Hello Guest it is January 25, 2020, 03:22:43 PM

Author Topic: Mach3 Lathe doesn't stop spindle during tool change.  (Read 3709 times)

0 Members and 1 Guest are viewing this topic.

Mach3 Lathe doesn't stop spindle during tool change.
« on: January 10, 2014, 03:43:28 PM »
I am new at all things Mach3. I just got my lathe conversion going and I am having trouble with the tool change. I found the option in general config under Tool Change to "Stop spindle. Wait for cycle start", and I have that checked.  The lathe will make a move to a tool change position and wait, but the spindle will remain on. The spindle will turn off if I hit the spindle off button on the screen, and in manual cycle an "M5" will shut it off but not when a program gives an M6 T*********x.  I am sure I am missing something please help.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Mach3 Lathe doesn't stop spindle during tool change.
« Reply #1 on: January 10, 2014, 04:03:20 PM »
Tool calls in a lathe are TXXYY where XX is the tool number and YY is the offset. If that is what you are doing then thats ok :)
Now as far as the stop spindle and wait option, I have never used it as I have a turret but I would have thought it would stop for manual tool changes. Can test out tomorrow if I make it to the worksop, and of course if I remember ::)
Other option would be for you to call a M5 just prior to the toolchange call and a M3 after.
Hood
Re: Mach3 Lathe doesn't stop spindle during tool change.
« Reply #2 on: January 10, 2014, 04:30:35 PM »
Hood, thank you for your quick response,  I am currently using the T0101 format to call my tools. I might have found a solution to stop the spindle. I inserted ' Code "M5"' into the bottom of my M6Start.m1s file and it will now turn the spindle off for a tool change.  Is this an acceptable solution? Also would the M6Start.m1s file be where I could put Gcode to move the tool back away from the work for a tool change? Or is there some place else that I am supposed to input the default tool change position?  I currently do not use home switches, I just home the machine at startup and use a master tool to zero out for part position.

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Mach3 Lathe doesn't stop spindle during tool change.
« Reply #3 on: January 10, 2014, 05:38:11 PM »
Yes thats the place you would put any code you wanted to do during a toolchange.
With a turret on a lathe normally you would have the toolchange position defined in the code as each part will be a different length and each tool may be a different length, so defining in code saves unnecessary moves.
Hood

Offline RICH

*
  • *
  •  7,402 7,402
    • View Profile
Re: Mach3 Lathe doesn't stop spindle during tool change.
« Reply #4 on: January 10, 2014, 08:35:42 PM »
Ok on stoping the spindle. I still use the motor switch.

Lots of ways I guess to work  and depends how tool table offsets are done........

I use work offsets along with the manual / quick change tool changer many times.

- I use the master tool to touch off at X&Z=0, then Zero World both axes.
- Then  move to a location that will serve as a tool change and Home location
  So i just move far enough away for the longest tool to clear the work, and the move is an easy, even, convienent, number  say X 2 Z 2.
  At that point I Zero World the X&Z again, and also Set Home for each axis.
- Now in  Part  coord I make a move back to X&Z  and zero the coords which creates a G54  offset for the part

In the gcode for a tool change you can add
G00 X....Z.... to a safe location  / no doubt about it
G28 X....Z.... at  the safe location and goes to home / tool change position
M6 T0303     Tool is changed in mach
G4 P120       ya got 5 miutes to change the tool and ged rid of that flashing indicator

Make sure you go home when program is completed.

CYCLE START and the program continues on

Make sure you go home when program is completed.

So if code is pieced together for a part from wizards etc and   based on X&Z =0 and you want to do another piece along the stock say some distance along the Z.
Just define the Z distance  in Work offsets G55 , MDI G55, rewind and run the same code again.

RICH

Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Mach3 Lathe doesn't stop spindle during tool change.
« Reply #5 on: January 12, 2014, 05:57:11 AM »
I tested this out yesterday on the wee lathe and it does seem Turn will not stop the spindle automatically when you have the Stop Spindle and wait option chosen, so doing it in the macro or code is what you will have to do.
Hood