|
N6#[2000+#100]=#[5023](MACHINE Z0 INTO
OFFSET)
this IS right, I moved
the # sign and put ( in front of it instead of
[.
Lee
Yes I'm sure. It works great in a OM
control.
----- Original Message -----
Sent: Wednesday, August 01, 2001 8:03
AM
Subject: RE: [mfg-smartcam] Fanuc tool
change
Just looking here, but on line N6, is are the # signs in the
right place?
Rick
-----Original Message-----
From:
lee [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 31, 2001
1:28 PM
To: Smartcam Mailing List (E-mail)
Subject: RE: [mfg-smartcam]
Fanuc tool change
Dave,
That program runs great as long
as I skip line 6 with it I get a parameter
error. Do you think 5023 is a
parameter to enter active tool z value? that
param must be different on
my control. I'll look into it.
Lee
-----Original
Message-----
From: Dave Wolfgang
[mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 31, 2001 5:56
AM
To: lee; Smartcam Mailing List (E-mail)
Subject: Re: [mfg-smartcam]
Fanuc tool change
Lee
This is what I
use. You must have macro B turned on in your machine.
Program starts at
tool #1
O1999
(TOOL-SETTING PROGRAM)
N1#100=1(SET #100
EQUAL TO FIRST TOOL)
N2DO1(BEGINNING OF LOOP)
N3T[#100](SELECT
TOOL)
N4M6(TOOL CHANGE)
N5M0(SET TOOL OFF
Z0)
N6#[2000+#100]=#[5023](MACHINE Z0 INTO OFFSET)
N7G0G91G28Z0(RAPID
TO Z AXIS ZERO RETURN)
N8#100=#100+1(INCREMENT TO NEXT
TOOL)
N9END1(END INDEFINITE LOOP)
N10G90(SWITCH BACK TO ABSOLUTE
COORDINATES)
M30
%
Dave Wolfgang
CNC
Programmer/Supervisor
www.hrindustries.net
<http://www.hrindustries.net>
----- Original Message -----
From: lee <mailto:[EMAIL PROTECTED]>
To:
Smartcam Mailing List (E-mail)
<mailto:[EMAIL PROTECTED]>
Sent: Monday, July 30,
2001 7:10 PM
Subject: [mfg-smartcam] Fanuc tool
change
everyone,
I'm looking for ideas and suggestions
on the best way to automatically
change a predefined number of tools for
entering tool length offsets into a
Fanuc 18-m. Our control doesn't seem
to have this option. We run allot of
short runs and using MDI to type
tool number +M6 up to 30 times is a waste.
It also would be nice to store
the Z value at the same time. This should be
a simple command, right? By
the way I know this isn't a SC question but I
know you guys\gals can help
me out.
Lee Greer
CNC\CAD programmer
Midwest Precision Tool
& Die
|
