I have a connection problem at the bottom of my shell, it was obtained by symmetrical the 2 sides of the shell. At the level of the plane of symmetry, several bad connections are formed, characterized by a tiny space between the 2 edges of the surfaces.
Can you help me join them and thus close the surfaces?
Hello
When I open your room, I don't see any bad connections :(
What level are they at??
For my part, whatever the measurement I make, each time, the objects intersect.
How did you see them? by zooming in?
Cdt
Joss
You can go through Insert/Surface/Stitched Surface. This tool allows you to sew 2 surfaces as its name suggests, with a certain tolerance of spacing to be defined. The result will depend mainly on the quality of the original surfaces.
Yes indeed I notice defects when zooming in, but what prompted me to look is the fact that I cannot form a volume with the "sewn surfaces" tool, a message alerts me that "more than 2 sheet metal bodies cannot be joined together to a single edge joint"
What does that mean?
Hello
I think the visual approximations misled you!
But SolidWorks doesn't always display edges correctly, and it can be confusing indeed!
To find out if your surface is properly closed, you can try filling it:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/Filled_Surface.htm
Concerning the sewn surface, see the help:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_DVE_KNIT_SURFACE.htm
But if the sewn surface solved your problem, choose the answer from @Benoit.LF, because he was the one who submitted the idea!
Indeed, I checked again and your surfaces are well bound. If you deduced that they were not sewn because of a big zoom, you should know that Solidworks has some graphical bugs and especially when you zoom all the way, you may have the impression that the surfaces overlap or that there is a slight gap between them but this is not the case, at least on your play.
The message "more than 2 sheet metal bodies cannot be joined together to a single edge joint" confirms that your surfaces are joined together. When your surfaces are joined, their common edge turns into a single edge, which is why you can't join two already merged edges.
Cdt
Joss
Thank you for your time (work :p) and your answers. I'll try to change the resolution if I find or change my method.
See you soon.
See you soon!
PS: if you could designate a "best answer", it would close your question and earn a few points to the members who participated, thank you!
For performance, you can try what the help offers, but the edges have always been badly displayed!
http://help.solidworks.com/2013/French/SolidWorks/sldworks/HIDD_OPTIONS_PERFORMANCE.htm?id=f9540f6c666741e2a5ab314cb45ad311#Pg0
In particular these two points:
Curve generation
Select one of the following options. (This option is only available when Complex Assembly Mode is enabled.)
Only on request The initial curvature display is slow, but it uses less memory.
Still (for each shaded model) The curvature is displayed faster than the first time, but you still use more memory (RAM and disk) for each part you create or open.
Level of detail
Move the slider to Off (no detail) or move it from More (slower) to Less (faster) to specify the level of detail during dynamic view operations (zoom, pan, and rotate) in assemblies, multibody parts, and draft-quality views in drawings. (This option is only available when Complex Assembly Mode is enabled.)
What bothers me is the message "more than 2 sheet metal bodies cannot be joined together to a single edge joint".
I don't have access to the tree structure of your part as I am under SW13, but do you have sheet metal bodies? It's "surprising" considering the shape I could see in it under eDrawing.
For work time, we'll end up later tonight because of you:D
simply try to lengthen all the surfaces that can be elongated
then you will only have to rectify the surfaces that are loose
@+ ;-))
The simplest, in my opinion, would be to close the half-shell with a "flat surface" function, and then only to do the body symmetry with fusion.
The problem seems to me to be (for the little bit of testing I did) that the contour line of the half-shell is not flat (in any case the function doesn't want to take the edges in red, see pj)
Hello
Having a version prior to yours I can't open your room,
However, did your sketch have a coincidence relationship with an original axis?
Maybe there is a slight gap in the sketch you have symmetrical?
Regards nicolas
Hello
I think your problem comes from the accuracy of the recovered 2D sketch (Sketch2). Indeed, by zooming in on the entities that should be on the plane of symmetry (right plane), we realize that this is not the case. Since you use this sketch to make your surfaces, it's normal that during symmetry, the bodies overlap.
The solution, in my opinion, is to retouch the sketch by putting constraints in relation to the plane on the right.
Kind regards
Hello
Several things about your room:
- It is better to work than half to obtain a volume and then to symmetrical as indicated by one of the speakers, so add a surface on the central part and sew
- To have beautiful surfaces, the basic postula is to have beautiful curves and simple curves (according to one of my teachers at the time when I was working under strim 100). Except on your parts your splines are not "clean" no tangency to the horizontal, no smooth curvature, no constraints. For example, on Esquisse3D number 3, I would put a tangency with respect to a vertical construction line.
@+
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