Fusion 360 trouble with fillets

[SteveIParticipant @stevei]

Hi,

 

I am having a spot of bother with Fusion 360 and fillet command.

I am currently only able to make “subtractive” fillets, when I have a spherical body coming in at an angle to another spherical body; see the 2 screen shots attached. I see in videos and screenshots users making fillets more suitable for e.g. a pattern. I have tried different approaches of extruding the second spherical body into the main body. I must be missing something.

Any tips?

 

Thanks,

Steve

[Swarf MakerParticipant @swarfmaker85383]

Hi Steve.  The reason is that you still have seperate bodies.  Join them together first and then the fillet will work as you expect.  At the moment you are just filleting the end of your upper body and that can only produce the result that you show.

[SteveIParticipant @stevei]

Hi Swarf Maker,

 

Thanks! That certainly allows the type of fillet I want. It has been a habit of mine to simple create new bodies until I am finished with the designing.

 

Thanks,

steve

 

 

 

[Ady1Participant @ady1]

I never use the fillet command in Alibre during a build because it can cause drawing issues if you need to reverse anything

Once I’m finished I may consider fillet/chamfer type commands but if there’s any part of a drawing I don’t have full manual control of during a build I avoid it until after full drawing completion

[JasonBModerator @jasonb]

I often fillet as I go along but model patterns and anything else as one single body so would have only got an internal fillet in a case like that.

Fillets can be tricky with most CAD programs, F360 seems to be able to do the odd one that Alibre gets tripped up by but can often be got around by changing the order fillets are applied in or adding a small radius one and then increasing it’s radius. The more complex the joining profiles the harder it can be. This patter n was quite hard to get all the fillets where they were needed and as it is for 3D printing it is not possible to leave them out and let the CNC’s ball ended cutter leave the fillets.

[NealebParticipant @nealeb]

I have seen it as a general recommendation to leave fillets and chamfers to the end. It doesn’t usually affect the design process and can save a lot of problems when you make a change where there is an existing fillet. Works for me! Insisting on a single body also gets round the problem of the two parts not quite touching which can give unexpected problems when you try to add a fillet.

[Alan Wood 4Participant @alanwood4]

Timely YT posting by Clough42 at the weekend regarding fillets.

[John Doe 2Participant @johndoe2]

Yes, often when a fillet or a chamfer won’t form it is because there is gap in your model.

I had difficulty with one design which I eventually traced to a minuscule gap between two parts – only a tiny fraction of a millimetre, in one tiny part of an arc, but as far as the CAD was concerned, the two parts were separate bodies, and therefore it would not create a fillet or chamfer between them.

I find that my CAD sometimes says “cannot perform the requested function”, or similar words, but without telling you why.

Note: if you are intending to shell out a solid shape; be aware that the wall thickness might suffer if you shell first and fillet later, (sounds like a cooking recipe !!).

If you complete the external shape including fillets first, then when you shell the body out, the wall thickness will be consistent in the areas on the inside of any external fillets.

[SteveIParticipant @stevei]

Hi,

 

Thanks all.

It makes sense now I think about it that you cannot add a constructive fillet unless the bodies are joined.

 

Steve

[Nigel BennettParticipant @nigelbennett69913]

+1 for Neal B’s suggestion to leave fillets until the end. it is so easy to reference a fillet during construction of following features. If – no – WHEN you go back and change a pre-fillet feature, it can upset not only the fillet but all subsequent fillet-dependent features. It then takes a lot longer to reconstruct it all without errors!

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