Creating flat patterns out of Swept extrusion

[Stugots]

We design heating elements modeled with a sketched path and round profile. Usually in "hairpin" type shapes. I need a way to be able to show these in a flat (unformed) state, and also be able to show stepped progression of bends for manufacturing instructions in the drawings. Any ideas?

It would be great if I could use the sheetmetal functionality of SW '06. Is there a way to do this?

 

[CorBlimeyLimey]

You should be able to do this with configurations.

Instead of using a sweep, extrude the hairpin shape (single line profile) as a Base-flange, but make sure that all bend angles are adjustable. The extrude distance should be the same as the material thickness. A swept square profile can be used but will need to be converted to a sheet metal part (Add Bends) and will create a larger file.

Apply full radius fillets to the edges. This config can be used for final pictorial views.

Create a new config and suppress the fillets. This should allow the new config to be flattened.

Create other configs (with suppressed fillets) to show the progression of bends required.

 

[Russell67]

I had this same issue in the past but with stuff that had only 2 bends and again the straight length was needed on the drawing. Because my part was round and it was a swept extrusion i created a formula that was

Straight Length = arc length + straight section + straight section.

"D4@Sketch1" = "D7@Sketch1"+"D1@Sketch1"+"D3@Sketch1"

I then added a custom property called Straight Length "D4@Sketch1". Make sure to add the quotes.

Because i still wanted control of my radius i dimensioned that and the angle between my straight segments. Staying away from parallel and perpendicular mates. All my straight dims were aligned, this way when that angle changed the length would remain unchanged.

To get the arc length dim what you do is start the dim command then select the arc section followed my the end points. This give the actual arc length as a simple dim. Mine was driven but i could still select it for my length it just gave me warning messages.

Then on my drawing i had a note linking to that property.

Also when i was creating my swept sketch i added a construction line with the equation so i could see the change in length at that point.

And as you add sections you can just update the formula.