Sheet metal cutting

Hello, my first post here (even if lurking for some time)

I have a problem using the sheet metal feature in Solidworks 2007.

I need to build an object made like a squared "C" (or a square box
with an opening in the middle of one face, for the whole lenght),
about 50x50mm extruded for 1000 mm.

This is a quick scheme:
http://img135.imageshack.us/img135/4976/tempprofilosd5.jpg

At both the ends, this extrusion shoud be cut at 45°: i need that to
be made as sheet metal, since I want to unfold that and cut on CAM
machine.

I create the base feature, and all the sheet metal extension
("flange", since I am using italian version of SW), but when I apply
the extruded cut it just gives en error on all the sheet metal
features.

Any idea on how to do that?

 

create the (2x) 45 deg planes first (construction planes)
sketch base flange (complete profile)
extrude base flange, direction 1, up to surface, construction plane 1
extrude base flange, direction 2, up to surface, construction plane 2

hth
kenneth

 

It works, thanks a lot.

After posting here I achieved about the same result, by modeling my
piece as a thin solid extrusion and then converting the piece (with
extruded cuts) to sheet metal.

I guess the error came up when the cuts, running through the base
flange, produced a 45 degrees cut on the edge: it seems that SW can
simulate only sheets cut with standard guillotine shears, and has some
problems with partial incisions like the ones made by a milling
cutter.

Is it possible to avoid having the edges rouded automatically by the
sheet metal function?

 

no.

 

other options besides Ken's (which was just fine):

Design as flat and insert sketched bends (cumbersome)

Design oversize, unfold, cut across bends, fold (less cumbersome than
design as flat, better for design)

 

Sketch the "C", use Base-Flange with Midplane option, make a cut to
the other end, mirror cut. No problems here.