sheet metal box with two inclinations

[arzigogolo]

Hey, guys.

I am trying to make a sheet metal box with the bottom tilted in two different directions, one according to the x axis and the other according to the z axis, serving me of the respective side edges or banks as a reference, than which, the two sides of the sheet must be tilted.
the box is located at the beginning of a conveyor belt, and the two inclinations serve to ensure that the objects that are inside, converge all towards the exit opening that is located in the lower corner of the four sides (in practice the pieces go down by gravity thanks to the sloped bottom on two floors, xz and xy).

I wanted to try to do it first as solid and then convert it into sheet metal, and in fact the solid I made it as I wanted.
the problem arises when converting it into sheet metal; as first step I extrude the rectangle which will be the base of the box and then I deform the bottom according to the two directions.
the emptied holding the thickness of 1 mm, and lastly convert it into sheet metal.

done this, as next step, with the fold command (bend), select the outer edges of the bottom, one by one, to transform them into folds, and the problem is precisely this: once selected the lower edge of the box (the long or short side are indifferent), I appear the preview of the fold, but then when I confirm with ok, it gives me error and does not, and the message is this: "No corresponding face has been found."

I press that if the bottom is straight, then with the corners at 90°, the command works fine and converts me into fold all the edges of the box, bottom and walls.

in practice is the inclined bottom that gives him problems.

I point out that the piece I tried to achieve with solidedge following basically the same procedure (of course the commands are slightly different in the name, but the result is the same) and I did not have any problems, it seems strange to me that with inventor (which is the software with which I am more comfortable) I must meet these difficulties.

I'm probably wrong with something, and I just wanted to ask for your help to help me realize it.

in the attached image there is the piece until I managed to arrive (i.e. before using the command "piega (bend)" which fails).
I hope I could explain myself, but I'm here.

Thank you for your help. :smile:

 

[rf.infissi@libero.it]

I was curious about it and I tried it, I managed it but taking a little different road, because the problem, I think it's in the fact that inventor doesn't know how to handle the splits between the faces and gives you error in the blindfold command.

I'll tell you how I did it.

- I created the solid as required
- I copied the solid to the surface and suppressed the solid processing
-I then created a sketch for each face (projecting geometry) and turned into the face. you have to be careful when there are unions between faces not bent to create a offset of the line of a small distance (other than error)

If you want clarification, ask.


I aalego some img to clarify:

 

[Tarkus]

It's always been my method, only that I "stap" the solid, that is I eliminate the face that doesn't need, I cut the edges with a very small fitting, I give the right rays according to the rule of explanation, and then I thicken to "thick".

done.

 

[rf.infissi@libero.it]

I also noticed a small mistake to my example.
or it would be better to create the solid set it in a set and to make the sheet part adaptive, so that the sheet part varies when the solid changes.
all this to give meaning to the parametric and not fixed geometry

 

[arzigogolo]

Thanks to both of you guys, I almost managed! :smile:

I managed to create the sheet with the method described by RF.infixes, only that does not make me the development.
I look better tomorrow and try again.
but the sketches projected on each of the 6 faces, is it as if I drew an internal rectangle offset of any distance, type 0.008 mm?

 

[rf.infissi@libero.it]

no the offset must be minimum the value of the variable "minimum discharge" (it seems to be called vosis)
look at the image and see where they are arred with the offset,this because otherwise when you develop the lower edges they are stacked and it is normal that by mistake

 

[Tarkus]

Guardian:http://www.cad3d.it/forum1/threads/...ra/page3?highlight=sviluppo+lamiera+da+solido

 

[arzigogolo]

[

no the offset must be minimum the value of the variable "minimum discharge" (it seems to be called vosis)
look at the image and see where they are arred with the offset,this because otherwise when you develop the lower edges they are stacked and it is normal that by mistake

I did! :finger:

Here are two images attached to how I did. In practice I followed your instructions to the letter and, after some difficulties, I made it.
It's amazing because I didn't think that the "do" command if used in the way you described me, automatically generates the connection beams between the stems and the bottom of the box, I never used it this way and for this purpose, and that makes me glad because I learned something more.


The only thing that leaves me a bit 'delused' between quotes, and that I thought that to make a similar object there was a more direct and less arzygogular way to convert a solid in sheet metal, I thought that there were some commands a little more ad hoc to do so, without having to go through so different operations.

inventor is however the software I prefer and I know better between solidworks and solidedge because in some things it is faster and more versatile, always in my opinion obviously, and that's why I thought there was a shorter method to get to this result.
In fact with solid edge, once the solid is created, it is converted into sheet metal, and with a command you create tears on the 4 corners of the box with which you can already generate development.
I did it during a test that I did in a company, where they asked me to create this box with the sloped bottom using solid edge.

In fact, apart from this operation that I think can be done more directly, for the rest I prefer inventor in everything and for everything.
Do you think there's any other method to use with inventor? to me for now does not come to mind.
Thanks again anyway!