wide radius bends to flat pattern 2

[armsflailing]

Hi all:

I'm using IV 10 Pro and am trying to model a sheet metal bent into a parabola. I have no problem creating the part as a standard part, but then when I convert it to sheet metal and try to make a flat pattern, it gets all wonky.

I am not sure how I might go about this beginning in the sheet metal environment, or if that would solve the problem of creating a flat pattern.

Any suggestions or similar experiences and solutions would be appreciated.

 

[aardvarkdw]

Just some clairification, are you trying to a flat piece with a parabolic curve or a parabolic dish like a satalite dish?

 

[btrueblood]

I assume here that you are speaking of a two-dimensional parabola, not a dish.

Inventor's sheet metal tool assumes your part is formed from some number of fixed-radius bends thru some angle. A parabola, however, is a smooth function, and has a radius of curvature that is also a smoothly varying function. The closest that the sheet metal "solver" could come to getting close to the flat pattern would be if you approximated the parabola with a series of linked fixed-radius bends and straight line segments. Of course, the "formed" part that results would look "faceted" at whatever level of resolution you approximated the parabola.

In the real world, you wouldn't fabricate the part this way, would you? You'd make a best estimate at the male/female punch form, and bang the part with a bit of excess on the ends, then adjust the blank (flat pattern) to suit. If necessary, you'd then go back and re-cut the punch/die to get the final shape closer to the desired shape. I assume you are trying to make some type of aero fairing; remember you can also rely on the underlying ribs/support structure for the fairing to help restrain the part in its desired shape.

 

[aardvarkdw]

Inventor can create a true parabola, to my knowledge, only from a spline, and even that is not nessesarily a true parabola. And of course, the flat pattern tool has an aneurysm when it tries to flatten a splined entity. If a piece of metal is bent into a parabola, the deformation of the metal is distributed over the total length of the bend. There isn't a single point in which Inventor can create a bend line and this causes the error, as far as the program is concerned the piece isn't "bent" and there is nothing to flatten but it still sees that it ins't a flat sheet and it has a fit. Like Btrueblood said, sketch in the points for your parabola, as many as you can, and then create lines between the points. Then use the contour flange tool on the lines you just created. When this is flattened you will have a bunch of small bends and your bent part will look a little faceted but it is as close as you can get with a flat pattern. To properly show the flat pattern you will want to hide all of the extra bend lines.

 

[armsflailing]

Thanks for your responses.

It is a flat piece bent into a parabolic curve, not a dish.

When I created this in the standard part environment, I used a series of points generated from the mathematical expression I needed to create the curve I wanted and then created a spline through the points. It looked great for my purposes. I was trying to create this type of curve for two separate projects. One is for a bent laminate wood furniture piece and the other is for a concrete form.

I will try connecting the points with straight lines and see if I can do it as a series of bends and see how close I can get.

Again, thanks for your help.