Problem creating a thickness on a part

3D Design Volume Model
1

Hi everyone

I'm looking to solve a design problem with Solidworks and I hope you can help me...
I currently have an extruded solid part (from a sketch by point clouds connected by a spline) but I would rather make it a hollow part (therefore with a thickness), however I have tried several functions: entity offset, surface offset, shell, etc. Nothing works...
This is a piece with a complex shape (see below), which I think is problematic because there is the tip of the ...

Do you think you can help me?

Thank you for all the answers you can give me.

Aurélie G.

2

If it's symmetrical, cut it. Redo your hull and then symmetry.

You may have less bp.

 

edit: and if it's not symmetrical but just extruded, resketch by converting the outer spline, offset to get the thickness, and then you extrude.

1 Like
3

Hello

The hull function should work. What's the problem?

It's already a volume, isn't it? No surface error?

See this tutorial: https://www.youtube.com/watch?v=v6NOIdhzrdc

Or the help page: http://help.solidworks.com/2012/French/SolidWorks/sldworks/HIDD_DVE_FEAT_SHELL.htm

2 Likes
4

Hello

Can you send your piece and say the height you want as well as the thickness?

5

and if for example you create  a room that is larger than your created room

and via the combined and subtract function you will have the mold of this said part, you will just have to create surfaces on this said mold and thicken them and come out of this said mold

@+ ;-)

6

What version of SW are you on?

The hull function works well normally.


2016-02-09__coque.jpg
2 Likes
7

Your tip must indeed be annoying to make it a thickness (you tried with shell tools with a thickness of 0.1mm for example. Or with a shell facing outwards by selecting the two side faces so as not to "shell" them?)

 

That said,  you should be able to get around the problem when extruding by doing a slim function. You can then choose a thickness and it should do it:)

However, it is at the time of creating the extrussion function that you can do it. You can't do it anymore if the extrusion has already been created

 

 


sans_titre.png
8

The problem is that it must have the shape of an airplane wing

A cross-sectional view is good but an ISO view is + meaningful

what version of SW do you have

or post your file in neutral format so that we can all work on it

@+

9

Hi everyone 

Thank you for all these answers and your responsiveness.

- I wanted to try the thin function but it doesn't appear in my extrusion function...

- The problem is that to create this piece, I used a point cloud with spline via data from a spreadsheet and I don't know how to create the same shape either bigger or smaller (because you would have to change each point data and I have a hundred...

- I work under SLW 2012,

- And I can't create a shell outwards because the profile created is my outward profile, I absolutely have to do it inwards .

- I'm going to try symmetry with shell (but I think my profile is not symmetrical...)

 

Aurélie.

10

post your file I'm under 2012 too ;-)

11

I'm under 2015, but at worst for me or the others we'll send it to you in STEP and you can use FeatureWorks to find the functions...

12

Hello GT22,

 

Here is my piece, thank you for your help.

A!ruélie


ag.sldprt
13

What room height and thickness??? Do you want a background in your room?

14

Here is your piece

didn't understand the problem

Sketch creation Convert entity offset That's it

attached file SW 2012

@+ ;-)


agd865.sldprt
1 Like
15

I would need a thickness of 7mm, how did you make GT22?

16

I specify that I am trying to shift the thickness INSIDE and not the OUTSIDE...

Indeed, otherwise the "shift entities" function works outwards...

17

7 mm will not be possible since the heel has a length of 3.001mm

but I find a walkthrough right away

 

1 Like
18

The point of the piece is only 3mm ext, it should be 14.5mm at least. Impossible to be 7mm thick...

1 Like
19

What is your process of making or producing this piece???

20

A solution:

You can shift the straight entity to get a straight line of about 14 mm:

Then, you create a dividing line, and you pass the shell over the long side, and there it goes:

 


ag.sldprt
4 Likes