Why do some sketch object lose their 'profile' status

[C.FOTI]

I was messing around with making a Platonic solid, a dodecahedron.  I know there are many ways to do this in Fusion  and tried out a couple.  First by creating the solid bodies then trying to arrange them (didn't work out).  So then I thought that I could create some pentagon profiles, line them up and extrude.  However, some of my sketch objects lost their profile status after rotating to the angle needed for the shape.

I know Fusion can be flaky when working with 3D sketches, but while this seems over the top nutty, I'm sure there's a reason for it.  Can anyone illuminate this for me? fusion file attached... 

[TheCADWhisperer]

I would fully define my sketches (2D vs 3D sketches).

I would almost never use Move...

[C.FOTI]

Thanks, but that was the first model and my question is about the second model (just profiles). 

The solids that you see come from a different profile and not related to my question.  Probably should have cleaned up the file but left it in so you guys can see what I was going after. 

[laughingcreek]

sketch lines have to be planer to each other to show a profile.  the ones that aren't showing a profile aren't.

[C.FOTI]

That's peculiar because each polygon is identical, and was created on the same plane and then rotated around axis's on the same plane.  Then I modified all to have a colinear constraint on the vertical lines they touch.  So I still don't understand why 2 are not profiles and 3 of them are.

[C.FOTI]

This gets weirder... so I roll back to time marker when there was just a sketch and a copy of it and start again from there.  I'm able to rotate the polygons into proper position 63.435 (+ and - as needed).  The uploaded drawing was at 62.5 each and I figured I could use constraints to snap things together (didn't work out). 

So now that I rotate into proper angle the objects immediately lose their profile status.  However if I were to go back to any random rotation where there's no touching on the vertical sides, then the profiles remain.  See the picture series.  It seems that profiles remain until the object touch one another on another edge other than the bottom one. 

Is this by design or a bug or a quirk in the way object are made in sketches?

Also why are some object marked with polygon constraint and other aren't when all objects were made with polygon command? 

[g-andresen]

Hi,

I think some of the tutorials by Christian Laholm might be of interest to you.

günther

[laughingcreek]

doesn't look planer to me-

[jeff_strater]

it all depends on how you went from the image on the left to the one on the right:

If you used a coincident constraint between the points, that will only move the connected lines, not the whole pentagon.  This will definitely pull it out of being planar.

You could model this, not as one sketch, but as a component with one sketch, containing one pentagon, then replicating that component, and use Joints to connect the pentagons to each other.  This will always do a rigid transform, keeping the pentagon planar

[C.FOTI]

I did use constraints before but I will give your suggested approach a try. 

But I still don't get why it behaves as it does (see video) I would like a comment on this video I've posted showing the behavior of the profiles at various angles.  https://autode.sk/2OH1baA 

What gives with Fusion profiles! | Search | Autodesk Knowledge Network

Shouldn't the behavior be the same regardless of angle?  So why does the profile get lost at certain angles and not others.

[C.FOTI]

Yeah, he has some good stuff there. I still think Fusion should make this easier! 🙂

Still however, I'd really like to know why fusion behaves the way it does as shown in my video below.

[TheCADWhisperer]

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@C.FOTI wrote:
Still however, I'd really like to know why fusion...

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Your sketch geometry that does not show profiles is not planar...

...back in a minute...

Examine the Attached file (you will have to zoom wayyyy in).

[C.FOTI]

Did you see the video I posted?

[TheCADWhisperer]

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@C.FOTI wrote:

Did you see the video I posted?

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No.  I only examined the geometry.

[jeff_strater]

 I did look at the screencast you posted.  What is most likely happening is that, when you rotate the second pentagon, there is some snapping that occurs, that "pulls" a point on the first out of its plane.  It could be lots of things, will have to be investigated further.  There is some auto snapping that happens in sketch.  Part of the issue, I think is that while 63.435 is pretty close to the right angle, I wonder whether the true angle is a bit different, and there are some accuracy problems.  The other thing I noticed is that there is a lot of overlapping geometry, caused by creating the pentagons as full pentagons.  Then, there could be some slight differences when things are put together, that also results in selecting different geometries when rotating.  The sketch solver has a tolerance that it uses (1.0E-6 cm, I think), and equivalences that are within that are "close enough".  However, it could be that the test for planarity is pickier than that, or the rotation amplifies some small differences into bigger differences.  In the screencast below, I show a technique, that while a bit tedious, does result in the behavior you expect.  At the very end, I us Measure to show that there is still an angle between lines on the rotated pentagons, which is what leads me to believe that the actual angle is still a bit off.  Anyway, there are lots of options, I think, for you to move forward.