Cannot emboss and press pull sketch

[Anonymous]

I am designing a bike tyre, and I want to emboss a sketch on the rim (see photos). I click "finish 2D sketch", then click split faces, select the faces onto which I want my sketch and I click my sketch as the splitting tool.

When I try, however to press pull the face (with offset type "new offset"), I receive an error massage stating:

"An existing fillet or chamfer could not be detected.

Try suppressing or deleting existing fillets/chamfers before attempting the operation."

I'd appreciate any help!!!
Error in press pull.Face being split.

[mavigogun]

It sounds, perhaps, as though the Press Pull is being attempted across a Fillet Feature- if that is the case, you might create the base geometry for the tyre by Rotating a Sketch Profile instead of rounding a solid via Fillets.

A more authoritative response will require the design- File > Export > and Attach the design to your reply.

[davebYYPCU]

But timeline has Revolve 1,

Fillets Nil.

[mavigogun]

---

@davebYYPCU wrote:

But timeline has Revolve 1,

Fillets Nil.

---

Doh!   Reflecting my level of sleep, apparently.   I should go do that.   I wonder if that seam is contribution to the failure?    I had a Bug-Numbered Press Pull failure across a seam about a month ago- but in my case the operation deformed across one point of the seam, as though snagged.   

Does it  make any difference if you select all of the Split Faces at the same time?    Do you have the same result with a Split Face performed free of any seam?

[Anonymous]

I have not used fillet.

I cannot press pull the feature. I want it to cut 1 mm from the surface.

[jodom4]

Hey ,

You might find this tutorial useful. It's got some great tricks to achieve the kind of thing you're looking to do:

[mavigogun]

---

@jodom4 wrote:

Hey ,

You might find this tutorial useful. It's got some great tricks to achieve the kind of thing you're looking to do:

---

Such a great exploration- so much packed into it.    On first viewing many-months-back, my response was "wow- I need to think this way"; still true.    Any clue who the author is?

[jeff_strater]

the reason for this error message is a bit low-level, but worth understanding.  When you do a face Move, or Offset, Fusion goes through the following process:

• identify any fillets adjacent to the selected face
• remove those fillets
• transform the face
• re-apply the fillets

Picture here an Offset of this face:

An incorrect result would be:

but, literally, that is what you are asking Fusion to do.  But, we don't want to do that, instead we want to get:

so, this is why Fusion does this "un-fillet, offset, re-fillet" operation.

Because these operations need to work on imported geometry, not just natively created parametric geometry, this process tries to identify the fillet in a geometric way.  So, the fact that your design does not contain any Fillet features is not related to the error, even though I agree this is confusing.

The upshot of this overly-long explanation is:  There is apparently a bug in the fillet-finding algorithm.  You can see, I hope, how all of the tangent-continuous, toroidal surfaces here could be confusing the logic.  You can see how they might be mistaken for fillet faces...

I was not able to reproduce the error from your STEP file.   I got a different error:

So, if you want to make it easier on us, if you can share the Fusion (F3D) file here, with the split faces on it, we'd be happy to take a look at it, and see if we can track down the geometry bug.