Material stop for lathe

[BillB]

Does Intercon and or CNC12 have an a way to place the tool in position to a desired z depth a material hard stop at the end of the code to reset the stock length?

Im using M55 for GO to X0, Z0 so this would work as a hard stop option but would be good to have it backed off a bit in X in case there is a nipple at the end of the stock left over.

IF not would be a great addition.

[cncsnw]

Just insert a "Line" move, in Rapid mode, to whatever X and Z coordinates, and with whatever tool number you need.

If you need the program to pause there while you advance the material, then insert an "M&G Code" operation with an M0.

If you want the program to just end there (stopping the spindle and leaving the carriage where it sits), then insert an "M&G Code" operation with an M99.

[suntravel]

Thats how I use material stop, for making multiple parts from a bar with a manual chuck:

Code: Select all

; --- Cutoff Cycle ---
N0002 T0400 
  M9
  G96 S120.0 M3
  G4 P1.0
  G0 X20.2 Z-15.0 T0404
  G1 X20.0 Z-15.0 G99 F0.07
  X19.0 Z-15.0 
  G0 X20.2 Z-15.0 
  X20.2 Z-14.5 
  G1 X20.0 Z-14.5 
  X20.0 Z-14.5 
  X19.0 Z-15.0 
  X19.0 Z-15.0 
  G0 X20.2 Z-15.0 
  G1 X20.0 Z-15.0 
  G75 R0.1
  G75 X-0.5 Z-15.0 P20.0 Q0.0 R0.0
  G0 X20.2 Z-15.0 
; Pull bar for next part
  M5
  G0 Z0.2
  X16
  M200"Pull bar and close chuck\nCycle Start to continue"
; --- End of Program ---
N0003  Z2.0 
  G28 T0400
  M5
  M9
  G40
; End of Program

Uwe

[BillB]

Thanks Uwe,

I like the added notation in the control, IS the M200 what calls this up? I would like to add something like that.

I got this code from Karl at Sherline, I got it working its so cool!! however had to omit (M6) as it was hanging up there. I looked at the list of CNC12 M Codes and there is NO M6 for tool change on the list. WHY is this?

(Bills Edited Version)
T26 (M6)
M05
G90 G00 X0.150
Z.010
M00
(feed the stock out)
G90 G00 Z1.0
X1.0
M03 S2500 (whatever rpm you are using for the next tool)
(Start the program again)

[BillB]

Can I add this to my program right inside of Intercon as I program a part using Insert F3, Other F10 G&MF2 code?

[suntravel]

Can I add this to my program right inside of Intercon as I program a part using Insert F3, Other F10 G&MF2 code?

sure

M200 stops the program, shows text between " " till you hit cycle start again.

Work through the lathe manual, it is very well explained.

Uwe

[BillB]

I want to paste this into Intercon, right in software instead of having to paste into the code text file? I see insert G&M code but it seams to only allow one line at a time? Every time you edit the CAM you need to Re-paste into the text file its a PIA. ; ( Can I do this?

(Bills Edited Version For pasting into Files)
T26 (M6)
M05
G90 G00 X0.150
Z.010
M00
M200 "Feed Stock Out, Clamp Chuck, Hit Cycle Start : )"
G90 G00 Z1.0
X1.0
M03 S2500 (whatever rpm you are using for the next tool)
(Start the program again)

[tblough]

You could save that as a subprogram and call it using M98. That way you only have to enter a single line using the Intercon G&M code insert.

Another way would be to make a macro using an unused M code and call it. That would be even shorter than typing M98 "programname.cnc"

[BillB]

You could save that as a subprogram and call it using M98. That way you only have to enter a single line using the Intercon G&M code insert.

Another way would be to make a macro using an unused M code and call it. That would be even shorter than typing M98 "programname.cnc"

OH that is awesome! thanks for the input.

For the M98, do I create a text file and reference it somehow to M98? can you give me the basics of how I would set that up?

Same question for the 2nd option, they both sound like good ways to do it.

[tblough]

Both are explained in the manual.