Solidworks Fold

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1

 

Hi all.

I would like to make a fold.

 

According to the figure below, I have to make 3 folds (fold 1, fold 2, fold 3) to make edge A and edge B coincide. 

Is there a solution to make the A and B stops coincide directly?

If not, I have the sketched fold function: for fold 1 and fold 3 there are no problems. However, it does not apply to cover 2.

In short, I have to make a pyramid by bending the 1,2,3 edge and the coincidence AB will be welded.
Small clarification: I don't know the angles, but it doesn't bother me because I'll try to bend degree by degree to get the most accurate

Can a member please give me help and advice?

Looking forward to your feedback.

Sylvain.

2

Hello

If you use the Sketched Fold feature; you have to put a small hole (Diam 3) at the intersection of the 3 folds and there it will work.

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3

In general, we do the opposite 

We start with a finished part

and we unfold

c a hopper ?

what version of SW are you under

post your file so that we can at least take some ratings

@+

4 Likes
4

Hello to you,

Thank you for your answers.

I'm using SolidWorks 2018.

GT22, I understand that we start from a finished part in general. 

So that you can understand, the file is basically a pdf file, converted to dxf and converted into a sketch. It's a flat review of Papertrophy that I got in pdf on the web. I would like to model it to make it in metal. 

In short, it is a sketch that I have converted into sheet metal. 

 

AC Cobre 427 I did indeed make a small hole in the material (diam 0.5 by doing an extrusion with material removal but it doesn't work.)

I tried with a diam 3, and it works!!

Thank you!

I put the file in PC.

Yours sincerely

 

 

 

 

 


Part3.SLDPRT
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5

With a 0.5 Diam Solidworks doesn't know where to go with the material of the deformation of the folds, but with a Diam of 3 it is quite good in general but to be adapted according to the thickness.

6

Perfect thanks,

Regarding the coincidence of the two stops, do you have a tip please?

Thank you again.

7

Do your 3 angles have to be identical? If so, you just have to double click on the sketched fold function 3 and you and once the angular dimension is displayed you double click on it and the window appears and in it you put a = then you double click on the sketched fold function 2 and there you click on the angular dimension and there they will be linked then you do the manipulation of the sketched fold 2 to the 1. That way, if you change the angle of the 1st, the other two follow, and it's easier to get there, and if the 3 don't have to be identical, do the operation with the ones that need to be. Don't forget to do a CTRL-Q after changing the angles for consideration.

8

Or you can use the closed corner function which is found in insert==>sheet metal==> closed corner and you select the two sides and they will meet.

9

Wonderful ac cobra 426,

I'm trying that right away.

 

Thank you again.

10

Good evening Ac cobra 427

I have the impression that the closed corner function only works with 90° faces, and this is because in the case of @ czirnyj.sylvain you can't make a chamfer.

@tous

In any case, the sketch called "Model" and which defines the flat surface is in my opinion erroneous even if  @sylvain assures us that he has recovered the shape as it is.

In addition, Sylvain did not bother to redraw the sketch, which makes the modification of this shape more than sporty.

Obviously there are no odds and no constraints of any kind,  in short everything you need to do (schmurtzz) a good time.

What I see is that without a precise knowledge of the angles and especially of the junction dimensions with the other sub-assemblies which must also be in sheet metal, the probability of being able to make the entire mask is almost nil.

What I think is that in this case SW only does what we want from the moment we can give all the dimensions without exception and especially the angular ones in this specific case.

To show what I'm saying, I've made the piece with the most likely dimensions to show how to do it with basic folds that are the sketched folds already suggested by @ Ac cobra.

You will see in the attached image that the perfect connection can only be made with filling with TIG MIG welding, because the edges form an angle that is not 90°. I superimposed the sketch of the original "model" on the one I had to modify to get the edges to join.

I would like to point out that no angle is equal to another. (Precision mirrored to Accobra's suggestion to know the possibly equal angles)

Advice to @ czirnyj.Sylvain , you have to start from a complete volume.

Personally, I would do everything from multiple planes and a fully edged skeleton (much like we would if we were dealing with everything in surface before the full volume was created).
Then I would cut my model into a number of sub-assemblies (given the shape and that there is a perfect symmetry between left and right: two sub-assemblies three at most should be enough (this is because of the constraints on the bending machine)

But the easiest way is to make the 3D model from the skeleton mentioned above, then to make a single volume, then as suggested to make a hopper from a full 3D volume and transform it into sheet metal. (We dealt with this topic recently and the how to make a complicated hopper is very well described.)

There you go!!! but my colleagues and friends will give you other ways of proceeding.

Kind regards

 

 

 

 

 

 


masque_tolerie_explication.pdf
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