Smoothed boss with guide curve

3D Design Volume Model
1

Hello
I'm under win 10 and sw 2017.
I'm trying to design a glass roof whose mold will be 3D printed.
I made 2d and 3d guide sketches.
I created plans and drew the couples on each one.
When I do my smoothed boss, I have a defect that I can't seem to solve.
I am attaching a screenshot and the SW file

Capture
Capture1683×901 156 KB

glass roof. SLDPRT (226.7 KB)

Thank you
Diiity

1 Like
2

Hello

Try to go to surface.

  • 1st surface: sketch 3
  • 2nd surface: bottom line sketch 3 and sketch 3D7
  • 3rd swept surface: upper line sketch 3 - sketch 3D7 + guide curves (radii sketches 5 to 15)
  • And then you sew the surfaces by checking create a solid.

But do you want the whole volume or just the curved surface?

verriere
canopy1672×998 133 KB

As I'm in SW2020, there's probably no point in giving you the SW file.

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3

Maybe simpler, split your sketch 3 into 2 separate sketches. To have the upper line in one sketch, and the lower line in the other.
And then in your guide curves you select: your sketch3D7 and your 2 new sketches (obtained from sketch 3).
And normally, you should get the desired result.

verriere 2
canopy 21640×999 125 KB

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4

Hello @diiity

It's the ultra-curved part of your guide line that makes you swarm.
If you want to keep it simple, you do a first part without the end
then you do another game but by bossing starting from the flat face the black lines (in the direction of the red arrow) and with two guide curves
That way you won't have the defect anymore normally

Otherwise there is obviously the method of @opiep27 (which I salute in passing)

Kind regards
image

1 Like
5

Thanks guys, it works by splitting the sketch 3 into 2 sketches, both in surface and solid.
Besides, I prefer solid because it's a mold, it has to be full.

On the other hand, I have the 3D sketch which is in yellow because originally I had used a construction line to have the right distance from sketch3 that I split.
I can't repair this sketch, I have to redo it, is there another solution?

6

Good evening @diiity ,

Personally, I don't see any sketches in error... Everything is blue or black.

To come back to the smoothing problem, another solution is possible without changing anything to the initial geometries: use the " Selection Manager " (right-click in a graphic area) to select only certain elements of a sketch, or composite entities: segments of different sketches + body edges...
Can be used for several functions of generating surfaces and volumes.

Good night

2 Likes
7

Sorry but I was wrong, it still doesn't work, I noticed it when I wanted to make a symmetry

8

Thank you all.
I succeeded with the method of m.blt.
I keep the video under wraps.
Diiity

1 Like