Fusion 360 post processor no longer prompting for tool change?

I’ve used the Carbide 3D post processor in Fusion 360 as long as I’ve had my Shapeoko 4. Up until last week, one of the first lines written to the NC output was a “Txxx M6” command. Now, it’s just an M0, then a spindle enablement. Totally bypassing the tool change (though there is a comment inserted about the tool change).

I’ve fixed the post processor myself locally, but curious if anyone else has has this issue?

I don’t use Carbide’s post processor, but I just tried it. It output the M6 for me. Looks like it was modified less than a week ago…is yours up to date?

On the same line? I didn’t think their post ever had inline comments.

Can you share what you modified?

1 Like

Seems I’ve got auto-updates enabled, not pinned to a version:

  $Revision: 44056 1b59ebd6e1654e97374d41a72521d80afdfb4ddc $
  $Date: 2023-03-13 13:57:35 $

Any chance the 2023-03-13 rev modified this? I don’t think I modified any tools, setups or machine configurations in Fusion 360.

 

Anyways, here’s the first few lines of output without my modification:

(Nut Slot)
M0
(MANUAL TOOL CHANGE TO T102)
S18000 M3

I added the onCommand(COMMAND_LOAD_TOOL); in the writeToolCall method of the post processor:

function writeToolCall(tool, insertToolCall) {
  writeStartBlocks(insertToolCall, function () {
    if (!retracted) {
      writeRetract(Z);
    }
    if (!isFirstSection() && insertToolCall) {
      forceWorkPlane();
      onCommand(COMMAND_COOLANT_OFF); // turn off coolant on tool change
      if (typeof disableLengthCompensation == "function") {
        disableLengthCompensation(false);
      }
    }

    if (tool.manualToolChange) {
      onCommand(COMMAND_STOP);
      onCommand(COMMAND_LOAD_TOOL); // Added by me
      writeComment("MANUAL TOOL CHANGE TO T" + toolFormat.format(tool.number));
    } else {
      if (!isFirstSection() && getProperty("optionalStop") && insertToolCall) {
        onCommand(COMMAND_OPTIONAL_STOP);
      }
      onCommand(COMMAND_LOAD_TOOL);
    }
  });
}

New output (though I guess the M0 is unnecessary, at least I get my tool change):

(Nut Slot)
M0
T102 M6
(MANUAL TOOL CHANGE TO T102)
S18000 M3

I confirmed my older .nc files contained that Txxx M6, thought they did not contain that comment (MANUAL TOOL CHANGE TO Txxx).

Edit: It definitely seems like the 3/13/2023 rev has a significant diff versus the old version:

03/13/2023 vs 04/21/2022

The tool.manualToolChange is a parameter set in your tool editor. It’s just a checkbox. If you uncheck it, you’ll get the correct output.
(this is in the Edit Tool dialog)

4 Likes

Thanks for the response. Confirmed that things look better without that checked, though it’s a bit misleading :smile:.

I’m guessing I was working around this on the previous rev of the post processor, but the latest version now requires that box to be unchecked to work correctly. I certainly haven’t updated all my tools to manual tool change = true anytime recently.

1 Like

So just to be clear, if I uncheck the box labeled “Manual tool change”… it will force Motion to ask me to manually change the tool?
I haven’t looked as deep as going into the line by line gcode, but I just recently had the same problem, I believe, and Motion displays “MANUAL TOOL CHANGE TO Twhatever” next to the Status line when I try to run a program I just created.

I exported five NC programs this morning. Of the five, four display a preview in Motion without a tool, but one of them does correctly show the tool. Three of those four, plus the correct one, are all using the exact same tool. When I edit any of my tools, they all have “Manual tool change” and “Live tool” checked; I haven’t changed it myself.

Before you changed this, did Motion also skip measuring the tool? And after you unchecked the box, did it behave as you expected and were used to; that is “insert tool blah blah” and then measures it and then runs the cut file?

Yes, I’ve always had my tools setup with “Manual Tool Change Required” (in my head that makes sense comparing the Shapeoko to a CNC with an automatic tool changer).

Pretty clear that the latest post-processor breaks the long existing model of how this works, I’ve since gone and unchecked that box for all my tools.

1 Like

That’s the weirdest thing. I guess Fusion thinks of the Shapeoko asking automatically for a tool change counts as an “automatic tool change”…whatever. I don’t have to understand it.

Thanks to you and @neilferreri both.

I don’t know how long you guys have been around here, but tool changes are much more “automatic” than they used to be. I’d say most people did anything they could to avoid them. The discussions then used to revolve around whether it was worth it to spring for the limit switch upgrade when that became available. Well, that and pulley set screws.
Really all this comes down to is whether that M6 is included. That’s the way tool changes are automatic.

1 Like

Sure, I don’t disagree that my idea of “Manual Tool Change” was wrong. But this type of change is pretty breaking and I’d imagine would catch more than a few newer users off guard.

This topic was automatically closed after 30 days. New replies are no longer allowed.