Fusion 360 Milling post with G64 Pn

G76 has no support

OK all, here's what I ended up doing.
I was going to start with Spangled's post, because I was going to have an overall G64 P0.0x value, combined with a per-operation G64 P0.0x value based on if the operation has a "smoothing" parameter applied.

But then I thought, that's not really what the smoothing is for. What we're really talking about is the overall tolerance of the operation, and a lot of operations which may need tight tolerance machining at high speeds may not have a Smoothing parameter, or you may not want to use Smoothing just to get your machine to not round corners under acceleration.

So I made it post out a G64 P0.0x block on every operation, which inherits the Tolerance value from that operation. (I am aware that this will actually result in a tolerance zone of double the input tolerance value. I'm fine with that, though it will undoubtedly cause some confusion. Fine for my purposes, I'll just put a conservative tolerance zone in there.)

I'm going to try using it like this for a bit, I haven't used it to run a machine yet, so keep yer finger on the E-stop button until you've run a test program.

You can change at any time theoperation Tolerance to G61
Its manly thaught for Engraving and 3D parts in wood plastic ...

98% of what I do is 3d parts in wood, so G64 is on most of the time. Does make me think I should put some code in the post which automatically switches to G61 if the operation tolerance is set below 0.003"/0.08mm or so, since the programmer's intention is to make a part as accurately as possible at that point.

Thanks for pointing that out Marty. I actually somehow hadn't noticed that neither G61 nor G64 appear to be implemented in the default post - unless your machine has a default G61 in the ini file, then you end up with G64 with no applied tolerance, which is pretty much the worst case scenario.

My take away from this is to firstly update my ini file so there's a G61 in there and then to look at a good way to implement G61 & G64 switching along with tolerance changes on an operation by operation basis.

Yes, the g64 with no P value makes some pretty wonky parts on my machine, since most of my operations are 250-450 ipm.

BTW I really like your tool change comment implementation. I have HSMworks comments stating the diameter, type, and intended feed rate in the tool library, so on tool change during a long production run I don't forget where I was in the process. It's saved me several wrecked parts already. Thanks.