Fanuc Turning Post Processor G code Errors

[lethal375]

I recently purchased a CNC lathe with Fanuc 21it control

My first attempts to run programs using the Fusion 360 Fanuc turning post processor have resulted in numerous G Code errors 

There are many G codes in the program that are not in the machine manual and not supported.

Am I using the wrong processor? 

[KrupalVala]

Hi @lethal375 ,

May I know, are you using generic Post processor or not? 

You can find latest and greatest Post Processor from our Post Library.

Click on following links,

• Post Library for Autodesk Fusion 360
• FANUC Turning

Thanks,

[lethal375]

I used the "Fanuc Turning/fanuc turning" from the drop down list.

Did not go to the "Library"  

[KrupalVala]

Hi @lethal375 ,

Could you tell me what error you are getting?

Thanks

[lethal375]

Alarm "010 Improper G-CODE"

%
O1002 (PIN2)
N10 G98 G18
N11 G20
N12 G50 S4000
N13 G28 U0.

(PROFILE ROUGHING1)
N14 T0100
N15 G54
N16 M8
N17 G99
N18 G97 S337 M3
N19 G0 X6.8 Z0.1969
N20 G50 S4000
N21 G96 S600 M3
N22 G0 Z0.05
N23 X5.8
N24 G1 Z-3.2315 F0.01
N25 X6.
N26 X6.08 Z-3.1915
N27 G0 Z0.05
N28 X5.6
N29 G1 Z-3.2315 F0.01
N30 X5.8
N31 X5.88 Z-3.1915
N32 G0 Z0.05
N33 X5.4
N34 G1 Z-3.2315 F0.01
N35 X5.6
N36 X5.68 Z-3.1915
N37 G0 Z0.05
N38 X5.2
N39 G1 Z-3.2315 F0.01
N40 X5.4
N41 X5.48 Z-3.1915
N42 G0 Z0.05
N43 X5.
N44 G1 Z-3.2315 F0.01

Here is the beginning of the program

Will not even start the program

Get alarm as soon as I hit cycle start

Last night I deleted some of the G codes in the beginning of the program that I felt were not required and it would start to run the program then same alarm would pop up.

Not at machine and cant remember what I deleted but I think it was G18,98,99  

These G codes are not listed in the manual 

[lethal375]

Just tried running the program in single block mode

G50 is definitly a problem

Eliminated the entire line N12 G50 S4000

Got it to run AUTO through the first roughing cycle

When it got to the finishing cycle that G50 S4000 stopped it agian

G50 is not in my machine manual and after researching it I found a listing that shows G50 as COMPENSATION "RESET ALL SCALE FACTORS TO 1.0" 

[lethal375 · Accepted solution]

I believe I have the G50 issue solved

While researching G codes for 21iT there was reference to model type A,B, & C

All indications are that mine is type B

I opened the processor file and line #52 was set to A 

Changed Line #52 type to B and saved

Ran post processor again and G50 is now gone 

I will try running the program on lathe tommorow

[KrupalVala]

Hi @lethal375 ,

You can directly choose/change "Type" as "B"  from Post-Properties.  

If you select Type-A then only Post will print the G50 with the maximum spindle speed.

Thanks,

[lethal375]

Thanks

That is much easier 

There is no mention of the different  "Types" and or need to select the correct one?

Only stumbled upon mention of it when researching 21iT alarm and G codes.