Actually, In your second example you could execute the G54 line of code,
then manually move the Y axis to near where the tool broke, move the
cursor to the G01Z-0.1 line and go from there (providing you can turn
the coolant on and the feed rate wasn't cleared by reset, if that's not
the case you would have to MDI a M08 F38.0, then {mem} {cycle start} ).
Although if you had cutter comp on in that move, no dice.
In the first example I think I would edit the missing info on the X 6.5
line, execute up to the G54 block (inclusive) then {edit} cursor to the
X6.5 line then {mem} {cycle start}.
J.G.
-----Original Message-----
From: Michael Senack [mailto:[EMAIL PROTECTED]]
Sent: Thursday, August 03, 2000 3:16 PM
To: 'Milling Precision Tool'; Jim Mivshek; [EMAIL PROTECTED]
Subject: RE: [mfg-smartcam] Start point.
We have a Hurco mill with an OM Fanuc control. Here is a sample of code
for
tapping...
N50M98P1
T05( 1/2-13 TAP )
G54G43X2.5Y-11.5Z2.0S91H05M03
G99G84Z-1.5F7.0R0.5M08
X3.5Y-11.5
X4.5Y-11.5
X5.5Y-11.5
X6.5Y-11.5 <-- lets say the tap breaks here
X7.5Y-11.5
X8.5Y-11.5
X9.5Y-11.5
X10.5Y-11.5
According to what your saying I would execute from N50 to the first X &
Y
position in single block WITHOUT the tap in the tap holder. Then I would
stop the machine, go into edit, move to X6.5Y-11.5 line, put the tap
back in
the tap holder, go to run mode and single block this line and IF
everything
went okay take single block off, and press start run button and run the
rest
of the program.
Is what I just said above sound like a good game plan?
Here is a mill sample from the same program...
N100M98P1
T08( 3/4 ROUGH SANDVIK CARBIDE E/M )
G54G43X1.5Y-12.575Z2.0S2546H08M03
G00Z0.1
M08
G01Z-0.05F38. <- 1st pass up the center of the slot
Y0.2
G41X1.025D38
Y-12.575
X1.975
Y0.2
G40X1.6
G00Z0.1 <- clear part
X1.5Y-12.575
G01Z-0.1
Y0.2 <- 2nd pass up the center of the slot and tool breaks half way
G41X1.025
Y-12.575
X1.975
Y0.2
G40X1.6
Using what you said how do you get the e/m to z-.1 depth at the
beginning of
the Y0.2 line without going through the 1st pass ?
-----Original Message-----
From: Milling Precision Tool [mailto:[EMAIL PROTECTED]]
Sent: Thursday, August 03, 2000 2:08 PM
To: Jim Mivshek; [EMAIL PROTECTED]
Subject: Re: [mfg-smartcam] Start point.
I have started in the middle of a program several times.
It
works best for
me on a Fanuc control. Scan through the program to find
where you need to
restart and wright down the line N number or put a N
number
there. Start
the program running in single block mode. Single block
through the
beginning of the program until you load the tool and
execute
the tool
length and spindle speed comands. Some times I will let
the
control execute
the first position move then I will put the control in
manual mode and
search through the program to the N number line in the
program that has an
X & Y location move of where I want to restart at. Put
the
control back in
run mode and push start and single block through a few
lines
to make sure
everything is alright. Take off single block and off you
GO.
Some times it
takes a little work but I have had good luck this way.
Play
around with
this method with the tool removed to see if it will work
for
you.
Good Luck.
At 07:55 AM 8/3/00 -0500, you wrote:
>If have a run time of 2 hours and my cutter snaps at
1.5
hours into it how
>can I start again at the point of breakage.
>I have tried starting in the middle of progam before
without success.
>
>I believe it needs to see the header code to know
cutter
comp, fixture
>offsets, feeds, speeds ect.
>How can I do this...
>
>Thanks
>Jim M. "Cherry Corp"
>
>======================================================================
>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]
======================================================================
