I was wondering why does using Face fillet creates a spline. I just noticed this while I was creating a part and my VAR confirmed that it is intentional.
IMHO, it should always be a radius. The intent of using the Fillet command is to add radiuses on edges. My VAR advised me to put the radiuses in a sketch but that is out of the question. Most people know fillets shouldn't be in sketches...
Part attached
Just tested on another part, a rectangle. Used face fillet on it, gives me a radius. Weird
I sent this to my VAR to ask him to explain the distinctions between them.
..hmm,.. I don't have 2019 but can import this into another program and your models corners are all fillets, not splines.
..maybe your drawings ortho views are at a skew and you're getting splines?
It seems like a spline as it doesn't give any radiuses, even inside the 3D part.
This one writes .125 radius (Congé4)
This one writes nothing (Congé3) If I click I can see it's an arc as it gives an arc length but there's no radius.
The explanation my VAR gave me was that whenever a cylindrical face is part of the selection of the fillet feature then SolidWorks will generate a spline.
I answered back to him that it was a ridiculous reasoning to have and that the principles were still the same. Asked him why can I do it with extrudes but SolidWorks can't.
He answered ''I understand your point Alex'', that's it.
Now that I think a little more about this, perhaps it is a limitation of SolidWorks.I'm guessing that a cylindrical face can have 2 different interpretations of tangence and the easiest way to have SolidWorks not mess around with this ambiguity, again I'm guessing, was to have it be created as a spline.
Alex,.. yeah, sorry, I do not have 2019 so I'm only looking at the imported data and all are fillets (symmetrical)... maybe the OP is playing around with the other options shown by Kevin Chandler below?
That's a full round fillet not a face fillet.
So, given the above geometry, you can see why selecting the fillet doesn't display a radius in the status bar. Your model is a degenerate case where the radius is constant from one side face to the other, but it doesn't have to be.
I understand your explanation but there is an option inside the fillet called ''Tangent propagation'' that should be doing what you just explained, unless I'm misunderstanding it.
tangent propagation propagates your selection (edges or faces). so in the help example, they did not need to select these faces:
Understood!
Guess I'll send an E.R. in as my VAR advised, I think there should be an option that a full round fillet can be forced as a radius.
Thanks Jim Sculley and Jeremiah Feist for the explanations.
After looking at this further, I see why you are complaining. For instance, for the model I pictured above, you can select the radius face along the straight portion of the part and it will show the radius in the status bar:
Refusing to do so for a radius attached to a cylindrical face seems a bit arbitrary.
Exactly! That is what makes me wonder, though as I think, it is a limitation forced by the possibility of 2 different tangencies. The opposite tangency to the one I picked could do something extremely weird and probably very hard for SolidWorks to calculate.
In your case, there aren't multiple possibilities of tangency besides reverting the tangency(which wouldn't be a fillet anyways), which is probably why it can display a radius.
Full round fillets can cause many issues. Often the underlying surface definition is heavier than a 2-face fillet. Also takes much more "modeling power" from the software. 3-face fillet faces are also more prone to corruption.
This is due to the underlying geometry at the kernel level, not the application. It also happens in NX and Creo.
IMHO, it should always be a radius. The intent of using the Fillet command is to add radiuses on edges.
Hello,
I will suggest that fillets are for the rounding of edges.
A circular edge, although the most common, is simply a singular instance of filleting.
Other than for a full round fillet, SW offers a change in profile and for a face fillet, you can also apply an asymmetrical fillet, which generates an ellipse (at the default profile, which can be changed).
Kevin
Perhaps my E.R. should be centered around sheet metals. I work with sheet metals on a daily basis and they are the reason I hate splines. Splines generally cause problems with nesting programs and they are why I try to avoid them as much as possible.
Perhaps a feature in sheet metal to create fillet edges that would keep their radius.
Alex Lachance wrote:
Perhaps my E.R. should be centered around sheet metals. I work with sheet metals on a daily basis and they are the reason I hate splines. Splines generally cause problems with nesting programs and they are why I try to avoid them as much as possible.
Perhaps a feature in sheet metal to create fillet edges that would keep their radius.
Like Mr. Salvador, I can't see your part either, but for sheet metal, I try to stick with the sheet metal break corner command instead of the standard fillet:
If you can't break a corner in sheet metal, then that's a flag.
Fillet will round pretty much anything.
Kevin
Unfortunately, the break corner does not work with an edge like this. I hadn't thought of trying it before though.
That's a full round fillet not a face fillet.
So, given the above geometry, you can see why selecting the fillet doesn't display a radius in the status bar. Your model is a degenerate case where the radius is constant from one side face to the other, but it doesn't have to be.