Tool with no SPEED or M3

[mr801]

Is there a way to make it so that a tool doesn't post out a speed and M3? I am using point toolpath for probing and Misc Int. for the probing cycles.

[Guyinthedesert]

Is there a way to make it so that a tool doesn't post out a speed and M3? I am using point toolpath for probing and Misc Int. for the probing cycles.

 

I know when forget to input a spindle speed, it'll post out S0M5

[Bryan Johnson]

Yes.

If tool number is constant, you could key off that and setup post to skip the output anytime that tool number is used.

[K2csq7]

I use point toolpaths for TLO checks. My posts output the speed but M05 instead of M03 or M04. If you want it I'd be happy to help, lathe or mill? What kind of post are you using?

I use a unique feedrate to trigger it in the mill post, and the lathe post gets triggered by a misc. integer. (the mill post can be easily changed to become triggered by a misc integer).

[MIL-TFP-41]

Like Bryan said, as long as your probe is always the same tool number (which is a good idea anyways) it is easy to do. see here.... http://www.emastercam.com/board/index.php?showtopic=62775&st=0&p=705872&hl=probe&fromsearch=1entry705872

[neurosis]

I put a 0 spindle speed for our probe and it posts out S0 M5. I was concerned about this when we first started using the probe but it has never been an issue. Of course I always double check to make sure!

[mr801]

Here is what I get:

 

14 L Z-.1 B+0 R0 F MAX M91

15 L X+0 Y+23.5 R0 F MAX M91

16 PLANE RESET STAY

17 L B+Q121 C+Q122 F MAX

18 ;TOOLPLANE NAME - TOP

19 ;MAX - Z+1

20 ;MIN - Z+1

21 * - TOUCH PROBE

22 TOOL CALL 150 Z S0

23 M5

24 L Z-.1 R0 F MAX M91

25 L X+0 Y+23.5 R0 F MAX M91

26 CYCL DEF 247 DATUM SETTING ~

Q339=0 ;DATUM NUMBER

27 CYCL DEF 7.0 DATUM SHIFT

28 CYCL DEF 7.1 X+0

29 CYCL DEF 7.2 Y+0

30 CYCL DEF 7.3 Z+0

31 CYCL DEF 32.0 TOLERANCE

32 CYCL DEF 32.1 T0.001

33 CYCL DEF 32.2 HSC-MODE:1

34 PLANE RESET STAY

35 L X+0 Y+0 F MAX M8

36 L B+Q121 F MAX

37 L C+Q122 F MAX

38 L Z+1 F MAX

39 TCH PROBE 412 DATUM INSIDE CIRCLE ~

40 Q321=+0; CENTER IN 1ST AXIS ~

41 Q322=+0; CENTER IN 2ND AXIS ~

42 Q262=+0.5; NOMINAL DIAMETER ~

43 Q325=+45; STARTING ANGLE ~

44 Q247=+90; STEPPING ANGLE ~

45 Q261=-.25; MEASURING HEIGHT ~

46 Q320=+0; SET-UP CLEARANCE ~

47 Q260=+1; CLEARANCE HEIGHT ~

48 Q301=+1; MOVE TO CLEARANCE ~

49 Q305=+0; NUMBER IN TABLE ~

50 Q331=+0; DATUM ~

51 Q332=+0; DATUM ~

52 Q303=+1; MEAS. VALUE TRANSFER ~

53 Q381=+0; PROBE IN TS AXIS ~

54 Q382=+0; 1ST CO. FOR TS AXIS ~

55 Q383=+0; 2ND CO. FOR TS AXIS ~

56 Q384=+0; 3RD CO. FOR TS AXIS ~

57 Q333=+0; DATUM ~

58 Q423=+4; COMPENSATION

 

This is what I want:

 

14 L Z-.1 B+0 R0 F MAX M91

15 L X+0 Y+23.5 R0 F MAX M91

16 PLANE RESET STAY

17 L B+Q121 C+Q122 F MAX

18 ;TOOLPLANE NAME - TOP

19 ;MAX - Z+1

20 ;MIN - Z+1

21 * - TOUCH PROBE

22 TOOL CALL 150 Z

24 L Z-.1 R0 F MAX M91

25 L X+0 Y+23.5 R0 F MAX M91

26 CYCL DEF 247 DATUM SETTING ~

Q339=0 ;DATUM NUMBER

27 CYCL DEF 7.0 DATUM SHIFT

28 CYCL DEF 7.1 X+0

29 CYCL DEF 7.2 Y+0

30 CYCL DEF 7.3 Z+0

31 CYCL DEF 32.0 TOLERANCE

32 CYCL DEF 32.1 T0.001

33 CYCL DEF 32.2 HSC-MODE:1

34 PLANE RESET STAY

35 L X+0 Y+0 F MAX M8

36 L B+Q121 F MAX

37 L C+Q122 F MAX

38 L Z+1 F MAX

39 TCH PROBE 412 DATUM INSIDE CIRCLE ~

40 Q321=+0; CENTER IN 1ST AXIS ~

41 Q322=+0; CENTER IN 2ND AXIS ~

42 Q262=+0.5; NOMINAL DIAMETER ~

43 Q325=+45; STARTING ANGLE ~

44 Q247=+90; STEPPING ANGLE ~

45 Q261=-.25; MEASURING HEIGHT ~

46 Q320=+0; SET-UP CLEARANCE ~

47 Q260=+1; CLEARANCE HEIGHT ~

48 Q301=+1; MOVE TO CLEARANCE ~

49 Q305=+0; NUMBER IN TABLE ~

50 Q331=+0; DATUM ~

51 Q332=+0; DATUM ~

52 Q303=+1; MEAS. VALUE TRANSFER ~

53 Q381=+0; PROBE IN TS AXIS ~

54 Q382=+0; 1ST CO. FOR TS AXIS ~

55 Q383=+0; 2ND CO. FOR TS AXIS ~

56 Q384=+0; 3RD CO. FOR TS AXIS ~

57 Q333=+0; DATUM ~

58 Q423=+4; COMPENSATION

 

What code would you put in the post for tool 150 to make it post out without the speed(S0) or M3 or M5? I always use tool 150 for my probing.

[Nils N]

I do the same as Neurosis, works great

[mr801]

I was hoping that I could do it with a S0/M5 but it alarms my machine.

[MIL-TFP-41]

You should be able to modify your post using very similar arguments from my above post. Basically (or exactly) you are telling your post that if the tool number is = to 150, then don't output that stuff. A quick glance at your code...looks like you have your speed callout and your spindle on callout on different lines....so they would be on different lines of your post. so you would add something like this to your "Tool Call" Line

blah blah blah ( if not( t$ = 150 ), *speed ), e$

 

and on your next line (Line 23)

 

blah blah blah ( if not ( t$ = 150 ), *spindle ), e$

 

 

[edit]

 

changed syntax

[Tim Johnson]

Here's how I turn the spindle off for probes;

 

      if virt_tlplnno = 2 | virt_tlplnno = 5 | virt_tlplnno = 6, n$, *sgcode,
      *sgabsinc, pfxout, pfyout, "(", no_spc$, pfcout, no_spc$, ")",
      [if (machine = 60 & t$ = 59) | (machine = 80 & t$ = 4), "M19"], e$
      if t$ <> tlngno$, result = mprint(stoollengthwarn)
     if (machine = 60 & t$ = 59) | (machine = 80 & t$ = 4), n$, "G43",
      *tlngno$, pfzout, e$
     else, n$, "G43", *tlngno$, pfzout, *speed, *spindle, e$