CAD Forum

​​​​​​​Hi everyone. I am dealing witha a problem some time ago. In my work, sometimes i have to design hoppers with twisted squares sections. (see image below). As you can see, the sheets metal components have two bends. coincident at one vertex.

Just in this coincident vertex (mark with a black circle in the attached image), solidworks can't solve it and return me an error. Until now, i cheat SW shifting one of the faces a bit. And then fixing the contour in AutoCad to send it to laser cut. This process is manually and waste some time in each part.

I have to say: I am conscient that to make this part as i want is "theoretically impossible" to manufacture on press brake. But the angles are low and we can make it with no problems in our workshop. So i am looking for a method to design this bends directly in SolidWorks.

Thank you!!!!!

If the assembly is welded together, a small gap in the bend lines crossing will enable SolidWorks to perform good. The remaining gap of 2 mm wide can be closed during welding.

Have you tried creating the hooper as a solid, then shelling it, and finally converting it to a sheet metal part? I believe that should work, and will probably make it a little easier to manipulate.

"Lofted Bend"
https://help.solidworks.com/2020/Englis ... D_BEND.htm

I took your original model: RED remodeled it: GREEN put them over top of each other in an assembly: (Close but not exact) Green model: Layflat of GREEN:

IMHO best way to fix it is like @Frank_Oostendorp showed:
But if that is not good, you could try editing the 2D Drawing. When I worked with sheet metal we used to attach a 1:1 flat view out from the drawing sheet so the guy in the laser machine would use it. I don't know how you do in your company, anyway:

I made a Edge-Flange, then in the drawing hid the lines and made a new one.
.dwg in e-drawings:
There might be better ways to edit the 2D drawing. I couldn't find how ^^



By the way, I would recommend to make the sheet metal using the native features for better bend control, k-factor changes etc:

Another quick fix for it. Delete everything past the Knit (Coser) and make the Convert to Sheet Metal.
It is possible to change the type and size of the Relief with the Bend Radius and the Auto Relief
Additionally, you could Flatten it and make an Extrusion to cover the Relief.
It will suppress when you un-flat

I don't work with these types of shapes, but I believe those who do start off with surfaces before using these surfaces as references for the sheetmetal creation.

The entire hopper can be done with one "Lofted Bend" and three edge flanges. It would be difficult to bend in one piece so you might want to cut out individual sections, 2 or more parts. Reduce welding... In my model I used Pablo's file only to get some dimension from. The loft sketches are open in the circled areas.

Dennis Bacon wrote: ↑Sat Jun 18, 2022 10:34 pm The entire hopper can be done with one "Lofted Bend" and three edge flanges. It would be difficult to bend in one piece so you might want to cut out individual sections, 2 or more parts. Reduce welding... In my model I used Pablo's file only to get some dimension from. The loft sketches are open in the circled areas.

image.png image.png image.png image.png

That's pretty sweet Dennis!