problem creating sheetmetal part 1

[fireminime3]

hello, i am trying to make a rangehood in solidworks 2010. I am able to make it a solid and shell but not sheetmetal to get a flat pattern of the pieces. i have included pictures of what the shape is for anyone who can help. also the actual part itself. Thank you

 

[CorBlimeyLimey]

You will not be able to flatten that part as one piece.

 

[KirbyWan]

But it looks quite manageable as three pieces. The problem with sheet metal tools is they are geared toward short discrete bends such as a 90° bend with a .125" radius. The long sloping bends where you have say 45° with a 24" radiaus can be done. Don't start with a solid and shell it. start with a sheet metal feature such as a base flange or you lofted bend.

-Kirby

Kirby Wilkerson

Remember, first define the problem, then solve it.

 

[CorBlimeyLimey]

I just noticed that you used splines in the profile sketches. SW cannot use splines to generate sheet metal parts. The splines will have to be approximated using arcs and straights.

This limitation is probably due to the inability to create a true spline-form using regular sheet metal forming equipment.

 

[CorBlimeyLimey]

If you want or need to use splines in the creation of sheet metal parts, add your vote to SPR 570092: Ability to convert a spline in 2D into a sequence of arcs and lines in the SW KB.

 

[fireminime3]

Thank you for the replies. I have tried using arcs and lines to do a lofted bend, i have also tried to convert it to a sheetmetal part. none of which has worked. when i do a lofted bend i cant get it to have the slope that i need. Anybody have any more tips? of did anybody get a chance to play with it?

Thanks

 

[CorBlimeyLimey]

Does this help?

 

[CorBlimeyLimey]

Just realised you are still on SW2010.

 

[fireminime3]

Wow, okay that would help a lot. I cant open the first one and the second link is a picture. but thats pretty much what i am trying to do.

 

[CorBlimeyLimey]

Copy Sketch2 from your original file into a new part
Start a new sketch and trace over the spline with two curves connected by a straight line.
Use the Sheet Metal tool to extrude a SM part
Create an angled plane to use as a cutting surface
Use the Cut With Surface tool to create the cut
Use the Mirror tool to create the full front piece

Repeat similar process for the side pieces.

 

[fireminime3]

Where you able to flatten the part? on the lower bend for somereason i cannot flatten it.

 

[CorBlimeyLimey]

Yes I was able to flatten my part.

For some reason, your Base Flange had four base bends. It should only have two.

Edit Sketch2, delete the coincident constraints at the line end points, and make the line tangential to the two curves. Adjust the connecting points to better match the profile, and close the sketch.
The panel should then be flatten-able.