G Code Alias Fanuc Parameter 6050
Category : Fanuc
Messing With Parameters Can Be Fatal!!!!!
G Code Alias Fanuc Parameter, to change this parameters you need to go to the setting screen in MDI.
Put a 1 in the parameter write box.
Today children we are going to change the parameter that allows us to alias a G code to a 9000 series program.
G Code Alias Fanuc Parameter
So for example if you were to put 384 in parameter 6050 then if you program G384 you would be directed to program 9010. (See the list below the program)
09010 (G384 Macro)
M9 (Turn off Coolant)
M5 (Stop Spindle)
G40 (Cancel Cutter Compensation)
G80 (Cancel Canned Cycle)
G0 G53 X0 (Return X To Tool change Position)
G53 Z0 (Return Z To Tool Change Position)
(Any Old Shit You Want to Do)
So when you program G384 in MDI or from a program it jumps into program 9010 and does all that lot.
Parameter 6050 is the G code for program 9010
Parameter 6051 is the G code for program 9011
Parameter 6052 is the G code for program 9012
Parameter 6053 is the G code for program 9013
Parameter 6054 is the G code for program 9014
Parameter 6055 is the G code for program 9015
Parameter 6056 is the G code for program 9016
Parameter 6057 is the G code for program 9017
Parameter 6058 is the G code for program 9018
Parameter 6059 is the G code for program 9019
There is just no end to the stuff you can do with this.
I’m not telling you anymore cos I need the work and probably couldn’t handle the competition. This bloke seems to know more than me about all this macro shit so go and visit him.
Don’t come crying back to me cos I wont have you on my site again.
Because you didn’t go I’ll tell you more….
You can alias programs to M codes and G codes.
Whats the difference?
When you alias a G code you get to pass parameters to it.
It’s like when you call a canned cycle for example when you call G81
G81 R1. Z-10. F100.
This would tell the machine to drill a hole 10mm deep. Well that Z figure of -10 is a parameter being passed to the cycle.
So when you program a special G code that jumps into a 9000 series program you can send information with letters.
With an M code sadly you can’t
Some More Interesting Parameters
3202 Unlock Program 9000 to 9999 and 8000 to 8999 to Edit
3401 Calculator Type Decimal Point or Integer
6005 Allows the Use of Local Subroutines (Newer Control)
6050-6059 Allows you to Call a 9000 series Program with a G Code
6080-6089 Allows you to Call a 9000 series Program with An M Code
3291 Wear Offset requires Key to Adjust
8134 3453 allows you to use ,R and ,C (Rads and Chamfers)
That’s it away you go.
Oh just one other thing before you go off and cripple your machine forever.
Do yourself a favor take a picture of the screen before you change a parameter. If you aint got a camera then you must have a piece of paper.
Even better back everything up.
If you have been affected by any of the issues in this post or need CNC Counselling then contact me.
If you want to learn to program CNC Milling Machines
Look no further Contact CNC Training Centre
Leave a Reply