Create a volume from a complex surface

3D Design Volume Model
1

Hello

I have an imported surface which I assume is from a 3D scan, it is a polyester body. The surface is a "shell" which means that it represents the volume of my bodywork and is therefore hollow. I would like to transform it into a volume body in order to add the cuts that we make in it. I use the thicken function for this but nothing to do solidworks don't want to thicken it by more than 0.5mm. I read in the solidworks help that there was a function to create a solid from a closed volume but I don't see it, I tried to close the surface (it is open at the bottom) but nothing changes even after sewing the surfaces.

Does anyone know a solution.

thank you in advance

 


habillage_ferme.sldprt
2

 if you create a sketch from below and

that you project the sketch from above you will end up with the outer limits of your room 

and you do an extrusion to the surface

I think it should work

ps: I can't open your file you're in a version too recent for me I'm only in 2012

Post a screenshot with the Creation Tree

@+ ;-)

3

Hello

 

The surface must be closed, then sew and check the option to form a volume:

http://help.solidworks.com/2013/french/SolidWorks/sldworks/HIDD_DVE_KNIT_SURFACE.htm

 

Or use the fill function:

http://help.solidworks.com/2012/French/SolidWorks/sldworks/Filled_Surface.htm

4

Otherwise, there is no need to thicken or fill the surface to make the cutouts

 

It is possible to make cuts in surfaces with the "restrict surfaces" function from a sketch or a plane:

 

http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_FEAT_TRIM_REF_SURFACE.htm?id=6999f4a7586a4c88a433b5ddc99b155b

1 Like
5

thank you for the answers

GT22 I admit I don't understand your technique

Lucas I had managed to close my volume with the filled surface tool but even closing the thicken tool does not work beyond 0.5mm as for the sewn surface I use it to finish closing my surface however the form a volume option is grayed out...

 

6

On the sketch below that you are going to create, you take the outline of your piece, the outer limits

So you have a sketch with the outer limits of your part if you do a simple extrusion you should have the periphery of your part in elevation 

If you do an extrusion to the surface you will fill your volume 

Is it clearer?

@+ ;-)

1 Like
7

GT 22 my part looks like this, the walls are hollow I don't really see how to do it with your DSL method.


habillage.jpg
8

Hello

 

-If it's only to make cuts, I'll use Lucas' answer: "restrict the surfaces"

-If it's for something else, like Gt22, Create an offset plane on your surface and extrude a rectangle of clutter "all the way to the surface".

2 Likes
9

In fact, the surface is not clean

The best is to cut in half to keep only one side of the symmetry (if it's symmetrical)

Remove all surfaces from the inner skin and thicken 

 

I tried to keep only the outer skin, then thicken inwards

but on the capture joins the surface to a defect of junction

 

You have to spend time repairing the surface


surface.jpg
6 Likes
10

Hello

 

First of all, the thicken function certainly doesn't work because of the micro rays that are non-shiftable (I don't know if this word really exists...).

 

So either you try to unravel the surface little by little if it's not possible in one go, then create the contours and close the volume.

Or, if it's only cutting for openings (windshield, window, etc.), you might as well, as Lucas says, use "restrict surface".

The hardest part will be to find the ideal angle and therefore the plane to effectively dimension the cut.

 

Finally, "form a volume from a surface" exists under SW but only when using another function such as "sew surfaces, filled surface, etc.").

Without any prior modification, it is impossible to transform a simple surface into a closed volume (except by thickening, but it still has to work).

 

Good luck

 

2 Likes
11

I try the offbeat shot I think I understood.

As for keeping only one skin I tried, and I repaired the surface with the sew function but I have the same problem of thickening more than 0.5mm


habillage_simple.sldprt
12

Now that I see your part I understand a little more your problem

If your part is symmetrical, cut it in 2 and create an axial plane

make a surface shift outwards of x mm this will allow you to better see the defects of surface continuities

Take the outline of your part on  the sketch which is on the axis so you will have the silhouette of your part and if you fill in the holes in the windows beforehand you will end up with a solid body

(be careful to see if the bending angles are less than 90°)

on which you can take all your surfaces via an inter offset and work as you wish

 

@+ ;-)

 

13
Wouldn't it be easier to create a larger volume and cut it by the surface?? I haven't seen the part but it may be to be considered Kind regards Bastien
14

Thank you for your help to all unfortunately I don't have time to continue this afternoon I will keep you informed in the days to come.

thank you again

 

15

Hello

 

Here is the file in parasolid and in volume!

You have the interior and exterior surfaces so no need to thicken.

 

To achieve this, several key steps:

 

  • Diagnose the surface import to correct slight surface continuity defects.
  • Put the option to have the "open" edges of the surfaces in another color to see the areas to be corrected (here in your case: see image in next post)
  • Cut the parts in symmetry
  • shift the surfaces to be corrected (exterior and interior) to 0 and sew them back together with a slightly larger tolerance (0.01 in my case)
  • Replacing old surfaces with new ones
  • Create the Flat Surface at Symmetry
  • Create the filled surface at the bottom
  • sew up and you get to a volume.

 

@+

 


habillage_ferme.x_t
5 Likes
16

Here is the image again


capture.png
4 Likes
17

Bravo Coyote ...

I thought that the surface with too much flaw to be able to reconstruct a closed body

Congratulations I vote for you ...

2 Likes
18

Thank you very much Coyote!!!

I had more or less given up. I had just cut the piece and made thicknesses of 0.5mm inwards  and keeping the hollow shape.

If you kept the original solidworks file, I'm interested in seeing your creation tree.

thank you again

 

19

I have the file but we must not have the same version when I opened it in my 2014 it tells me that the file is in old version that's why I made a X_T.

 

@+

 

1 Like
20

OK indeed I'm in 2013 but I'm going to take a long time to move on to 2014 and I have it on another post to watch