Face Fillet

[SpenceSolutions]

Hello,

I am trying to model a Face Fillet between two solids in a multibody ipt.  I can not select a second set to fillet.

I have unchecked "optimise for single selection".

I have tried various sizes of fillet radius and also modelled with a gap the two solids bodies but still no luck selecting both solids.

Please find attached example.

Thanks

Paul

[imajar]

Face fillet does not work across bodies - you will need to combine the bodies first.  See attached.

[SpenceSolutions]

Hello Aaron,

Thanks for your reply. I have re modelled with out multibodies, extruded th eparts so they interfere and then I can fillet.

But I thought the idea of Face Fillet is that is would fill a gap between two solids ? He is a simple model "PArt 4"  Two solids ( not Multibody ) that I should be able to join with a face fillet ?

I have done this with two cylinders at 90 degs to each other and the face fillet fills the gap between the cylinders.

Am I missing something here ?

Regards

Paul

[imajar]

I'm not sure what the original design intent was for face fillet, but definitely it is useful for connecting disconnected faces in a variety of circumstances - including disconnected lumps.  In my experience though, it doesn't always do what I think it should do. 

I was a bit confused by your statement about "PArt 4", did you intend to attach a  part?

[SpenceSolutions]

Oh ! Yes ! Part 4 attached. 🙂

[imajar]

I wasn't able to get your sample part to face fillet either, and I'm not sure what the reason is why some disconnected lumps will fillet while others don't.  Hopefully somebody from the dev team can chime in on that one.

[JDMather]

Why does this need to be a Face Fillet?

Is your goal simply to test out Face Fillet solutions, or is your Design Intent to create some geometry that you thought perhaps Face Fillet might be the solution, but there could be other solutions?

[SpenceSolutions]

Hello JD,

I posted that model as an example. My real case is a web for a wheel. I have attached a screen shot of the sketch as I originally drew it.

I revolve the dia 35 hub and then execute a 3mm symmetrical extrude on the web,  ( the web has the 25 dimn at the hub intersection point ) and 3D this leaves a gap between the hub and web at each side of their point of tangency.

I thought a face fillet would blend both parts together but after I select the dia 35 face I can not select another face.

I originally modelled as multibodies but changed that to single solid. Still no luck.

I then continued the web sketch "into" the dia 35 hub and extruded. This obviously gave me interference between the hub and web. I could then face fillet one face on the web to the dia 35 face at a time.

Apologies for the late response , I am in NZ.

Please find attached screen shots.

Regards

Paul

p.s

Just been watching one of your you tube postings.

[johnsonshiue · Accepted solution]

Hi! Inventor is not good at this kind of Fill Fillet. In some cases, it may work (with Help points). But, in most cases, you can run into failure easily. This kind of fillet is a bit open-ended. I suggest you add more geometry before filleting.

Many thanks!

[JDMather]

---

@SpenceSolutions wrote:

...this leaves a gap between the hub and web at each side of their point of tangency.

---

There are a plethora of techniques to eliminate or avoid that gap altogether.

 - Model from the center of the hub and add the hole to the hub later.

- Replace Face the end of the spoke.

- Move Face the end of the spoke...

Probably several other techniques I could think of - then add Fillets.  (Could then be Face Fillets or Edge Fillets.)

[SpenceSolutions]

Hi All,

Yes, as said I did get around the problem by running the web into the hub and there are many work arounds.

I am just surprised that Face Fillet wouldn't work in this instance so I was looking for confirmation that " it wasn't me".

Ok. Thanks to all replies. Limitations of Face Fillet noted.

Regards

Paul