Fusion 360 - Lathe Post ??

I'm leaning Fusion and started poking at LinuxCNC posts for the lathe. I built a 1/4" rod in Fusion and asked for a 1/4-20 threading operation. I ran this with two posts, one for LinuxCNC Turn and one for Tormach Slant Bed. The Post(s) aren't too long and came out like this:

%
(POST_LATHE)
G7                               (Lathe Diameter Mode)
G18                             (Z/X Plane)
G90                             (Absolute Distance Mode)
G20                             (Inch Units)
(G54                            Tormach - working coordinate)
(G40                            Tormach - cutter compensation OFF)
G53 G0 X0.                 (Rapid to machine X=0 : Post Option or G28)
G53 G0 Z0.                 (Rapid to machine Z=0 : Post Option or G28)
                                     (also Post Options for X only, Z only, etc)
(G30                             Tormach uses G30 rather than G53 - same unless G30.1 used to set X&Z)

(THREAD1)
T1 M6                           (Load tool #1)
(N10 T0100                  Tormach uses this for tool ????)
G54                               (Use work coordinate 54)
M7                                 (Mist coolant ON)
G97 S500 M3               (Spindle RPM Mode, Speed = 5500, Start spindle clockwise)
G95                               (Units/Revolution activated, ERROR IF NEW FEED RATE IS NOT SPECIFIED)
G90 G0 X0.65 Z0.2      (Absolute Dist Mode, Rapid move to X and Z - Safe X and Z)
G0 Z0.2123                  (Rapid move to Z - start point for thread control line)
(                                     Tormach moves X before Z)

                                      (Canned Cycle - 1/4-20 thread - looks OK)
G76 P0.05 Z-1. I-0.4 J0.016 K0.08 R2. Q29. H0. E0.04 L0
(                                    Tormach doesn't include H, E or L - maybe cuz they are zero in this case?)
                                     (Post Option for end taper L1, L2 and L3 - haven't tried)

G0 X0.65 Z0.2             (Rapid to Safe X and Z)

M9                                (coolant OFF)
M5                                (Spindel STOP)
G53 G0 X0.                  (Rapid to machine X=0)
G53 G0 Z0.                  (Rapid to machine Z=0)
(G30                             Tormach again uses G30)
M30                              (Program End)
%

My main question regards the G95 which turns on "Units per Revolution" Mode. I don't think this is needed for G76 threading and can't see why it is included. Does G95 only affect cutting moves like G1? Does it affect G2 and G3? The documentation indicates the G95 requires a new feed F declaration, but that may only show up upon a G1 move? I have not tried loading this G-code into a LinuxCNC controller yet.

What scares me is there is no reset before ending the program. There is no G94 to reset the mode to "Units per Minute". I can easily see executing an MDI "G1 Z-1 F4" and having the machine take off at 4 inches per revolution. Very exciting but undesirable.

Is anyone using the Fusion Posts for LinuxCNC lathe?

Thank you for any insight.

Hugh

if you have a program like notepad ++ and have a post processor that is close but not quite what you are looking for you can get inside of the post processor and tweak it in to what you need. you can actually change quite a bit of stuff inside the post processor with a program like notepad ++

so to add a little more you could alter the ending block of the post processor to add the G94 to the code it spits out. if that's what you are looking for? i'm more of a mill guy but have been using fusion 360 for a while now. you can save a copy of your post to your desktop and direct fusion to use that copy to post your programs from.

it seems to be a simple enough fix if that is the only concern?

machinedude:

Thank you for the response. I've done some hacks (too crude to be called mods) to my Fusion milling post. I've heard a programming editor (java script?) will ease modifying these posts but I, like you, are just using an generic editor (Emacs).

But it's not the physical editing of the post. It's more why the G95 is there at all. I don't think the threading cycle G76 requires it. But both LinuxCNC turn and Tormach Slant Bed posts output the same thing. I'd like to know what it does here, or get confirmation that I can removed it without ill effects. I thought someone here would have this insight.

When I get time I'll have to run some tests using more that just a threading cycle. Maybe a threading and then straight turning. See what the code does about G95 and G94.

