lamiera curva e fori

[lelecup13]

hi to everyone, I tried to find something inherent in my problem but I found nothing:frown: I have what I have to do and I can't do:

Starting from a flat sheet, I have to bend it by giving it a certain radius of curvature.

Later on on this curved sheet I have to make holes at a determined distance from each other.

How can I do that? thanks in advance

 

[Ilario]

the curved drawings and make the holes, then develop it later.
or flat drawings, holes, then pieghi.

but if you do not specify the version of inventor, your level of preparation, the specifications of the sheet and holes, it is difficult to help, because as you exposed it seems that a real problem does not exist...

 

[Tarkus]

hi to everyone, I tried to find something inherent in my problem but I found nothing:frown: I have what I have to do and I can't do:

Starting from a flat sheet, I have to bend it by giving it a certain radius of curvature.

Later on on this curved sheet I have to make holes at a determined distance from each other.

How can I do that? thanks in advance

to understand better:
In reality, first, cover the sheet and then do the holes so that the holes remain cylindrical and not deformed by the bending if you reverse the working cycle?
Are the holes equidistant and related to a rectangle or polar series?
Is the axis of the holes perpendicular to the surface of the sheet?
If you could post a file, even autocad is fine, you could be more accurate.

 

[lelecup13]

the curved drawings and make the holes, then develop it later.
or flat drawings, holes, then pieghi.

but if you do not specify the version of inventor, your level of preparation, the specifications of the sheet and holes, it is difficult to help, because as you exposed it seems that a real problem does not exist...

Okay, I'll try to be more precise.
I have inventor 2008, I haven't used it for a long time and I have to make a sheet with development 690 mm and has a radius 5300 mm. I don't know what command I have to use to fold the sheet with a certain radius and how to make holes later.

Sorry about incompetence again, I imagine it's a simple thing, but as I said before I use inventor recently. Thanks again

 

[Tarkus]

Okay.
I have 2009 and if I give you an example file then don't open it, so I try so
sheet metal environment:
in fashion sketch:
1)designate the curve of the sheet that you need to realize, adding to
an end of the arc a small straight line (even 0.1 mm), with the arc itself.
2) exit the sketch, set the sheet module on the thickness you want to use
and through the border flange command, create the sheet of the height you want.
3) Now start making a sketch on that little face of 0.1 mm that you
it was created at the end of the arch; it is always in sketch, if you expand the
command "project geometry",under you find "project flat model",click us
and then click at any point of the curved surface of your sheet.
you create a profile that is the development of sheet metal.
draws in this profile all holes, or sunshades or any closed shape
you want to get.
4)close the sketch and click on the "cut" command;choose drill profiles that
you want to get, quit the flag "through fold", and finally give the ok.
Here you are your curved and perforated sheet.:biggrin::biggrin:

 

[Tarkus]

I add that you create holes deformed by the next curvature.
If I had to file them, for example, they're not good.
in this case you have to create a tangent plan at the curvature where you want to make the hole, and then do a sketch where you create the warp center, then you can use the normal "hole" command from sketch.... .