What is the name of this part's fillet thingy? And how to achieve it in OnShape?

vu_nguyen404

I came across this interesting fillet thing but I don't know what is the name of it to search how to do it? Can you tell me what its name is and I'd really appreciated if you guys show me how to do it in OnShape also!
Thanks in advance!

S1mon

I would most likely create a shape like that with a fill surface (using an arc or Bézier to control the crown) or a sweep.

Some CAD tools have more of a continuum between fillets and chamfers which include chamfers that have a crown. Usually they also have variable fillet/chamfers. However I've never seen one that has a variable chamfer with a negative crown which is one way to describe the shape you're looking for.

eric_pesty

It looks like the "negative" shape could be done with a variable fillet so you might be able to use that on a separate body with a boolean.

Ignore this, I am completely wrong!

If you don't want to go into surfacing a lofted cut can do that:



https://cad.onshape.com/documents/770c9a212c05dcfee874c102/w/e964fb5663168eae96d3ae10/e/25e8222c6e61354ad01a0e09?renderMode=0&uiState=655bdb96a7adf04a160e3f5b

S1mon

I would recommend against using loft or boundary for a two sided surface like this. It will let you, but it will create degenerate points. These are not great for downstream stability of models. 

As for surfacing vs solid stuff, it's not hard to create the surface and then split the part.

Here's a quick example: https://cad.onshape.com/documents/85b08877ffd85424f7e54c90/w/7eac22832f797b0128fedddb/e/460ba3373588523309efe129

martin_kopplow

Some CAD Systems can create a face fill with a user defined angle relative to the two adjacent surfaces. Catia for example can do this. You would then create the boundary curves on the two (or more) faces, fill between them, and specify a 'negative' angle for the edges, that is an angle smaller than he angle between the face and the chord, to create a concave face.

In Onshape, we don't have the option to specify an angle, but we can loft with tangency, if we have two faces to match the tangency to.

https://cad.onshape.com/documents/7fe142a82ff4ab432104d2db/w/db3fce38923c5a14ee153077/e/150e9e5a030e573c38a87c77?renderMode=0&tangentEdgeStyle=1&uiState=655bedc6d894656739a5d8f4

Compared to lofting with an arc as a guide, this may also work for more irregular bondary curves, while being easily controllable with a single sketch. The thangent reference faces could also be created by a drafting extrusion from the top face and a cut line:

https://cad.onshape.com/documents/b7a75978e1ee860e4c9290a7/w/f2283d7652e9bc4cf9988a61/e/462ca7b1d596fe72dea60fde?renderMode=0&uiState=655bf5384fcdc1376b2e4af5

vu_nguyen404

Thank you guys! I find it most suitable for me using @S1mon 's method. Others are still very very appreciated!