Problem with unfolded view that does not correspond to reality

2D plans Layout
1

Good evening to you.

I made a plan for making a basket for work, and I wanted to have it laser cut, and then have it bent, at a professional in this kind of thing.

He tells me that my unfolded view is wrong...

I guess it's true, but despite his explanations, I can't seem to make it stick. 

His explanations were.

If you want to make a square of 100*100 (outer sides) thickness 8, your calculation is as follows:

100+100-2* the thickness which gives us 184 mm.

I managed to unsign it, its square and my unfolded glue by putting the radius at 8 mm and the K factor at 0.28.

it works for a square, but I want two folds, in the shape of a "U" if you want, so the calculation would be 100 +100 +100-3* the thickness??

I can't...

I attach the cart file and then the drawing since I can't put two files.

Thank you in advance for your help.

Lucbirus


cart.sldprt
2

there you have the MEP.

Thank you


cart.slddrw
3

Hello

You have to remove ±4* the thickness (±2* the thickness per fold) there you should get there.  (23-3)+(3-911-3)+(23-3)=945 basically if you want it's ± = on the inside sides so in your case 20+905+20=945 so your dev is right....

1 Like
4

For a thickness of 8mm you should not work with the K factor

Try to work with crease loss.

 

This loss at the fold will be equal to 2/5 of the thickness.

 

For an angle of 100x100 we will have 100- (e/3*2) +100 - (e/3*2)

or 100-5.3+100-5.3 = 189.4

 

for a U, it's the same thing, remove 2/3 of the thickness per wing

100+100+100-5.3-5.3-5.3-5.3 = 278.8

 

To fold this dough I use a 100 V with a radius of 17mm

 

To sum up, put loss at the bend = 2/3 of 8mm so loss at the bend = 5.332

 

EDIT: For the loss at the fold, it's 2x 5.332. as much for me.

2 Likes
5

Hello AC Cobra 427.

thank you for your clarifications; I'm going to review my plasn tonight and maybe try to send them for correction to the folder, just to see if it's what it's worth and that for future plans, it's fair.

 

hello Bart.

So I understood at first but your calculations, I'm not too much.

When I take back your calculation:

For an angle of 100x100 we will have 100- (e/3*2) +100 - (e/3*2)

or 100-5.3+100-5.3 = 189.4

Can you explain to me where this "e/3*2" comes from? Thank you for your efforts.

a+

Lucbirus

 

 

 

6

For each wing, 2/3 of the thickness must be removed.

To remove 2/3 of the thickness, I do -(e/3*2) or if you prefer -2/3e


para_tole.png
7

Hello

Folding, a vast subject. To make a good press there are x rules to follow. It is necessary to take into account the material, the fiber direction, the machine, the vee, the punch, the bending angle, the thickness ........ the rule is the sum of the outside dimensions + delta " L ". The delta " L " and depending on the vee, thickness, bending angle, punch. To find them I attach a table which should normally be the one on your machine but tampis the one will do.

May the force be with you.


calcul_de_ld_pliage.xlsm
2 Likes
8

 stole something to play.

may the force be with you.

 


presse_plieuse_developpement_delta_l_dossier_ndeg1.pdf
1 Like
9

For Bart:

ah ok I understand better, thank you very much.

 

Hello OBI WAN

Wow, indeed there is something to have fun with, and to understand even better. I'm the type of person who assimilates drawings or videos better than texts that are too long. but thanks to those who in the background (of texts) too.

It's clearer in my mind, knowing that I'm going to put these docs aside, for my future cases.

I'm going to do a few applications tonight if I have time, just to assimilate all this.

 

Thanks to you guys, you're great, but you knew that, didn't you?

a+

Lucbirus

 

1 Like
10

The best thing would be for you to tell us what type of folding machine you have as well as the tools.

 

that will allow you to guide you as much as possible =)

 

If not, who has the right developed? =)

11

So the folder tells me this:

To put it simply, when you bend a thickness with the appropriate Ve, there is no correction to be made.

