maximum subprogram nesting levels?

[Jody]

What is maximum subprogram nesting levels? and how do I find out what I can put there and why?

 

Thanks

Jody

[Guest]

That info should be in your controls manual.

 

On my Fanuc 16i's I can go 4 levels deep.

[Guest CNC Apps Guy 1]

Most controls have a limit to the "depth" that you can go in Sub Programs. Usually it's 4.

 

O1

M98P111

M30

 

O111(LEVEL1)

M98P222

M99

 

O222(LEVEL2)

M98P333

M99

 

O333(LEVEL3)

M98P444

M99

 

O444(LEVEL4)

DO SOMETHING

M99

 

If in program 444 you had another sub call, you'd get an alarm.

 

HTH

[Jody]

What does 4 levels deep mean? We have a HAAS VM3. I will go get the book and see if it will tell me.

 

thank you

 

Jody

[Jody]

Oh so you can only call 4 subprograms in the actual program?

 

Jody

[EZ3PUTT]

4 levels deep mean that the main program calls up a subprogram, which in turn calls another subprogram etc. 4 times.

[Jody]

Wait that is not what you mean. you are saying that you can right a program then a subprogram in the program then a subsubprogram in the subprogram......

 

that is it! I think

 

 

Thank you

 

Jody

[Guest CNC Apps Guy 1]

Yes Jody. You got it. Going more than 1 or 2 deep gets dicey though when you go to troubleshoot something. The deeper you go in subs the harder it is to trace "issues".

[Jody]

Ok how and why would you need to do that? and do you have MC do that or is that something that you write manually?

 

Thanks John, James and EZ

[Guest CNC Apps Guy 1]

That would be something you'd do manually and honestly I do not know what would posess someone to do that in all honesty. I'm a KIS guy myself. (Keep It Simple) Mastercam goes 1 deep. Main, Sub, back to main.

[Tim Johnson]

I go three deep every day and four deep about 10% - 15% of the time. Here's one I wrote today. (three deep)

 

main level;

code:

---

G91 G30 X0 Y0 Z0

M06 T32 (4.60MM COOLANT THROUGH CARBIDE DRILL)

#930=4010

T40

M[#926]

M[#925]

M[#927]

M98P5002 (<<<<<<<<<<<<<)

M09

M56

M58

M05

G91 G30 X0 Y0 Z0

M01

---

1 level deep

code:

---

O5002 (1 SIDE FRONT FOR CLUSTER VISES 8 PARTS)

#900=[#903-1] (-START FRONT SIDE BOTTOM 0-)

M98P[#930+3] (-RUN FRONT SIDE BOTTOM 0-)

IF[#909LT2]GOTO103(END TOOL)

M98P[#930+4] (-RUN FRONT SIDE TOP 0-) (<<<<<<<<)

IF[#909LT3]GOTO103(END TOOL)

G00 Z[#919] (RETRACT)(-END FRONT 0-)

M98P[#930+3] (-RUN FRONT SIDE BOTTOM 90-)

IF[#909LT4]GOTO103(END TOOL)

M98P[#930+4] (-RUN FRONT SIDE TOP 90-)

IF[#909LT5]GOTO103(END TOOL)

G00 Z[#919] (RETRACT)(-END FRONT 90-)

M98P[#930+3] (-RUN FRONT SIDE BOTTOM 180-)

IF[#909LT6]GOTO103(END TOOL)

M98P[#930+4] (-RUN FRONT SIDE TOP 180-)

IF[#909LT7]GOTO103(END TOOL)

G00 Z[#919] (RETRACT)(-END FRONT 180-)

M98P[#930+3] (-RUN FRONT SIDE BOTTOM 270-)

IF[#909LT8]GOTO103(END TOOL)

M98P[#930+4] (-RUN FRONT SIDE TOP 270-)

N103 G00 Z[#919] (RETRACT)(-END TOOL-)

M99

---

2 levels deep

code:

---

O4014

N0140 G90 G00 X0 Y0 G54P[#4130+1]

N0150 G68 X0 Y0 R180.

N0160 M98 P4013 (<<<<<<<<<<<<<<<<<<)

N0170 G69

N0180 M99

---

3 levels deep

code:

---

O4013

(4.60MM COOLANT THROUGH CARBIDE DRILL)

N0010 #919=6.

N0020 #900=[#900+1]

N0030 G00 G90 X2.3 Y-.38 (B0.) B0. G54P[#900]

N0040 G43 H32 Z.375 S1687 M[#933]

N0050 Z.225

N0060 G99 G81 Z-.083 R.225 F4.16

N0070 X1.8

N0080 X1.3

N0090 X.8

N0100 X.3

N0110 G80

N0120 G00 Z.375

N0130 M99

---

My post writes it all

[Guest CNC Apps Guy 1]

 

Different strokes for different folks.

[Roger Peterson]

Subs are useful, nested subs are useful. With todays controllers where memory is not an issue you only really need to do it if you think you may need to do online edits. I like using subs for repetative work, in subs I do call other subs but only for drill locations because it is so nice to edit one sub with locations for all the drill toolpaths. Other instances may be for overriding a G10 work offset position, a probe cycle, or some engraving, a short warmup routine to go to a much higher spindle speed (this is usually done automatically now), etc....

 

HTH

[Guest CNC Apps Guy 1]

In many probing/tool breakage detection macros they go a couple subs deep so you have to be careful you're not exceeding the max number.

[tryon]

I believe if you call your subs with G65 you can go deeper than 4. You dont need to pass arguments with G65 it just allows you to. I dont think i have ever went past 4 myself.

[Guest CNC Apps Guy 1]

Interesting...

[Psychomill]

Many of us know that you can nest up to 4 levels (Fanuc) with a M98... This is from the Fanuc manual:

 

" Calls can be nested to a depth of four levels including simple calls (G65) and modal calls (G66). This does not include subprogram calls (M98). "

 

Is this to say that you can go 7 or 8 levels deep? So from the 4th level M98, you can macro call to a sub, then go 3 more levels from there?

 

I'm with James though... KIS or KISS....

The Haas book doesn't say how deep you can nest. At least I've never found it. But with M97 available, why bother unless you have "common" subs for different parts.

Mazaks can nest to 8 levels.