Fusion 360 - EMC Post ?

I'm trying to learn Fusion 360. I have a start on this but am by no means competent. I've tried to post a small part to G-code using the LinuxCNC (EMC) post processor. On a tool change I get this command:

G43 Z0.06 H1

or similar. There is a modal G0 above this which applies to the Z move? I've been too scared to try in on the machine. Would this command even work, with the Z0.06 embedded? When will the Z0.06 move happen, before or after the tool length comp? The Z0.06 moves to clearance height over the part, so the intent is to apply G43 first. Very confusion, or I'm missing something.

I spent a day leaning enough about the Fusion Post to hack a change to this. Even if this command works it's confusing to me. On my post the G43 is on a line above the Z move.

Does anyone know of a "better" LinuxCNC post for Fusion 360 milling? How is their Post for LinuxCNC turning?

Thank you for any insight.

Hugh

You might need to include a little more of the gcode before, including and after the tool change.  I'm struggling to picture what you are referring to.
I use a copy of the standard linuxcnc postprocessor in Fusion360 on my mill.

Sorry. I was mostly interested in that particular command line. But some more context would have been good.

This is a test part with a simple circular pocket (1/2" end mill) with a chamfer around it's top (1/2" spot drill). I don't think it'll matter much to the code, but I selected Autodesk's Generic 3D milling machine. For a post I used the EMC2 milling post from the Autodesk library. There is another post, just EMC, which I didn't try.

The program preamble and first tool change are as:

(POST-TEST-STOCK)
(MACHINE)
(  VENDOR AUTODESK)
(  DESCRIPTION GENERIC 3-AXIS)
(T1  D=0.5 CR=0. - ZMIN=-0.5 - FLAT END MILL)
(T20  D=0.5 CR=0. TAPER=90DEG - ZMIN=-0.2 - COUNTERSINK)
G90 G94 G17 G91.1
G20
G53 G0 Z0.
(2D POCKET2)
T1 M6
S7639 M3
G54
M8
G0 X0.465 Y-0.0681
G43 Z0.6 H1
G0 Z0.2
G1 Z0.15 F126.06
S7640
X0.4654 Y-0.0669 Z0.1391
.........
Hugh

It's not executing G43 then Z0.6 then H1. G43 requires the corresponding H1 offset to be specified on the same line and will apply it to the Z0.6 move if you specify it on the same line. You could instead write G43 H1 on one line, then the Z0.6 on a subsequent line.

Short answer is yes, the H1 offset will be applied to the Z0.6. 

You should get a copy of one of Peter Smid's books which explain the common G and M codes and show how they should be used. I prefer "CNC Control Setup for Milling and Turning" although the more commonly referred to one is "CNC Programming Handbook (3rd Edition)". Other references are available online but Smid's books are a good place to start.

Muzzer:

I think of G43 H1 as one command. I'm surprised the Z0.6 intermixed is OK. Sounds like it follows the rules though. I studied the LinuxCNC documentation and it didn't answer either question.

I hacked my Post to output two lines which is much easier for me to read:
G43 H1
Z0.06

I thought I had a book by Smid but don't now see it on the shelf. Must have lost it during the last move. The LinuxCNC documents and forum have answered all my questions until this came up.

Thank you for the insight.

Hugh

Andy:

Thanks for the note. Good to know it works, but it is weird.

Thanks.

Hugh

This is weird and puzzling. I've just posted a file with a roughing operation followed by a threading operation. These use different tools and the post has called for the new tool (change from T4 to T6) but there's no G43 to be seen. The LinuxCNC documentation seems to be expecting a G43 on a tool change - is there an innocent explanation for this? I'm using the default LinuxCNC post processor from Autodesk (v 43267 from 2021-04-13).

I might have to go inside and drink lots of tea and / or beer the way things are shaping up here!
 

Im with you, the g43 should be there.  Heck it is in the version I run.  I had to edit the PP so it would NOT produce it. My remapped m6 deals with all the tool offset stuff.

you might need to have a look at that version of the PP and see if there is some reason for g43 not being generated.  NYCNC did a good video on how to edit the fusion PP. 

I've done quite a bit of PP editing previously, to create a post for a Chinesium controller. I notice that Hugh (currinh) was getting G43s in his code at the top of this post. No idea what's going on here but perhaps he could compare his PP version and see if we have the same vintage? What about you, Jaco - what version do you have? It's in the header of the post.

Thanks
EDIT - I seem to have bottomed out 2 of those puzzles just now by searching within the post processor.
1:
Firstly I spotted this on the 5th line down:

description = "LinuxCNC Turning";
vendor = "LinuxCNC";
vendorUrl = "www.linuxcnc.org";
longDescription = "Turning post for LinuxCNC. Use Turret 0 for Positional Turret, Turret 101 for QCTP on X- Post, Turret 102 for QCTP on X+ Post, Turret 103 for Gang Tooling on X- Post, Turret 104 for Gang Tooling on X+ Tool Post.";
var outputG43OnSeparateLine = false;
.....

So you can force G43 to be output on its own line. Hopefully that will answer Hugh's question that started this thread. Changing it to true should force a new line for each G43.
2:
Further down, the G43 output is dependent on whether you have a manual toolchange. It is actually specified within the tool library within Fusion, within the setup for the specific tool you are changing to. I have no idea why they reckoned a G43 should only be output for a manual change but it's presumably because an ATC takes care of the offsets.

}
    writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6), conditional(tool.manualToolChange && !outputG43OnSeparateLine, gFormat.format(43)));
    writeBlock(conditional(tool.manualToolChange && outputG43OnSeparateLine, gFormat.format(43)));
    if (tool.comment) {
      writeComment(tool.comment);
    }

Selecting "manual tool change" results in G43s returning. You see - drinking enough tea will fix almost anything!