3D contouring with form tools

[crice.midsouth]

Is there currently a way to use form tools in 3D contouring toolpaths?  I do a lot of mold work and need to be able to rough and rest machine with high feed cutters.  Right now, the only way I know of to make that work is to tell my software I'm using a bullnose end mill.  That leaves quite a bit of material on the part that the software thinks isn't there.  I really need a better way to do this.

[seth.madore]

Sadly, no.

[leo.castellon]

If you are using Sandvik tools, you are in luck, Fusion has a tool library that you can import: Tools for Autodesk Fusion 360 | Autodesk Fusion 360 . Now whether that helps with programming, I am not sure. I have an Ingersol tool that I use for high feed milling and I do remember that the tool definition that I created was close, but in some places, it left more material than desired for finishing as the shape of the tool wasn't perfect. It would be nice if we could get this to work better.

LeoC

[crice.midsouth]

Seth,

Are there any plans to add this as a feature?  I didn't see any mention of it on the roadmap.

[seth.madore]

---

@crice.midsouth wrote:

Seth,

Are there any plans to add this as a feature?  I didn't see any mention of it on the roadmap.

---

We have some loose, undefined plans to add more tool types, but I'm uncertain if they would be intended to be used in "legacy" roughing toolpaths (the HSM Adaptive and Pocket that have existed since the beginning)

[crice.midsouth]

Leo,

I'm currently using Ingersoll Chip Surfer high feed modular cutters and others.  Ingersoll has .step files of all their tooling online, but I can't use form tools with any of the 3D toolpaths in Fusion.  If you're saying you know a fix or a workaround for this, I'm all ears.

[leo.castellon]

Unfortunately, no. I do not use high feed mills often and I recently discovered Sandvik's offerings for the available tools for Fusion. I haven't had the time or need yet to see what happens if I tried using a Sandvik's high feed mills in one of the adaptive paths. At the time we were making a lot of parts out of 17-4 PH and the high feed end mills worked great, although since there was a lot of surfacing work required and I couldn't define the tool exactly, I left stock to leave a little more than desired to make sure it didn't undercut any surfaces.  

LeoC

[leo.castellon]

I just played around with Sandvik's tool offerings in the Fusion library, and it doesn't seem to help, so sorry for giving you false hope. Hopefully Fusion works on this type of strategy, as high feed end mills work great in hard materials. 

LeoC 

[crice.midsouth]

I'm not sure how a new tool type would help.  High feed cutters would be very hard to define just by a "tool type".  The best way to do it would be to allow 3D machining with form tools.  The forms would have to be generated by the cutting tool manufacturer of course, but that doesn't seem to be an issue.  Any brand of high feed cutter I've used offers .step files.  Other CAM systems have had this functionality for quite a while now.

This is one of several issues that are beginning to sour my opinion of the software.  I began using this CAM software several years before Autodesk bought it, when it was still HSMWorks.  I'm sad to say that I'm shopping for new software now.

[a.laasW8M6T]

You don't need a form tool to use High feed cutters.

All you need to do is define them as a Bullnose endmill and use the "Programming radius" Data from the tool manufacturer like below the RE value:

On my Taguetec Highfeed insert mills the Programming radius is on the back of the insert packet.

as Highfeed cutters are really only used for roughing, this approximation results in (IMO) acceptable results, and it doesn't ever violate the model.

I cant say for certain but I suspect most Cam software treat high feed mills the same way.

[crice.midsouth]

I'm fully aware of the "programmed radius".  For the cutter I'm running right now, it's .098". I realize that probably works for most people, but not for me.  On a 1/2" Ingersoll Chip Surfer High Feed, that will leave about .040" on a ~15 degree slope. Most of my work is in HRC45 and harder.  It doesn't work out real well for your finishing tools when you plow a spade ball nose into .040" of stock that wasn't supposed to be there.  If you can't accurately predict how much stock will be left after an operation, what's the point?

[a.laasW8M6T]

Yea it totally see what you mean there, I've not experienced that myself(other than material in corners) but I can see that would be frustrating, obviously different types of feed mills will yield different results.

To be fair Fusion is a (relatively) cheap software, IMO its still pretty lacking in decent 3D finishing paths too, I mean you can get good results but it takes a lot more work than it should to get there.

I used a 12 year old version of another software the other and the 3d contour toolpath was waay nicer.

I know we will but getting support for Circle segment tools in the future, but no Idea about form tools for 3d milling, I don't think you could force a circle segment definition to do what you need

[seth.madore]

No, Circle Segment tools (in Fusion) are not going to be compatible with current HSM toolpaths.

I would like to see how other CAM packages solve for the geometry of high feed mills. It must be a prevalent issue, seeing that all tool MFG's offer up substitute geometry...