What is the best way to surface machine 3D fillets on complex part geometries?

[Anonymous]

Where I work, we make parts with 3D fillets that wrap around the edges of our parts.  Nothing is flat and there are lots of complex geometry.  Visual requirements are very strict and our parts need to look like jewelry when they are given to the final customer.  Many other CAM systems have the ability to generate tool paths that morph between two curves and maintain constant contact with the the part as the tool spirals around the surface.  One lead in and one lead out.  

How do you accomplish this with Fusion 360?  The Blend strategy is close, but it often generates lots of little lead in and lead out moves that will leave witness marks on the part.  How do I get blend to make a smooth, constant spiraling motion as it machines the fillet?  Example (simplified) file attached.  One lead in and one lead out.

[David_Whittaker]

We need a solution to this problem.

[martin.dunschen]

The "Morphed Spiral" strategy can give good results for these cases. You need to select machining boundaries, the inner and outer edge of the fillet you're intending to machine. I will try to post a simple example.

[martin.dunschen]

Here an example. Admittedly there are a few lead moves, but they are confined to the edges. Additionally I used 'touch surfaces' on the geometry tab to restrict all cutting moves to the fillet.

[DarthBane55]

Hi, this type of operation is always a bit of a struggle, sometimes changing the tolerance by 0.0001" makes a huge difference on the result, but you have to play a lot with this to get it "decent".  Instead of showing this on a pre-made sample, would it be possible for you to use the actual file from OP?  I am very curious to see a good toolpath on that part.

[brad_francola]

Nice of you to post an example file 😊.  I see the tool doesn't quite make it to the edge of the fillet - I'll play with this and see what I can do.

[brad_francola]

Made a few changes.  This is the best I could do.  It has a fair amount of lead-in / lead-out moves but it seems like it's trying to cover the entire fillet.

[HughesTooling]

The problem I've found is you need the inner containment curve to be Centre and the outer curve Outside. The only workaround is create a sketch and project the silhouette then offset by the radius of the cutter, well just under so you don't get any water falling. This problem, needing different containment (centre and outside) is a problem I've come across with other CAM software as well. Any chance Autodesk can come up with something that allows for different offsets for the inner and outer boundaries?

Here I've offset by 1.49mm for athe 3mm cutter. File's attached.

Mark

[brad_francola]

I had a similar problem.  I used parameters in the expression for "Additional Offset" to accomplish this.  Check out the attachment.  And I'll take a look at yours.

[HughesTooling]

@brad_francola  The trouble is using touch\avoid surfaces gives a poor result. If you can use boundary curves you don't get all the disengagements\engagements around the edge.

Mark

[DarthBane55]

Can you guys use OP's file?  He took the time to create a file to show his current issue, would be nice to see it on his part and not a random sample part.  Sometimes geometry causes different issues/outcome...  if possible...  🙄  Still nice to see the sample as well of course, but now, will this work on his part?

[seth.madore]

@Anonymous  and @brad_francola are the same person 😉

[HughesTooling]

Here you go. Not sure why but Fusion wouldn't let me use an offset of -(1/32 - 0.001) so I just use -0.03.

Mark

[DarthBane55]

@seth.madore  hehe, I kind of thought so, but could not be sure...  still, the geometry is quite different, specially original model has some "sharper corners", and I had tried on it and could not succeed with a super clean path, so wanted to see it done on it.

@HughesTooling  thank you, will have a look for sure, it looks very clean on picture.

Something to learn for me from this, thanks again!

[brad_francola]

I have to say, of all the things I've tried, this is probably the best solution I've seen so far. I will try Morphed Spiral with machining boundaries on more complex parts and let you know what happens.  Many Thanks!

[brad_francola]

@HughesTooling  I used your method on an actual product.  So far, it's the best result I've seen.

Additional Offset = -(tolerance*5)

Bottom Height from Model Bottom Offset = -tool_cornerRadius+(5*tolerance)

Tolerance = .0001

This is close to being perfect other than the fact that the bottom edge of the fillet (where it's close to becoming vertical) starts to get a little wonky.  But, I don't think you would ever see this on the part.

Long term, they need a tool path with the convenience of Blend.  The workflow associated with offsetting geometry can become burdensome depending on the part complexity.

Thanks for your help!

[DarthBane55]

If flow would work right, it would be the ticket.  But it doesn't, at least not on your part, unfortunately.

the weird thing is the flow uses the actual solid model instead of creating an internal STL like all other 3d toolpaths, so you would think that it should create a much smoother result, but in most cases, it does not.

[Mattxer]

Yeah, I've had issues with flow just on simple surfaces. It can be quite the headache to get working. Also like posted in the above picture, the toolpaths can get really funky in some parts.

[HughesTooling]

---

@brad_francola wrote:

@HughesTooling  I used your method on an actual product.  So far, it's the best result I've seen.

Additional Offset = -(tolerance*5)

Bottom Height from Model Bottom Offset = -tool_cornerRadius+(5*tolerance)

Tolerance = .0001

---

Did you do the offset curve offset undersize or are you just using the Additional Offset? If you're just using the additional offset it might be worth making it -0.001 to minimise the wonky bottom edge. As long as you use a cut around the silhouette to clean up I doubt you'll notice a -0.001 or even -0.002 offset on the morphed spiral OP.

[brad_francola]

Hi. 

I offset the curve formed by the profile of the part by radius of the tool. 

Then, I set Additional Offset = -(tolerance*5).

Bottom Height from Model Bottom Offset = -tool_cornerRadius+(5*tolerance)

Tolerance = .0001