Check Geometry shows error in Sweep

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Jacutus
Posts: 5
Joined: Sat Apr 15, 2017 3:57 am

Check Geometry shows error in Sweep

Post by Jacutus »

Check Geometry shows that the Sweep is solid but invalid and Shell1 is not connected.
Shape Content shows:
VFP_Proto_Helmut_with_Front_and_Back_Brims.Sweep:
VERTEX : 400
EDGE : 610
WIRE : 212
FACE : 212
SHELL : 1
SOLID : 1
COMPSOLID : 0
COMPOUND : 0
SHAPE : 1436
Anyone have any idea what I'm doing wrong here and what I do to correct it?
VFP Proto-Helmut Single Brim Sweep.jpg
VFP Proto-Helmut Single Brim Sweep.jpg (318.47 KiB) Viewed 953 times
https://www.dropbox.com/s/sylelwnua4krk ... FCStd?dl=0

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.16.6706 (Git)
Build type: Release
Branch: releases/FreeCAD-0-16
Hash: f86a4e411ff7848dea98d7242f43b7774bee8fa0
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17
renatorivo
Veteran
Posts: 2611
Joined: Tue Feb 21, 2012 8:07 pm
Location: Torino - Italy

Re: Check Geometry shows error in Sweep

Post by renatorivo »

It's not exactly what you want, but it's an idea
VFP1.png
VFP1.png (73.42 KiB) Viewed 890 times
VFP-Renato.FCStd
(488.42 KiB) Downloaded 17 times
Renato
Jacutus
Posts: 5
Joined: Sat Apr 15, 2017 3:57 am

Re: Check Geometry shows error in Sweep

Post by Jacutus »

Thank you! Could you give me step by step instructions on how you did that? It looks better than what I have.
renatorivo
Veteran
Posts: 2611
Joined: Tue Feb 21, 2012 8:07 pm
Location: Torino - Italy

Re: Check Geometry shows error in Sweep

Post by renatorivo »

Jacutus wrote:Could you give me step by step instructions on how you did that?
I'm trying
1 - Import useful items (ImagePlane, HollowSphere001, Front of Brim Sketch)
2 - Since your cut object is made up of many edges, and after it requires a fusion with a cube, I changed its profile and its position just below the top line of Front of Brim, this to intersect the results
fig1.png
fig1.png (94.91 KiB) Viewed 828 times
3 - Pad001 and Cut004 are the next operations
4 - Simplified Front of Brim Sketch, but you can do better...
fig2.png
fig2.png (7.64 KiB) Viewed 828 times
5 - Sweep004 along the outer contour with Frenet = False, this allows the faces to follow the contour orientation
6 - Check Sweep004 and Cut004
7 - Fusion001 -> Check -> Valid

Sweep between two Sketches requires the same number of points between the initial and the final figure, otherwise the result is unpredictable.
Sweep along a segmented path tends to self-intersect and is not valid. It generates a bunch of lines and creates very large files.

VFP Proto 1,33 MB
VFP_Proto_Helmut_with_Brim_Sweep.Sweep:
VERTEX : 400
EDGE : 610
WIRE : 212
FACE : 212
SHELL : 1
SOLID : 1
COMPSOLID : 0
COMPOUND : 0
SHAPE : 1436

VFP-Renato 488 KB
VFP_Renato.Sweep004:
VERTEX : 32
EDGE : 56
WIRE : 26
FACE : 26
SHELL : 1
SOLID : 1
COMPSOLID : 0
COMPOUND : 0
SHAPE : 142

Renato
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