Build Thread- HOW TO: Make your own MasterCam X Fanuc 6t Post

[KyleH2]

I thought I might give some starting advice to anyone who was searching for what I was. It turned (haha get it?) out to be easy.

I had an Ikegai lathe with a Fanuc 6T-a that I didn't know much about and wanted to program using Mastercam X. I started by creating a new command file called Ikegai based off the generic slant bed 2x file and saving a copy. Also make sure to BACK UP YOUR GENERIC FANUC POST. You can use the Fanuc, MPLFAN, whatever.

Anyway open Generic Fanuc 2X lathe in Notepad youll see a bunch of commented out stuff.

I was currently outputting G54, program names that start with O00XX while my machine used G50 and :00XX for the program name format.

What to do:

Part 1:
Hit ctrl+f for find. Type in old_new_sw
Set your old_new_sw to 0 for the Fanuc 6t

old_new_sw : 0 #Switch old (6T), new (0T+) cycle formats, 0=old, 1=new

Part 2:
Scroll to the top of the document and click anywhere.
Ctrl+f type in home_type youll find a thing that explain mi1 and home_type. Set home_type to your home_type, in my case it was 0
Keep finding instances of home until you come to a number questions list
question 301 will deal with your WCS, set that accordingly. In my case 0 for G50.
Keep finding, you'll find other places mentioning setting an integer (again, 0) to set the post to output G50 instead of G54.

# Following Misc. Integers are used:
#
# mi1 - Work coordinate system: (home_type)
# -1 = Reference return / Tool offset positioning.
# 0 = G50 with the X and Z home positions.
# 1 = X and Z home positions.
# 2 = WCS of G54, G55.... based on Mastercam settings.

home_type : 0 #Flag for type of home location, read from misc. int.

301. Work coordinate (-1=REF, 0=G50, 1=HOME, 2=G54's)? 0

1. "Work Pos. [-1=REF,0=G50,1=HOME,2=G54s]"//0

1. "Work Pos. [-1=REF,0=G50,1=HOME,2=G54s]"//0

Part 3:
Now my post is setup for a Fanuc 6t, to output G50, but the file name still is not correct.

Again scroll to the top and click anywhere to start searching. Hit ctrl+f. Type in program number and search.
Comment out (using the # symbol) the lines that say to use O like 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
fmt U 2 sub_trnsx$ #Rotation point
fmt V 2 sub_trnsy$ #Rotation point
fmt W 2 sub_trnsz$ #Rotation point