Postprocessor for FANUC 0T

[spotlite]

Hello,

I am using the standart FANUC TURNINC post processor for my old CNC lathe with FANUC 0T.

Already figured out how to get rid of "G54" command (it is not supported by FANUC 0T).

The only problem now is drilling as the fanuc do not support G8x commands, drillings must use G7x commands (G74), etc.

Can not find suitable post processor for it.

PLEASE ANYONE - HELP!  🙂

[LibertyMachine]

Please post the following:

1) What the code is spitting out that is not acceptable

2) The same code edited to run on your machine

[engineguy · Accepted solution]

@spotlite

All I could find in the Help files was a "workaround" for this as it was a known issue at the time, it seems that changing the "capabilities" settings as per the following link will get your PP to output G7* numbers instead of the G8* ones you are getting. Don`t know if a proper "fix" has been done for it but apparently this does work

Original line is :- capabilities = CAPABILITY_TURNING;

Try changing to :- capabilities = CAPABILITY_MILLING|CAPABILITY_TURNING;

Here is the link to the original workaround solution :-

http://help.autodesk.com/view/fusion360/ENU/?caas=caas/discussion/t5/Fusion-360-Computer-Aided-Machi...

Sorry, that`s all I have, Seth will know if there is a proper "fix"

Regards

Rob

[spotlite]

OK I modified that, but now I have another error:

Error: Command START_SUB_SPINDLE_CW is not defined.

Hmmm....

[spotlite]

In fact I cannot get proper output from the post processor as it refers drilling as milling operation.

[engineguy]

@spotlite

Try the attached modified PP, it seems to work reasonably well here, probably needs some more tweaking for your use (It still has G54) it is the latest Fanuc PP I could find in the online Library.

Regards

Rob

[engineguy · Accepted solution]

@spotlite

Not sure if the Machine selection might be causing this error, I have a simple 2 Axis Lathe that I use so maybe if you haven`t already done that and are using a "Generic Mill/Turn" or another one from the Library that is also a Mill/Turn Machine then it might be worth creating a simple 2 Axis Lathe that uses all the dimensions/travels/feeds/speeds that your actual Lathe uses, might help, I only have a simple 2 Axis Lathe so I created one in Fusion right from the start !!

Works OK for me !!

Regards

Rob

[spotlite]

OK, post processor generates the following code:

%
O1001
N10 G98 G18
N11 G21
N12 G50 S6000
N13 G28 U0.

(DRILL5)
N14 T0303
N15 M8
N16 G98
N17 G97 S2000 M3
N18 G0 X-0.582 Z45.
N19 G0
N20 Z35.
N21 G73 X-0.582 Z14.5 R34.5 Q4.125 F100.
N22 G80
N23 Z45.

N24 M9
N25 G28 U0. W0.
N26 M30
%

When run on FANUC 0T, it stops at line N21 with FANUC error code P/S 07 (Illegal use of decimal point).

[engineguy]

@spotlite

Code seems a bit odd to me, unless you have driven tools and are drilling a hole off centre then I would expect your X value should be X0 not X-0.582, check the position of your hole in your drawing.

Usually it is the "-" that is throwing the error so if you re-check the hole position and get an X0 position then it is possible the alarm will be cleared.

I am not at my workshop so don`t have access to my old Fanuc manuals so that`s the best I can offer you for now, won`t be able to get to the shop for a couple of days now, sorry that`s all I have for now !!

Regards

Rob

[spotlite]

   OK, here is what happens:

Fanuc Turning post processor generated following for chip breaking cycle:

G73 X0. Z14.5 R34.5 Q4.125 F100.

But I need to edit this to:

G74 R1         //this value goes not export  anywhere?? Should come from chip break parameter in CAM

G74 X0. Z14.5 Q4125 F100.

Could you edit the post processor for me, please?

[engineguy]

@spotlite

Sorry for the delay getting back to you but I have been trying to get the PP configured to output the Fanuc two line canned cycle without much success I am afraid, it needs someone with a lot more knowledge of the PP than I currently have.

I have got it to output the G74 and not have the R* value on the same line but so far I have not been able to get it to generate the Q value correctly or the first G74 R* line, here is a sample of the canned cycle code it currently generates :-

%
O1112
N10 G98 G18
N11 G20
N12 G50 S6000
N13 G28 U0.

(DRILL CHIP BREAK)
N14 T0101
N15 M8
N16 G98
N17 G97 S2000 M3
N18 G0 X0. Z0.45
N19 G0 Z0.2
N20 G74 Z-0.5751 Q0.0625 F8.
N21 G80
N22 Z0.45

N23 M9
N24 G28 U0. W0.
N25 M30
%

@LibertyMachine  Seth, I think this needs to be passed up to the PP Developement people or someone with a lot more experience than me!!

@spotlite However (There is always a however) the PP seems to be very "broken" as I have come across a very weird and horrible workaround, if I select "Dwell before Retract" and set a time of 0.25 seconds under the "Cycle" Tab the the PP outputs the drilling cycle as straight code with what appears to be all the correct feeds/rapids required  to drill the hole!!

Here is the same hole as the above canned cycle but with the Dwell, very, very weird but at least the hole could be drilled !!

%
O1112
N10 G98 G18
N11 G20
N12 G50 S6000
N13 G28 U0.

(DRILL CHIP BREAK)
N14 T0101
N15 M8
N16 G98
N17 G97 S2000 M3
N18 G0 X0. Z0.45
N19 G0 Z0.2
N20 Z0.08
N21 G1 Z-0.0625 F8.
N22 G0 Z-0.06
N23 G1 Z-0.125 F8.
N24 G0 Z-0.1225
N25 G1 Z-0.1875 F8.
N26 G0 Z-0.185
N27 G1 Z-0.25 F8.
N28 G0 Z-0.2475
N29 G1 Z-0.3125 F8.
N30 G0 Z-0.31
N31 G1 Z-0.375 F8.
N32 G0 Z-0.3725
N33 G1 Z-0.4375 F8.
N34 G0 Z-0.435
N35 G1 Z-0.5 F8.
N36 G0 Z-0.4975
N37 G1 Z-0.5625 F8.
N38 G0 Z-0.56
N39 G1 Z-0.5751 F8.
N40 G4 P250.
N41 G0 Z0.2
N42 Z0.45

N43 M9
N44 G28 U0. W0.
N45 M30
%

Fusion file and PP used attached as well.

Once again sorry I haven`t been able to solve this for you properly.

Hope you get a solution and please let us all know if you do get one as we all need the help !!

Best regards

Rob

[jluck001]

It has been a while, but has anyone got a working post processor for the Fanuc 0T? We have a Nakamura lathe that has a 0T but have found no working post processor.

Thanks,

Justin

[seth.madore]

The generic Fanuc turning post is going to be your best bet, and then edit it to suit your needs.