitly by the G76 cycle? Seems like one would want to to
this with another tool, but I guess it could be pretty convenient
though as part of the threading action. Or is this just "stay out"
information so the cycle can be optimized?

Don, if you want to post the one line form online it'd probably be
appreciated by the group members as well. Although I've begun back-
decoding it from the Gcode made by Lathe Quick Code (thanks to Fred
from imserv), it'd be very helpful to have a specification to start
from. Bad form to rely on others' programming to enforce a standard -
even though that's exactly how it happens in the real world!

I think I might end up supporting both with a global dialect option
for 2 line vs 1 line G76 forms, since no doubt both will have their
adherents.

Thanks again. This helps immensely.

Dave Kowalczyk
Everett WA

--- In CAD_CAM_EDM_DRO@yahoogroups.com, "Andrew Erwood" <a_k@a...>
wrote:

> Hi Donald and Dave,
>
> Here is the definition of G76.
>
> G76P(m)(r)(a) Q(d min) R(d);
> G76X_ Z_ R(i) P(k) Q(dd) F(l);
>
> m = Number of finishing cuts
> r = Chamfering amount
> a = Angle of tool tip
> d min = Minimum cutting depth (specified in radius value)
> d = Finishing allowance (in radius value)
>
> X = X axis destination
> Z = Z axis destination
> i = Taper value (in radius value)
> k = Height of thread (in radius value)
> dd= Depth of first cut (in radius value)
> l = Lead of thread
>
> For example:
> G76 P010060 Q100 R200;
> G76 X60.64 Z-25. P3680 Q1800 F6.;
>
> This code cuts a thread with one finishing cut, no chamfer on the

exit of

> the tool, with a tool tip angle of 60deg. It will have a minimim

depth of

> cut of .1mm and will have a finishing allowance of .2mm. The minor

diameter

> of the thread is 60.64mm and it will cut a thread 25mm long in the

Z minus

> direction. The height of the thread is 3.68mm and the depth of the

fist cut

> is 1.8mm and the thread has a lead of 6mm. This thread is a

straight thread

> with no taper.
> As a general rule of thumb, on a 1.5mm pitch thread I would have

approx 12

> passes to complete the thread with a full form insert and I run

about 250

> meters/minute cutting speed. At this speed I get VERY good tool

life.

>
> Hope this helps.
>
> Regards
> Andrew
>
>
> -----Original Message-----
> From: Donald Brock <don.pat.brock@p...> <don.pat.brock@p...>
> To: CAD_CAM_EDM_DRO@yahoogroups.com

<CAD_CAM_EDM_DRO@yahoogroups.com>

> Date: Monday, December 30, 2002 8:46 AM
> Subject: [CAD_CAM_EDM_DRO] Re: G76 format?
>
>
> >Dave,
> >
> >I'd like to help with this also. I'll post another responce to this
> >monday evening when I have my manuals/notebooks in hand. Let me

know

> >if you prefer a group or off line responce.
> >
> >I'm totally in favor of the fanuc method which does the g-76

(canned

> >cycle) multipass threading (both tapered and straight)with a single
> >line of code versus the the two line command canned cycle as used

on

> >the mitsubishi and others. They are basically the same just

different

> >methods of entering the varibles for the macros.
> >
> >I may have a print out of the mitsubishi g-76 macro somewhere. I'm

in

> >the middle of changing isp's so my e-mail address may not be valid

if

> >you try to respond off line.
> >
> >Donald Brock
> >
> >> Anyone know what the defacto-standard is for G76 canned cycle
> >> threading these days? I'd like to implement this in my control,
> >and
> >> as you all know, we're not exactly short of variety in G codes.
> >>
> >> Thanks.
> >>
> >> Dave Kowalczyk
> >> Everett WA
> >> Author of TurboCNC --> http://www.dakeng.com/turbo.html
> >
> >
> >Addresses:
> >FAQ: http://www.ktmarketing.com/faq.html
> >FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> >Post Messages: CAD_CAM_EDM_DRO@yahoogroups.com
> >
> >Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
> >Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
> >List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@a...
> >Moderator: jmelson@a... timg@k... [Moderator]
> >URL to this group: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
> >
> >OFF Topic POSTS: General Machining
> >If you wish to post on unlimited OT subjects goto:
> aol://5863:126/rec.crafts.metalworking or go thru Google.com to

reach it if

> you have trouble.
> >http://www.metalworking.com/news_servers.html
> >
> >http://groups.yahoo.com/group/jobshophomeshop I consider this to

be a

> sister site to the CCED group, as many of the same members are

there, for OT

> subjects, that are not allowed on the CCED list.
> >
> >NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING

THEM.

> DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........
> >bill
> >List Mom
> >List Owner
> >
> >
> >
> >Your use of Yahoo! Groups is subject to

http://docs.yahoo.com/info/terms/

> >
> >