 

We will always unfold the inside sides ...

 

 

 

Example:

 

For a 100 x 100 external square in 8 mm thick,

We will take a Vé of 8mm x 8 = 64

And the developed part will be 100+100 – 2x the thickness = 184 mm

If I use another EV for any reason, it's up to the bender to make the necessary changes

 

 

12

I know that the folding rules are very difficult and it really depends on the folding machine used.

Is it done in-house or is it outsourced externally? For my part, the parts are subcontracted and in this case, I don't put the unfolded of my parts. It's up to the folder to put the dimensions he needs according to his material, but I attach a step of my parts so that he doesn't have to redraw everything if he needs to start from a 3D.

Then if it's done internally then you should see the board associated with the folding machine used, as indicated by Obi Wan. In solidworks, you can indicate the bend loss instead of the bend factor. I've never used it but let's see if your unfolded follows properly afterwards.

3 Likes
13

If we follow the logic of your folder, the press will be about 267...

 

As a folder, it seems weird to me but hey, I don't have 20 years of experience in it =)

14

Just I would like to react to what @nathalie-1 said, she is right, if you subtract, don't give development, it's her problem. If you give a devellopè you engage your responsibility in case of a bad part he will say that it is your fault, don't forget you order a finished part the way to make it is up to him.

+1@nathalie

May the force be with you

 

 

15

So basically it comes back to what I wrote in my 1st post. Basically, you have to take the inside ribs...

16

I disagree.

 

If we follow this principle, it would give 100-8+100-16+100-8 = 268mm

 

I'll pay you cherries if you manage to make a U of 100+100+100 with a developed of 268. I'd like to see the result.

 

We are subcontractors in bending and I deter when a customer gives me a false press. The best way to be sure of the unfolded is to give the desired dimensions to the folder so that he can do the press himself or to make a good press directly =)

1 Like
17

On 8mm I agree but up to 5mm it's +- in inner ribs to 5 tenths and these tenths are ridiculous because if the sheet metal is harder you will have a smaller radius so you will lack material and if it is more molten you will have a larger radius and extra material.... And moreover the material tolerances are at chi... because you can very well be delivered in 3mm or 2.8 or 3.2 and it's still within the norm...

18

Yes, I have my cuts and piages done by a specialized company, that's why the manager told me that my devellopés were fake. I imagine that he must return the DXF files before giving this in prod..

For the rest, I will indeed not send any more developers. I'll see if it disturbs him or not. I thought it was a lower quote, since he has nothing to do... but maybe not.....

I'm going to see this detail with him directly.

But what I'm going to do from now on is to dimension the inside and no longer the outside ribs, for everything that is sheet metal bending, if that helps...

19

I find that sheet metal work is very technical when we have not studied it (in BTS CPI for example, we do not see the notions of sheet metal). And despite good will, sometimes you have to let the specialists do things. For my part, to have my developing checked, I learned to calculate my dimensions at the level of the neutral fiber, on the other hand at that time you need to know the bend radius.

I worked for a company where we did the cutting and folding in-house... Of course, I was lucky to only work on very thin sheet metal and with only one bending machine. But this is not always the case and depending on the machine or the Vé to use your odds are not the same.

For a job well done, I think it's better to pay a little more to the subcontractor (and I don't think he takes a lot more because he'll only do it once on your part) than to spend hours finding the right dimensions to develop it. And then if he has to touch up the dxf, then in his quote he necessarily provides a little margin for it. When quotating, don't forget to set the minimum bend radius either. .

2 Likes
20

Of course, bending on thin sheet metal and thick sheet metal is not the same.

 

We have 2 folding machines, one with a press and one with an apron.

We bend from 0.63 mm up to 10mm.

I use the K-factor method for sheet metal up to 4mm. Above this thickness I use the crease loss.

 

Whether you give the inner or outer sides does not change anything for your subcontractor as long as it is indicated "interior or exterior", he will calculate the developed himself according to his tooling