Unusual threading

[rdshear]

I have a very unique situation. We have a VTL that the owners retrofitted with a Heidenhain Mill control. I have successfully converted a lathe/mill post to run every aspect of the machine except one. That is threading. While the machine does thread, it is a VERY crude process. This is accomplished by changing the start point of each pass to "step off" the thread profile.

 

Here is some sample code from a thread I cut a little over a year ago.

 

code:

---

7  ; KENNAMETAL BUTTON TOOL 

8 ; #A3SSR200626 WITH

9 ; #A3R218106P00DF INSERT

10 ; .218 DIA BUTTON TOOL

11 ; TAUGHT ON X AND Y AT THE C/L

12 ; OF THE BUTTON.

13 ;

14 TOOL CALL 4 Y S45

15 L M3

16 ; Q1 = THREAD PITCH

17 ; Q3 = X DATUM SHIFT AMOUNT

18 ; Q4 = Y DATUM SHIFT AMOUNT

19 FN 0: Q1 = +0.94488

20 FN 0: Q3 = +0.48

21 FN 0: Q4 = +0

22 ;

23 ; LABEL 1 WILL STEP OFF AT A 45

24 ; DEG

25 ; ANGLE USING DATUM SHIFTS TO

26 ; CHANGE THE X/Y POSITION.

27 ; THIS LABEL IS USED TO ROUGH THE

28 ; THREAD PRIOR TO THE FINISH

29 ; PASSES

30 ; NOTE: ALL TOOLPATHS ARE AT THE

31 ; C/L

32 ; OF THE BUTTON TOOL.

33 ;

34 LBL 1

35 L M3

36 ; SHIFT THE AMOUNT NEEDED

37 CYCL DEF 7.0 DATUM SHIFT

38 CYCL DEF 7.1 X+Q3

39 CYCL DEF 7.2 Y+Q4

40 ; GO TO SETUP POSITION

41 L X+16 Y+1 R0 F MAX

42 ; X OVER TO C/L OF THE RADIUS

43 ; OF THE ROOT OF THE THREAD

44 L X+15.3217 R0 F MAX

45 ; SYNCHRONIZE CHUCK AND TURRET

46 L M50

47 ; MAKE PASS ON THREAD

48 CYCL DEF 18.0 THREAD CUTTING

49 CYCL DEF 18.1 DEPTH -8.625

50 CYCL DEF 18.2 PITCH +Q1

51 CYCL CALL

52 ; PULL OUT

53 L X+16 R0 F MAX

54 ; DECREMENT X AND Y

55 FN 2: Q3 = +Q3 - +0.1

56 FN 1: Q4 = +Q4 + +0.1

57 ; IF Y IS BELOW OR AT ZERO LINE

58 ; RUN

59 ; AGAIN

60 ; OTHERWISE CLEAR DATUM SHIFTS

61 ; AND EXIT

62 ; LABEL

63 FN 12: IF +Q4 LT +0 GOTO LBL 1

64 FN 9: IF +Q4 EQU +0 GOTO LBL 1

65 CYCL DEF 7.0 DATUM SHIFT

66 CYCL DEF 7.1 X+0

67 CYCL DEF 7.2 Y+0

68 LBL 0

---

This code was hand written as I'm sure you noticed. What it essentially does is change the start point of the cut, sychronise the chuck with the infeed, and make a pass. I then manually program the pull out, and move back up.

 

Also, if you are looking at the code, think of 'Y' as 'Z'.

 

My question is:

 

Is there any way to get Mastercam to automatically change a start point and repeat a cycle to achieve something similar?

 

As you can imagine, we do very little threading on that machine. But I have another job with 22" dia square threads 1/2" pitch I have to program. I know this won't be the last time either. If I can figure out how to get MC to do the work for me it would be great.

 

Thanks in advance for any help you can give,

 

Rick

[rdshear]

Much simplified, here is what I need to figure out at minimum for each pass.

 

code:

---

1  L X+16 Y+1 R0 F MAX

2 ; X TO CUTTING RADIUS

3 ; AT THE ROOT OF THE THREAD

4 L X+15.3217 R0 F MAX

5 ; SYNCHRONIZE CHUCK AND TURRET

6 L M50

7 ; MAKE PASS ON THREAD

8 CYCL DEF 18.0 THREAD CUTTING

9 CYCL DEF 18.1 DEPTH -8.625

0 CYCL DEF 18.2 PITCH .5

1 CYCL CALL

2 ; PULL OUT

3 L X+16 R0 F MAX

4 L Y+1 R0 F MAX

---

The only thing that would change pass to pass is the 'Y' ('Z') at line 1 and the 'X' at line 4.

 

Is this even possible through Mastercam or is it something I'll have to live with manually programming?

[crazy^millman]

I would think you could create a custom drill cycle to do this with very little problem. You might could do this with a threading cycle out of Mastercam, but think it would be some work in the post to get it right, but possible.

 

HTH

[rdshear]

I had thought of a custom drill cycle. If I'm thinking right, I'd have to "drill" each point (start location) and maybe use some of the drill paramaters to pass the threading depth and pitch?

 

The only downside I see to that method (assuming I could get it to work )is the number of points I would have to create and MC not knowing the type of tool. It would have to think it was a drill for a drill cycle (right)??

 

Ideally, a custom groove would be nice. I thought of maybe setting a misc-int to direct a manual groove to a custom thread cycle. That way MC would generate the start point (possibly) and the tool type could be accurately defined ??

 

Is my thought process correct on those??

 

I will most likely have to do this job by hand but I would love to come up with a way to make this process easier.

 

I'm the only programmer in the shop who programs for this machine. So it's kinda my baby. So far I've been pleased with what I've made it do... This is really my last big hurdle.

[Matthew]

Have you tried using "longhand" for the thread cycle insted of the "canned" cycle? I use this all the time and it steps the starting forward slightly each pass. This is under 'thread cut parameters' in the 'nc code format' drop down menu.

[rdshear]

I haven't tried that. Does that only work for 'V' shaped threads or will it work with buttres and square threads as well?