Fill - This operations creates intersecting edges
Jeroen_4
Member Posts: 9 ✭
Hi,
I am fairly new to Onshape and have been playing around with it for a month or so. Currently trying to make a printable 1:87 scale model of a Frisian sailing ship, a so called "skûtsje". I have been able to creat the hull already and an now working on the deck.
I have created the outline of the deck (Dek side 3D sketch) with a projected curve (curve to face) and then mirrored it (Dek side 3D mirror) it using the right plane. Had then intended to use 4 guides (Dek guide 1 ... 4) to ensure the double curvature of the deck.
Problem however is that I am unable to use the Fill command with the two outside curves only. It tells me that the fill did no regenerate properly as "This operations creates intersecting edges".
Any idea what I am doing wrong here?
You can find my project at: https://cad.onshape.com/documents/83370e8bf558710b1f02b691/w/f2e633345116cb456ccaaf11/e/9a74c87a8823405591ed5d41
I am fairly new to Onshape and have been playing around with it for a month or so. Currently trying to make a printable 1:87 scale model of a Frisian sailing ship, a so called "skûtsje". I have been able to creat the hull already and an now working on the deck.
I have created the outline of the deck (Dek side 3D sketch) with a projected curve (curve to face) and then mirrored it (Dek side 3D mirror) it using the right plane. Had then intended to use 4 guides (Dek guide 1 ... 4) to ensure the double curvature of the deck.
Problem however is that I am unable to use the Fill command with the two outside curves only. It tells me that the fill did no regenerate properly as "This operations creates intersecting edges".
Any idea what I am doing wrong here?
You can find my project at: https://cad.onshape.com/documents/83370e8bf558710b1f02b691/w/f2e633345116cb456ccaaf11/e/9a74c87a8823405591ed5d41
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Best Answer
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Overall you've managed pretty well for someone new to Onshape.
The issue with your fill is that projecting the side sketch on to the thickened body is producing some funkiness at the ends of the curve. The outer edges of a fill need to be all tangent or nominally on a surface which is continuous. The ends of the two Dek side 3D sketches are not good.
I added some bridge curves at each end to replace the bad bits (and then trimmed the other curves) and was able to get fill to work (with or without the internal guides).
In general, thicken (in 3D) or offset (in 2D sketches or 3D surfaces) doesn't alway produce great curves or surfaces. There's no simple mathematically exact offset of anything more complex than the basic analytic curves or a degree-2 Bézier. In general they are convoluted multi-span degree-3 curves (or surfaces) with crazy density and a propensity for subtle little wiggles or errors.
https://cad.onshape.com/documents/36b64aed90b38f25360dddba/w/203d77fd805bf097a2f5fff5/e/04b51462e126f816b579cc43Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
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Answers
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See if this loft gets what your looking for.
https://cad.onshape.com/documents/b8ea708f7c5786d0f142cc84/w/04aa2c8c2c70f6135aab2a88/e/50dad2eb9a4161fc9a533bf4
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Overall you've managed pretty well for someone new to Onshape.
The issue with your fill is that projecting the side sketch on to the thickened body is producing some funkiness at the ends of the curve. The outer edges of a fill need to be all tangent or nominally on a surface which is continuous. The ends of the two Dek side 3D sketches are not good.
I added some bridge curves at each end to replace the bad bits (and then trimmed the other curves) and was able to get fill to work (with or without the internal guides).
In general, thicken (in 3D) or offset (in 2D sketches or 3D surfaces) doesn't alway produce great curves or surfaces. There's no simple mathematically exact offset of anything more complex than the basic analytic curves or a degree-2 Bézier. In general they are convoluted multi-span degree-3 curves (or surfaces) with crazy density and a propensity for subtle little wiggles or errors.
https://cad.onshape.com/documents/36b64aed90b38f25360dddba/w/203d77fd805bf097a2f5fff5/e/04b51462e126f816b579cc43Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
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@glen_dewsbury
Your loft solution may work for the needs of a model, but typically you never want to loft two edges together like that since both ends will be degenerate. NURBS surfaces do not like to be 3 or 2-sided. They are all 4-sided, sometimes with trims. 3 or 2-sided surfaces will often fail to offset or thicken - a likely next step in a lot of modeling workflows.
The joint between the two halves is also not tangent.
Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
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Partially. It does create the surface for the deck, but if I thicken it, the deck becomes two separate parts which I cannot join (boolean) with the hull. Trying a different rout now, by first making the hull and deck, without the gunwale, as one part. Then I should be able to hollow it, make the hole in the bottom and add the gunwale. Will report back on my efforts...
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Thanks, this is very helpful. Would there be a way to thicken this surface and join it with the hull?0
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Thanks for the tip S1mon.0
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I did a move boundary on the edges of the surface to make sure that it could join with the hull.
https://cad.onshape.com/documents/36b64aed90b38f25360dddba/w/203d77fd805bf097a2f5fff5/e/04b51462e126f816b579cc43
Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
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