Solidworks Flat pattern

[AdrianBy]

Hi

I am struggling to flat pattern this part.

I am attempting to convert it to sheet metal by inserting a bend, but it doesn't let me. Would anybody have any ideas?

Thanks for any help, its greatly appreciated

 

Adrian Main Body in 2mm SS 316.zip

[shift1313]

Adrian, that part is not something that will work for "Convert to Sheet Metal". it is meant for things like solid blocks or bodies.

 

You can use Sketch1, which is under-defined by the way and should be fully dimensioned, as the Base Flange/tab, but that won't let you flatten it. A rounded part like this is less of a "flatten" and more of a "form" type operation. To make this work you need to do a Lofted-Bend, but your sketch will need some adjustment.

 

1. you need an open sketch with smooth edges. If you are drawing the inside or outside edge make note of this because you will need to add fillets to all the sharp corners.

2. you will need a second profile for the loft. Simply make an offset plane your distance(1150mm is what i used) and "Convert Entities" to just bring the same sketch1 profile into your new sketch.

3. Define how many bend lines you want.

 

I opened it in 2015 and said the file was a previous version. depending on the version of Solidworks you have, the tools have changed a good bit. I attached two screen shots to show you the formed and flat pattern.

 

In 2014 (I think) Solidworks added something called "Surface Flatten" on the surface tab. This allows you to select complex surfaces and get a "flat pattern" of it. Mainly used for things like composites or even making decals. Just remember a part like you have here is "rolled" or "formed" and not bent in the normal fashion which is why SheetMetal functionality doesn't really suit it.

 

[AdrianBy]

Hi Shift1313

I lofted/Bent the sketches and it works perfect.

Thanks for taking the time to reply:)