I am using fusion 360 (latest update) and EX controller.
Everything works well but I am having trouble when a tool change should be directed to the tool height setter however it shows “”Press CYCLE START to continue (jogging enabled)” eg T1 to sayT8
Pressing CYCLE START will lead next to “Spindle About to start. Press Cycle Start” which of course leaded to the gcode running without a tool change.
Pressing MTC will do nothing. Pressing Hold feed then MTC will also do nothing
It’s probably something small I am over looking but any help would be appreciated
The code appears to do what you say, in that M0 pauses, then M3 starts the spindle. There is no automatic tool change (T or M6) in your code. What type of fusion360 license do you have? They only support automatic tool changing in the more expensive licenses (commercial and above IIRC).
The code looks like it expects you to do the tool change manually during the pause, and then hit CYCLE START.
You need to uncheck that setting and run the file again.
I can understand how you arrived at checking this box… the tool change IS a manual tool change, but as far as the controller is concerned it’s automatic, it doesn’t know you broke your wrenches and swapped a tool
That’s what starts a tool change. The letter T is for tool number, so in this case 5. The M6 is the actual script that does the tool change. The M6 is the thing that drives over to your touch plate and asks you to swap the tool.
By setting your tools in your library to manual tool change you’re removed that M6 script, so there’s nothing to walk you through the tool change.
It’s done this way because the M6 script lives on your controller and is unique to it. This way no matter what your setup is, the M6 script can do your tool change for you.
So in your particular case your M6 script it set such that it asks you to break out your wrenches and swap your tool. Those with ATC spindles will have the draw bar activated, and when we release our tool rack with ATC that M6 script will do the tool changes for you.
What this means is that the G code is the exact same no matter what setup you have.
So just to underscore this: Every tool change no matter how it’s done NEEDS that M6 command, so DO NOT check “manual change” in Fusion or you’ll be removing that command.
Sometimes you might not want to use the tool setter and just set the Z offset manually or with the mobile touch plate, a single large surfacing bit for example. In that case all you have to do is comment out or delete the Txx M6 line in the G-code file generated by Vectric or Fusion. Should be quicker than running through the Tool Change prompts.
If you want to manually set your Z offset you can do that manually in the WCS table. There you can key in a Z offset value. Common use case is if you know the thickness of your material already and you don’t want to bother to measure it, you just type it in the Z slot.
As far as measuring tools:
EVERY tool you put in the spindle needs to be measured. No exceptions. This happens during a tool change in a few different ways. Normally this is done off of the tool heigh setter.
If you have a large tool (like a slab flattener) that can’t fit on the tool height setter you have options:
You can use the MTC button, when you enter the diameter if the tool is too large to fit it will give you the option of moving around in XY to get your tool on the setter. This can be useful if you just need to get a wing of a slab flattener on the plate.
Now lets say you absolutely cannot get the tool on the plate, there’s a “manual tool measure” option in the UTILs menu. This will allow you to measure a tool off of your spoilboard. (you also have this option during a tool change as well)
If you do not measure a tool all of your cut heights will be off, and you risk breaking a tool or wrecking work.
I just ordered my 4896 and reading these posts are very educational. I’m quite new, having owned a Yeti Smartbench for the last few years and experienced numerous issues that are finally making sense.
I expect I’ll find these forums invaluable from day 1.
Yes there are some learning curves but over all I have liked the changes to EX. For my purposes it’s much more stable and I don’t get random “crashes” for projects that I would get in the past. Additionally, since getting the solution for Fusion I really like the touch off. It has made tool changes a breeze and less error prone. The only problem is now I am eyeing a new spindle so I don’t have to wrench off the bits.
I did switch from steppers to the servos and it was worth the upgrade if you can justify the cost (came from Nema 23). They are buttery smooth and accurate.
Agreed - biggest change for me was that the EX controller/CNC12 can actually handle long and complex g-code files that Mach4 would freeze or skip steps on.
Yeah the tool change time can really add up. Cutting out the need to use the corner finder every tool change has been great, but the new quick tool change spindle is going to be a game changer.
