Flattening a swept helical part

In the case of having to model a sheetmetal "rail" with a helical profile, one is left- oftentimes- trying to model a cylinder, unfold it, and cut away excess material only to find that it fails to re-fold correctly. However, there is a suitable case where a user can model a helical sweep, insert bends, and unfold it for the purposes of adding features. But let us first look at what defines a helix as well as a sheetmetal part.

The helix functionality of SolidWorks is an inserted Curve and is created from a simple, planar sketch of a circle. The options to create and control the helix include:

1. Pitch and Revolution- the number of revolutions by the over-all pitch of the curve
2. Height and Revolution- the over-all height and number of total revolutions of the curve
3. Height and Pitch- the over-all height and total pitch of the curve and
4. Spiral- a 2-D/planar spiral controlled by the total number of revolutions.

The outer diameter is controlled with the intial sketched circle. The pitch is defined as the total linear travel divded by the number of revolutions. So, for example, a height of 4in and pitch of 8in would result in 1/2 of a turn (180 degrees of revolution).

And this is paramount because, in order to flatten a helical swept feature, the pitch can not be less than 1/2 the over-all height of the curve and can only be whole, constant value multipliers. Or, in other words, in a curve with a height of 4in and a pitch of 8, the pitch may be set to multiples of 2x, 4x, etc. This, however, will allow SolidWorks' sheetmetal functionality, Insert Bends, to create a valid sheetmetal part that may be unfolded to the flat pattern.

When a non-sheetmetal part has bends inserted, assuming SolidWorks can unfold it, two types of bends are created: Flatten and Process. The Flatten Bends do just that: they flatten the part. In the case of a cylindrical or a helically swept part, the Flatten Bend type is a round bend.

A sheetmetal part is also defined by or controlled with what is called the "k-factor." This value differs by material type, gage,  and processing. But, to simplify the definition the k-factor is the neutral acis situated within a bend. There are excellent resources on-line at both www.sheetmetaldesign.com and www.sheetmetalguy.com; I'd encourage you to visit those sites.

Lastly, in order to create our helical part, we need to sweep a closed profile that is designed to the thickness of our material. This profile is swept about the helical curve we created.  Sheetmetal bends can be inserted after the sweep creation and additional cuts can be added after folding and re-folding. Click here to download an example file.

Comments

[matt]

That's one way to do it I hadn't considered. That uses the "old school" insert bends method.

I've had some sample models on my site for a couple years that use the "new" sheet metal techniques.

http://mysite.verizon.net/mjlombard/

Go to the SWParts link and scroll down to the "Things you shouldn't do with sheet metal" part.

The part there has a more complex technique to do an elliptical helix. The basic idea is that you create the edges of the part and do a Lofted Bend. This method uses an intersection curve made from two surface bodies, but there are a lot of ways to do it.

Thanks for showing your method!

[harpreet]

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