Fusion 360 - EMC Post ?

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!

Hello

I have do last week the same things : allowing G43 with ATC, imo this is a no sense to use G43 only with manual tool change.

But you can do other way and use a remap for add the G43 with all M6 command.

At many point the original fusion 360 postpro for linuxcnc is really confusing (using G28 for retract produce G28 U. W. with lathe post pro)

Br

Muzzer: The code I posted at the top of this thread is for milling. I used the "Enhanced Machine Controller (EMC) / emc" and the "Autodesk Generic 3-axis" for the machine. It gave the above result whether the machine used an automatic tool changer or not. (Although I haven't tried the manual tool change in the tool library.) The variable "outputG43OnSeparateLine" isn't present in the LinuxCNC milling post.

In my other thread about turning I used "Autodesk Generic Mill-Turn Lathe" and "LinuxCNC turning". Due to your response I noticed that the code in that thread has no G43 commands. I found that when you post NC code, where you select the machine, these's an option to "Edit" the machine. You can select whether it has an automatic tool changer or not. However this has no effect on the NC code. The G43 commands are still missing.

I finally figured out where you pointed to to select a manual tool change in the tool library. After this change I started to get G43 commands. It does include a pause M0 though. Not optimum because my LinuxCNC is set up for manual change and also pauses for tool change. But this will be easy to change if need be.

How did you ever figure out this was in the tool library? Congratulations. I'd have never stumbled upon this. Thank you.

It is scary. Checking the manual box in the tool selection is something I'd likely forget. Another reason to set up a solid/fixed tool crib for the lathe. Or more likely, change the post to always give G43 on tool changes.

Thanks.

Hugh