Fanuc post

[mpmcnc]

We recently purchased an OKk HM4 with a Fanuc control and I am trying to get teh post set but I am new seting up posts so I am looking for some help. I am using the genaric fanuc mastercam post and here is how my progam post out.

 

%

O0

(PROGRAM NAME - 123 )

(DATE=DD-MM-YY - 18-04-07 TIME=HH:MM - 20:55 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

( 1/2 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .5 )

N104 T1 M6

N106 G0 G90 G54 X-3.25 Y-3.25 S4500 M3

N108 G43 H1 Z2.

N110 Z.225

N112 G1 Z0. F10.

N114 Y3.25 F75.

N116 X3.25

N118 Y-3.25

N120 X-3.25

N122 G0 Z2.

N124 M5

N126 G91 G28 Z0.

N128 M30

%

 

 

And I need it to look like this.

 

%

:123

(PROGRAM NAME - 123 )

(DATE=DD-MM-YY - 18-04-07 TIME=HH:MM - 20:55 )

N100 G20

N102 G0 G17 G40 G49 G80 G90

( 1/2 FLAT ENDMILL TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .5 )

N104 T1 M6

N106 G0 G90 G54 X-3.25 Y-3.25 S4500 M3

N108 G43 H1 Z2.

N110 Z.225

N112 G1 Z0. F10.

N114 Y3.25 F75.

N116 X3.25

N118 Y-3.25

N120 X-3.25

N122 G0 Z2.

N124 M5

N126 G91 G28 Z0.

N128 M30

%

 

Where the two zeros are at the start of the program I need to have a colan and then the program number put in that line.

 

Any help is much appreciated.

[Randy Morton @ Clem Industrial]

I am sorry to hear you bought an Okk...haha Just jokes. We have about 8 of the in the shop, 7 verticals and 1 horiz.

 

Basically, all you want changed is the program number start? If that's it, you can do search in the post for

code:

---

fmt  O  7   progno$      #Program number

---

and change the O to a :. With the number you have to go into the setup for that job and change the number (can't remember the name off hand, but it's in the same window with Stock Setup, but one tab to the left at the top).

 

And if you have already got your program toolpathed, you will need to check all your toolpaths (green check) and then right click, edit common, and change program number to reflect what you need.

 

HTH =]

[mpmcnc]

I have several lines that are like that do I just change the first one? And will that put the : in front of it?

 

#Move comment (pound) to output colon with program numbers

fmt O 7 progno$ #Program number

#fmt ":" 7 progno$ #Program number

fmt O 7 main_prg_no$ #Program number

#fmt ":" 7 main_prg_no$ #Program number

fmt O 7 sub_prg_no$ #Program number

 

Thanks.

[3rdstring]

Change this

 

quote:

---

#Move comment (pound) to output colon with program numbers

fmt O 7 progno$ #Program number

#fmt ":" 7 progno$ #Program number

fmt O 7 main_prg_no$ #Program number

#fmt ":" 7 main_prg_no$ #Program number

fmt O 7 sub_prg_no$ #Program number

---

to this

 

#Move comment (pound) to output colon with program numbers

#fmt O 7 progno$ #Program number

fmt ":" 7 progno$ #Program number

#fmt O 7 main_prg_no$ #Program number

fmt ":" 7 main_prg_no$ #Program number

#fmt O 7 sub_prg_no$ #Program number

fmt ":" 7 sub_prg_no$ #Program number

 

HTH

[mpmcnc]

I changed those settings and now it posted out like this.

 

%

:0000(115)

(DATE=DD-MM-YY - 18-04-07 TIME=HH:MM - 23:14)

(MCX FILE - T)

(NC FILE - H:115.NC)

(MATERIAL - ALUMINUM INCH - 2024)

( T1 | 3/8 FLAT ENDMILL | H1 )

N100 G20

N110 G0 G17 G40 G49 G80 G90

N120 T1 M6

N130 G0 G90 G54 X-2.6875 Y-2.5 A90. S3500 M3

N140 G43 H1 Z2. M8

N150 Z.1

 

 

Im not sure if the four zeros and the parenthesis are going to matter. I wont be able to try it on the machine until tommorow.

 

Thanks for the help.

[Randy Morton @ Clem Industrial]

Kinda looks to me like the (115) is taking the place of your program name. From the MPFAN.PST this is what I read;

 

code:

---

"%", e$

*progno$, e$

"(PROGRAM NAME - ", sprogname$, ")", e$

---

If you happen to take out the e$ after the *progno$ then it would put your program name on the same line as your program number. Your program name can be edited in the same way I outlined above, but instead of changing the the prog. #, change the NC file name. That is what will output when you post, and I would wonder if you changed that by accident instead of the program # to get that output.

[Matthew]

Right click on your operations, select "Edit Selected Operations" then "Change Program #"

[mpmcnc]

I changed the post to match that and now it looks like this.

 

"%", e$

sav_spc = spaces$

spaces$ = 0

*progno$, e$ sopen_prn, sprogname$, sclose_ prn, e$

#sopen_prn, "(PROGRAM NAME - ", sprogname$, ")", e$ sclose_prn, e$

 

 

now when i post out a program it put the program number in the next line like this.

 

%

:0000

(115

(DATE=DD-MM-YY - 19-04-07 TIME=HH:MM - 15:40)