In your 9000 program you have a G53. I thought it was basically the same as
G28.
I've never used G53, what is it, and how is it used?
Bob.
Mike Sharp
<[EMAIL PROTECTED]> To: "Smartcam Users Group
Sent by: ([EMAIL PROTECTED])"
[EMAIL PROTECTED] <[EMAIL PROTECTED]>
i.sdrc.com cc:
Subject: RE: [mfg-smartcam] Haas
tool change
question
09/02/03 10:45 AM
I do the same as Michael, except I also have a sub for tool change for tall
parts. It moves the machine to the X & Y referance position. For regular
tool change I use program 8500, for tool change that needs extra clearance
I
use program, 9000. These are the programs I use for the Fanuc's.
%
O9000 (TOOL CHANGE CLEAR MOVE)
N10 G00 G91 G28 Z0. M05
N20 M01
N30 G90 G00 G17 G40 G49 G80 G98
N40 G90 G53 X-40.0 Y0
N50 M06
N60 M99
O8500 (TOOL CHANGE CYCLE)
N10 G00 G91 G28 Z0.0 M05
N20 M01
N30 G90 G00 G17 G40 G49 G80 G98
N40 M06
N50 M99
Mike
-----Original Message-----
From: Michael Senack [mailto:[EMAIL PROTECTED]
Sent: Tuesday, September 02, 2003 7:16 AM
To: [EMAIL PROTECTED]; [EMAIL PROTECTED];
[EMAIL PROTECTED]
Subject: RE: [mfg-smartcam] Haas tool change question
This is all foggy now as I have not programmed Fanucs for a while. But as
best as I can recall without looking through old archive documentation,
when
I programmed the 6M/10M Fanuc Controls I assigned an 8000 series program to
do the tool change/reset everything.
The 8000 series programs had to have a parameter turned on
to edit them. This meant the operator could see the program
but not edit it.
The program looked similar to this sample
%
:8013( RESET PROGRAM )
M09M05( spindle and coolant off )
G90G00G80G20G94( absolute , rapid , cancel can cycle , inches , ipm )
G28G91Z0.0 ( retract spindle on z axis to its tool change home position
)
G40G90G99G49 ( CDC off, absolute, retract to R , cancel tool length? ) M01(
optional stop ) M99
%
These controls allowed us to assign a g-gode to call this program. I used a
G13 code to retract the spindle, and reset everything.
Why? It was easy for the operator to use. If they were in the
middle of a cut and needed to stop the machine all they had to
do was switch to MDI and enter G13 and press cycle start.
Also programming a G13 code to do four or five lines of code are a lot
easier to remember and less error prone.
-----Original Message-----
From: [EMAIL PROTECTED]
[mailto:[EMAIL PROTECTED]
Sent: Tuesday, September 02, 2003 8:41 AM
To: [EMAIL PROTECTED]; [EMAIL PROTECTED]
Subject: RE: [mfg-smartcam] Haas tool change question
Rob,
I am not familiar with Haas machines, though its my understanding that the
controls are Fanuc "compatible" (please correct me if I'm wrong.) I know
that with a Fanuc control equipped with Macro B, you can write a Fanuc
macro
which would be called in place of the standard M06 tool change command.
Said
Macro could check the machine position and move to a "safe" tool change
position before executing the M06 command. This Macro would be assigned
within the Fanuc parameter settings to replace the standard tool change
command. The downside is that this macro will be active all the time unless
you physically change the parameter back to its original setting.
I bring this up because if your Hass control has the same capability, you
may be able to write something similar to address your problem.
Regards,
Chris Kocourek
Flextronics CTC
-----Original Message-----
From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]
Sent: Friday, August 29, 2003 4:27 PM
To: [EMAIL PROTECTED]
Subject: [mfg-smartcam] Haas tool change question
We work with tall fixtures on large angle plates on a Haas VF2 mill. The
tool change level is about 4" lower than the highest point of the spindle
travel. The G91 G28 Z0 line takes the spindle to tool change level, and
sometimes this isn't high enough to clear the fixture.
My question is this:
Does anyone know another code, or some other way to have the spindle go all
the way up?
I am currently adding lines at the machine like: G00 G90 G54 Z8.0
(depending
on where part Z zero is) to take the spindle as high as possible, but this
changes with each program and setup.
Thanks,
Bob.
Robert T. Callahan
Greene, Tweed & Co.
CNC Programmer
Corporate Manufacturing
[EMAIL PROTECTED]
215-256-9521 ext. 1569
======================================================================
To find out more about this mailing list including how to unsubscribe, send
the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
======================================================================
To find out more about this mailing list including how to unsubscribe, send
the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
======================================================================
To find out more about this mailing list including how to unsubscribe, send
the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
======================================================================
To find out more about this mailing list including how to unsubscribe,
send the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
======================================================================
To find out more about this mailing list including how to unsubscribe,
send the message "info mfg-smartcam" to [EMAIL PROTECTED]
======================================================================
