Fanuc SubPrograms

[TheePres]

Question for the Fanuc Gurus;

Is it possible to incorporate a subprogram into main body, as done on FADAL type programs. As opposed to seperate programs??

[DavidB]

Yes it can.

Main program calls a subprogram or subprograms by M198 followed by program number. In the subprogram the end of program has a M99 which takes it back to the main.

 

HTH

[Jerosu]

Ya, you could use a "Goto" macro statement if you wanted I guess. Then a block number for your "subprogram" which wouldn't be a subprogram really, just a different section of the main program. Sort of a bunch of leapfrogging if I understand your question correctly.

[Tim Simmermon]

We do that with our Haas machines, it works the same. I haven't tried tweaking it in MCam yet. Mcam posts the subprogram in the same file, but it gives it a program # (O####). I change the O to a N, and the subprogram callout from M97 to M98 or vise versa (can't remember which one is a local call).

[Guest CNC Apps Guy 1]

The problem with GOTO is it searches the entire program. If you use a DO/WHILE it goes much faster. Then you could have certain conditions so that if you want to have a section of code run a certain number of times, set a counter and say WHILE[#100LE#500]DO1 etc....

Like so;

 

#517=0

#122=3.

#123=120.

#112=15.

#113=-.75

#102=1.

#103=1.

IF[#122GT 1.]THEN#122=1.

IF[#112GT 15.]THEN#112= 15.

IF[#102GT 1.]THEN#102= 1.

 

#121=1

#124=#14004

WHILE[#121LE#122]DO1

 

#111=1

#114=#14002

WHILE[#111LE#112]DO2

 

#101=1

#104=#14001

WHILE[#101LE#102]DO3

 

#517=#517+1

#115=#14003

X#104Y#114B#124

 

#101=#101+1

#104=#104+#103

END3

 

#111=#111+1

#114=#114+#113

END2

 

#121=#121+1

#124=#124+#123

END1

[tryon]

Fanuc needs to fix/add this to the controls. Local sub program calls are the shiz. Mazak,Yasnak i80m,Fadal,Haas can all do this.

[g huns]

Do it every day on my 16m. M98 calls subprogram, M198 calls subprogram from data-server. I load programs into data-server, O1001, O1002, O1003 and so on. Have a control program in memory that just says

M198 P1001

M30

M198 P1002

....

Works the same in memory, just gotta have way smaller programs.

[DavidB]

quote:

---

M198 P1001

M30

M198 P1002

---

Remove the M30

[heavychevy2155]

M97 is the local subs the P word looks for the N number in your program. If you use this on a horizontal, like at the end of the program use a m98 to call another sub for the other pallet. You can run it to nesting problems if you do not use a m30 at the end. There is probably away around this, just havent took much time to find the answer.

[g huns]

I use the M30(stop, rewind) cause most often I just load one program at a time, run it on all my parts, the load the next one. Helps keep meh head staight.

[tryon]

I have always considered a local sub program as residing in the main program. The subs are contained after the M30. So you can use subs all you want and you only load one program. As Tim explained its pretty easy to setup your post for this, doing just as he said.

 

ex.

%

O100;

;

;

T1M6(SPOT)

G0G90G54X0Y0M3S500

G43H1Z2.0

G99G81Z-2.5R.25F100.K0

M98H90(jumps to line N99)

G80(returns here after M99)

G0G91G28Z0

M1

;

;

T2M6(DRILL)

G0G90G54X0Y0M3S1000

G43H2Z2.0

G99G83Z-25.R.25F134.K0

M98H90(jumps to line N99)

G80(returns here after M99)

G0G91G28Z0

M30

;

;

N99(HOLE POSITION SUB)

X0Y0

X35.

Y20.

X50.Y50.

M99

;

;

%

[TheePres]

Tryon,

For which control does your example work on?

and would it not be M97 instead of M98, also others mention "P" as block number search, youre example uses "H".

 

James,

Im sure youre method would do job quite nicely, but you lose me quickly at mention of macros.

[tryon]

That example is for a mazak. If you leave the "P" out of the "M98H99" it will search for N99 in the program calling the sub. Leaving out the "P" is what makes it a local sub call. Fanucs cant do it simply.

[robk]

Been doing it for years. Sample from our horizontal;

quote:

---

%

O1000(MAIN-PROG.SUB.100 )

G0G17G40G80G90

G0G91G28Z0.

G0G91G28X0.Y0.

G90G53X0.Y0.Z0.

G91G30XYZ0.

M1

N1G0G90G54

M11

B0.

M10

M98P100

M1

N2G0G90G55

M11

B0.

M10

M98P100

etc...

etc...

etc...

---

[DC Gorn]

Anyone know any good books on Macro Programming? After seeing James code it reminds me of the old basic I did back in high school. I have avoided Macro so far but I feel like its time.

[Lars Christensen]

DC Gorn,

 

I just got my company to buy me this book.

 

Macro book

 

(Thanks to jmparis for posting that URL back in day)

 

I have read it, and been taking some notes, seems like a good starting point. However James and the other macro people we have here has to be aware, that the minute I can break into our horizontal, that I am going to have alot of questions for them.

 

Lars

[Guest CNC Apps Guy 1]

Here's a Simple Snippet.

 

G10

#148=1 (RESET OFFSET COUNTER)

#124=0 (RESET B COUNTER)

#526= 1. (NUMBER OF INDEX'S IN

#527= 120. (B INDEX AMOUNT)

#528= 1. (NUMBER OF PARTS IN X)

#529= 1. (X STEP AMOUNT)

#530= 15. (NUMBER OF PARTS IN Y)

#531= -.75 (Y STEP AMOUNT)

IF[#530GT 15.]THEN#530= 15.(Y STEP MAX SAFETY)

G11

 

N39

T1039M06 (T1039 - 1MM PROBE TIP - 1 FLUTES - )

#148=1

(CHECK CURRENT TOOL OFFSET)

#101=#[10000+#506]

IF[#101LE3.0]GOTO99999

T1001

#148=1

WHILE[#148LE#517]DO1

M11

B0.

G00G54.1P#148G90X0.Y0.S500

G43H99Z2.

M10

G54.1P#148

Z.5

(***** SET XY BORE ZERO *****)

G65P9800R-0.S.375W54.1V#148Z-.2I0.J0.

Z2.

M11

#148=#148+1

END1

G52 X0 Y0 Z0 B0M09

G28 G91 Z0 M219

G30 G91X0 Y0

G49

M01

 

This one will make as many parts as you need in X, Y, and/or as well as B. Each part has it's own offset. Pretty small footprint, and won't change in size if I want to add parts. One caveat, the parts need to be fixed spacing distances in X, Y, and B. I'm certainly not a MACRO guru but I do like them for their power, and I've incorporated them into several posts so I do not need to use and keep track of sub programs which can be a chore.

 

James teh Sub H8r

[Psychomill]

Hmmm .... Half of us are "one page" and the other half is on another page of this book.

 

Theepres is looking to do internal subbing, NOT external (like M98 or M198).

 

The answer for FANUC (as some have mentioned here) is NO. There are some work arounds but not quite as effective. I use a lot of "While/Do"s like James mentioned. You can use "GOTO" but as he also mentioned, this causes the control to seek the file from the top. If the program is long and/or the control is slow, this will actually "pause" the machine until it finds it.

 

Another way is to use "M99P???" with a counter set in variable, but this has the same effect as a GOTO when its used in the "main body" of the program.

 

Haas has M97, Mazaks M98H?? .. Yep, Fanuc needs to add this to their stuff.