Why can't I loft these two simple profiles to create (fake) a variable radius fillet?

StephenG

The two profiles have the same basic shape and same number of vertices on each profile.



Is it because the two profiles have an edge that superimpose one another?

Is there another technique I should try? 

elif

@StephenG please do file a bug report. I think I know what's going on. Thanks.

elif

@StephenG  Please take a look at 
https://cad.onshape.com/documents/2a88780b60140dd38ada5591/w/9435e6b2eae78fdef93d3dbb/e/9624a06e3a694b40ab5c4b46

Is this not what you had in mind?

StephenG

I just tried separating (creating a gap between) the two...


Well, I'll be... it worked, gave me the exact solid volume I wanted.  Is this a bug?

michał_1

StephenG

So (based on your video) my understanding is that is will only work for generating a surface from open profiles. Using closed area profiles to create a solid is forbidden.

Is this a bug?   

konstantin_shiriazdanov

don't think this is a bug, it is some side effect

michał_1

@StephenG not quite, I would guess that loft tool is trying to build a face between two edges that are in the same place, so my first thought was to remove that edge.

elif

@StephenG please do file a bug report. I think I know what's going on. Thanks.

elif

In the meantime, can you try adding vertex matching to your solid case? (Using a pair of vertices not on the shared edge)

StephenG

I just tried the "Match Vertices" option; didn't help.

I will go ahead and submit a bug report, but in the future I would like to see a mechanism exist that would allow me (the author) to "promote" a question, or discussion to either a feature request or a bug report. The information (context) of discovering this limitation (bug) is important for the person(s) understanding how to address it.
   
In the interim I suggest you tweak the Online Help to make users aware of this limitation...


Add the following text....

  o Profiles curves cannot superimpose other curves in profiles selected to be part of the loft.

elif

@StephenG  Please take a look at 
https://cad.onshape.com/documents/2a88780b60140dd38ada5591/w/9435e6b2eae78fdef93d3dbb/e/9624a06e3a694b40ab5c4b46

Is this not what you had in mind?

StephenG

How did you do that?

Wait a minute... I see how you did it. When I checked the Match Vertices option I never completed the important step of actually designating what vertexes to match together. I just assumed the software would preform its magic and give me the most "relaxed" solution with minimum twisting. I can envision how loft looks at the vertices of each profile and tries to create an ordered relationship that will create a result with minimum twist. I am guessing when two vertices have the equivalent XYZ location it thought this cannot be, something must be wrong. Should be a simple code fix to handle this condition.

So why didn't OS prompt me, "Hey dummy, if you use the Match Vertices option you got to at least give me 1 set to match up!"?

Is it true that one can only specify 1 set of vertices to match? Why the limitation and why doesn't the UI wording reflect that? "Match vertices" should read "Match 2 vertices" and it should not be possible to select more than 2. And it should not be possible to select 2 vertices from the same profile sketch.

OS is full of places where you have to know precisely how to drive it; easy for someone who wrote the code but kind of challenging for a new user. A little more bounds checking and selection filtering in the UI would go a long to making the product easier to master. 

Anyway, much thanks for showing me the errors of my way.