Re: Correct use of subroutines
My old school answer is that most subs should be written in (G91) Incremental
mode.
My more modern method can be either G90 or G91 depending on the application but
I use variables for D, F, Z and loop to run Z level roughing and finishing
often using several tools.
RE: G84
BTW it is the programmers job to lie to the machine - the machine should NEVER
lie to the operator.
The value you use for your F should be exactly what the machine feeds at. No
IF's ands or buts... 100% F
This is also a key safety point - The operator needs to be able to read the
G-code and KNOW exactly what the machine will do when it tries to execute that
code.
Now if you are using a using a specific tool which needs to run at a reduced
feed then you as the programmer should alter the programed feed rate. In this
case if you wanted to use a Osub to do your tapping and you wanted it to feed
at 95% thats fine - its all man readable in the Osub - Fixed cycles don't
display the inner workings so others would not know of your 95% mod.
While I started out on a Bandit CNC way back and subs were critical with
controls that could only handle like 99 command lines. I have also run the
FANUC, OKUMA, HAAS gauntlet but with LinuxCNC the line limit isn't - so simple
top down programs are often simpler, the geek in us would rather loop, than cut
and paste.
What I would like to know is that if you put:
G00 G20 G43 G54 G90 Z.5 H# S1000 M3
G84 X1. Y1. Z-.5 R.2 F20.
X2.
G80 Z1.
M2
What action or error is observerd with the current release. Note this would
require a full programmable spindle with feedback.
What Should happen when the above code runs is:
Spindle On FWD (CW) 1000rpm (spindle at speed set)
Tool rapids to Z.5
rapid to X1. Y1.
rapid to Z.2
feed spindle at 20 IPM to Z-.5
spindle reverses (any observed dwell is from the spindle controller) and feeds
out at 20IPM to Z.2
tool stays at Z.2 (G99) OR tool rapids to Z.5 (G98)
tool rapids to next hole location ( X2. Y1.) and cycle repeats.
(G80) Fixed cycle mode cancel, tool rapids to Z1. (note: some name brand
controls will execute an M5 when a G80 is read)
program end.
I'm all for adding some missing functions that would make it easier to use
commercial CAD/CAM systems. I hope to work with Mecsoft and AlibreCAM to get a
3 axis post and later a 4 axis post once I finish a suitable test bed machine.
Also hope to work towards a lathe test bed.
Greg
------------------------------------------------------------------------------
Learn Graph Databases - Download FREE O'Reilly Book
"Graph Databases" is the definitive new guide to graph databases and
their applications. This 200-page book is written by three acclaimed
leaders in the field. The early access version is available now.
Download your free book today! http://p.sf.net/sfu/neotech_d2d_may
_______________________________________________
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