Thanks for the help.

Hugh

Strongly suggest you go on youtube, search for NYCCNC, and check out his post processor video(s).  He has one where he demonstrates Visual Studio Code and some g-code / F360 plugins used for editing post processors.

The massive win is that you can have a code file and the post processor open side-by-side, and when you select a part of the gcode, the plugin will show exactly what part of the post generated it.

Makes reverse-engineering and editing posts so much easier it's like cheating.

I'm using Fusion lathe for LinuxCNC and when I generate a threading operation it uses G33 rather than G76 (see below). You might stick to the LinuxCNC puzzle initially, rather than confuse matters by using 2 different post processors, despite the fact they both use LinuxCNC. Clearly Tormach saw fit to create their own flavour of post.

Confusingly, G95 seems to be a bit of a minority sport - it's normally a milling command, so not sure what is happening here. You will notice that my Fusion / LinuxCNC / G33 results also show a G95 but there is no feedrate given. I have to wonder what the originator of the G95 command in LinuxCNC had in mind and also have to suspect the documentation isn't accurate when it talks about feedrate required.

The free Visual Studio Code is available in both Windows and Linux and has excellent plugins for Javascript and specific Fusion post editing (look on the Autodesk site). You can even test out post processors from within it and the syntax highlighting plugins are very useful.

%
(8880)
(THREADING TRIAL)
N10 G7
N11 G18
N12 G90
N13 G21
N14 G53 G0 X0.
N15 G53 G0 Z0.

(THREAD1)
N16 T0 M6
N18 G54
N19 G97 S500 M3
N20 G95
N21 G90 G0 X22.7 Z10.306
N22 G0 X10.939
N23 G33 Z-19.246 K2.
N24 X11.833 Z-19.694 K2.828
N25 G0 X22.7
N26 Z10.204
N27 X10.569
N28 G33 Z-19.164 K2.
N29 X11.833 Z-19.796 K2.828
N30 G0 X22.7
N31 Z10.125
N32 X10.284
N33 G33 Z-19.1 K2.
N34 X11.833 Z-19.875 K2.828
N35 G0 X22.7
N36 Z10.059
N37 X10.045
N38 G33 Z-19.047 K2.
N39 X11.833 Z-19.941 K2.828
N40 G0 X22.7
N41 Z10.
N42 X9.833
N43 G33 Z-19. K2.
N44 X11.833 Z-20. K2.828
N45 G0 X22.7
N46 Z10.
N47 X9.833
N48 G33 Z-19. K2.
N49 X11.833 Z-20. K2.828
N50 G0 X22.7

N51 M5
N52 G53 G0 X0.
N53 G53 G0 Z0.
N54 M30
%

The G97 drops you into rpm mode, essentially turning off G96 (CSS) if that was programmed earlier and follows G95 maybe by default or because it was selected? 
I think you can delete it or leave it. Looks like some of my old threading programs have it also. 
I would do a dry run and see what happens. The G53 and G30 is what I would be cautious about. I think Tormach uses G30 as the turret return position prior to a tool change. I would delete it unless you know exactly where that is on your machine. On my lathe it would rapid to the machine Z home position away from the chuck.

spumco:

NYCNC is where I saw the editor. Muzzer says it's Virtual Studio Code. I hate Windows and have only relented to a dual boot with Linux to run Fusion. But Mizzer says it's available for Linux also. Having the editor and source code linked would be a great help in Post work, even if I had to do it under Windows. I'll have to get a copy.

Thank you.

Hugh

Muzzer:

I'd bet that Fusion LinuxCNC Post uses G33 if you don't check "canned cycle" and uses G76 if you do.

Using the two Posts I just wanted to see if Tormach also called G95. I was surprised that the two codes are nearly identical. Tormach seems to use G30, rather than G53 G0, and lists a lot more documentation. like a tool list. I suspect Tormach was written from the LinuxCNC Post.

My only thought regarding G95 and feed rate is the error would be thrown at the first G1 move. There are none here so it should be OK. But without a resetting G94 I think it could be trouble.

I will get a copy of Visual Studio and try it out for Posts. Thank you.

Thanks.

Hugh