What is the purpose of the live tool option in Fusion 360 ?

[Aadithya01]

I think the live tool option has come in the recent updates and I am wondering what is the purpose of the live tool option in Fusion 360 .. 

[LibertyMachine]

I can only assume it's for Lathe Mill/Turn machines, but beyond that I'm uncertain what it's purpose is

[ivan.stanojevic · Accepted solution]

That is intended to give the information to the post-processor so that the user could have the full control of the post output whether the tool is static or live.

But I'm still not sure if they have already implemented this in all generic mill-turn posts.

You can use the following parameters inside your post:

If it is not a live tool:

onParameter('operation:tool_live', 0)

and

tool.liveTool=false

If it is a live tool:

onParameter('operation:tool_live', 1)

and

tool.liveTool=true

You can find more info on the following link:

https://forums.autodesk.com/t5/hsm-beta-testing-english-deutsch/added-live-tool-setting-for-hsmworks...

[Anonymous]

Its kind of confusing to see this option when you are defining a tool for a mill, since there is no concept of a live tool on a mill.

From what is posted in here, there would be no end-result to changing this setting for example, on a tool used for 3-axis milling (on a mill?

[LibertyMachine]

With the exception of the probe, literally any other tool is going to be a "live tool" in a mill. You needn't worry about that setting in regards to mills.

[Steinwerks]

---

@LibertyMachine wrote:

With the exception of the probe, literally any other tool is going to be a "live tool" in a mill. You needn't worry about that setting in regards to mills.

---

We do broaching in our Haas, it's not live 

Of course I had to program it with a macro by hand and not HSM...

As an aside, nothing's really as scary as ramming a tool down a hole at 300 IPM with the spindle off.

[LibertyMachine]

Yeah yeah, you knew what I meant 

I also did external knurling on my Matsurra, also with spindle locked. Hand programmed, due to it's nature. 

I figured if the most recent poster was getting hung up on this "live tool" tickbox, he wasn't about to be doing anything extremely off the norm

[Anonymous]

You guys have been really helpful in this forum, so thank you!

However, I am hearing that unchecking this box has the effect of locking the spindle?

I am def not broaching at 300ipm on my haas, at least not yet. 🙂

Cutting my first mold this morning though!

Ryan

[LibertyMachine]

No, it will not lock the spindle (at least not in my tests). Just leave the box checked (as it's the default behavior) when you create a tool.

[Lonnie.Cady]

I was under the impression it was put there for lathe work.  Since a drill is a drill in the tool library and could be used in either a lathe or a mill.  In a lathe if the hole was at X0 you could drill by turning the chuck and feeding the turret.  However there may be times on a live tooled lathe when you are at X0 but would prefer to have the live tool spine vs the chuck. This allows you to override the default behavior when at X0 of spinning the chuck vs tool

[LibertyMachine]

That is correct. Hence why it has very few applications in the areas of Milling

[Steinwerks]

FWIW any tool that ISN'T defined as a probe will, I believe, error out a milling post with a spindle speed of zero. Haven't done any testing on that though, but I did see code relevant to such behavior in the Haas post.

[LibertyMachine]

That does not appear to be the case with the Fanuc post. Unticking the "Live Tool" checkbox and posting the Fanuc.cps (generic) post still spits a spindle speed

[Steinwerks]

Well you still have to set the spindle speed to zero. Live Tool would override whatever configuration is set up in the post to use the correct M-code, it doesn't turn the RPM to zero automatically.

At least that's how I understand it.

[Laurens-3DTechDraw]

Alright,

Let's get this straight.

In the generic Mill posts this box doesn't do anything. The post doesn't check for it and the CAM side doesn't change.

For lathes with driven tools this is used to determine if you want to drill on center with a static tool or a driven one.

All good mill-turn posts check if the hole is on center and check if the tool is live or not.(You shouldn't be able to use a static drill/mill in case of excenter drilling)

[timdrnecK6QSP]

Well thats unfortunate because there are _several_ types of tools I use in the mill that I'd like to NOT turn. In addition to the aforementioned probes and broaches, there are Drag Engravers, Drag Knifes, Laser modules, plastic extruders, Sharpies, etc. I can go in and hand code of course but it would be handy if simply unchecking the 'Live Tool' box on the laser module tool would actually do what you'd expect it to do.

[Laurens-3DTechDraw]

@timdrnecK6QSP

What I explained is the generic behavior.

But you could use it for other things if you like.

You are free to edit post processors to your own liking.

So what you are after shouldn't be too hard a job.

[timdrnecK6QSP]

Thanks Laurens,

Just a little frustrating, my previous attempts at modifying the posts for my Centroid controller has been pretty hit-and-miss. I suppose I just need to dive in and teach myself all the subtleties of working with those posts but I'd rather be making chips...

If the check box is _available_ for a mill tool, then it's perhaps something that should communicate with the available generic posts to drive the expected behavior. I was primarily replying to earlier posters who implied that it would be rare to not have a live tool in a milling application and didn't mean to seem as though I was being critical of your helpful reply.

[Laurens-3DTechDraw]

@timdrnecK6QSP
I don't think many people would expect a milling post to just not output rotation if this check box would be off. And I mean that in the way that a lot of users never use stationery tools in their mill and would be rather confused by the concept. So I feel it could cause a lot of trouble implementing this.
But I would be willing to assist in editting your post.

[david-carlson]

My interpretation is that it makes the spindle speed set to 0 RPM not rotating and stationary.  Then instead of drilling into something or milling on it it just plunges on the Z axis kind of like a file would with something clamped in a vice. If you put a file in the chuck you’re not going to want it spinning so uncheck live tool.  Broaching and lathes is where you want live tool unchecked.