If you set parameter 3401 BIT 0 (DPI) to a 1 then you can input numbers like a calculator.
X5000 will be taken as 5000mm
If you set parameter 3401 BIT 0 (DPI) to a 0 then your numbers will be taken as microns..
X5000 will be taken as X5 (in other words 5000 microns you would need to program X5000. to get 5000mm
X5000000 would also work
This should make it work. If it doesn’t then maybe you should call the Samaritans.
Decimal Point Fanuc Parameter Why?
It doesn’t really matter how you set this it’s entirely up to you. What I would recommend is that you make all your CNC machines behave in the same way.
Teach everyone to always input a decimal point and then if it’s needed then you got it.
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) G90 (Absolute) G0 G53 X0 (Return X To Tool change Position) G53 Z0 (Return Z To Tool Change Position) (Any Old Shit You Want to Do) M99
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.
The Bonus
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.
