Cannot create standard sheetmetal lap joints using any method

[Anonymous]

I believe this feature would actually be classified as a hem operation in Inventor, however currently (2016) the specific geometry cannot be modeled either with Hems or any other feature.  Many of my customer's would refer to this as a "Lap Joint" or "Overlapping seam" in sheetmetal, and it is a common request from them.

The image above shows my closest attempt at creating the Lap Joint.  I've sketched an offset profile and attempted to use a Contour Flange feature to extrude the sketch.  Using this method, at least I get a preview.  However when I click OK to build it, Inventor errors with the following message:

I believe the issue at hand here is creating a flange wall that is parallel with it's attachment wall, and offset by a distance close to the thickness of the material causes two partial bends with not enough distance between them for Inventor to create a straight segment.  This is clearly visible in the image above.  (Notice the "S" shape of the contour flange)

This is a basic sheetmetal construction method used commonly in many sheetmetal boxes and enclosure fabrications.  I've been asked by numerous people how to create this particular feature in Inventor, and to date I've not found a solution within sheetmetal that accomodates it.  Users typically "fake" this into sheetmetal parts by reverting to solid body modeling tools.

Typically a Lap joint has one wall bend under another overlapping one.  Sometimes both walls need to offset (one 1/2 material thickness upwards, the other downwards) to create a nice seam.  Ideally, a Hem operation should be able to slightly offset the edge of a wall, without actually bending it, to accomodate this need.

[Anonymous]

Hi

Look at this video from about 6:25.... 🙂

https://www.youtube.com/watch?v=4NdE1xh_UrU

[Anonymous]

That is close, but not exactly what I'm after.  I'm looking for a new command (probably a new Hem style) that can provide the results above with a couple selections and a dialog box.  Creating these types of features using flanges of any sort is akward and unpredictible.

-Jim

[AlexanderVokes]

Try making your contour flange sketch without curves, and replace them with a 45 deg angled section so that you have a Z-shape instead. If your bend radius (sheet metal style setting) is too large it will still fail, but you can angle the line more to compensate. It does need a straight section between the bends but at least in this way the feature works.

[Anonymous]

I've been making these type of lap joints since version 2008 without ever resorting to solids. Like Alexander said, don't make to contour flange sketch with a radius. If your material is .062 inch thick, sketch from the bottom of the start feature straight out say .125 angle down at 45 deg to .063 below the first line and then staight out another .125". Contour that profile using the bottom edge of the original feature and you're done. From the opposite edge of the original flat feature you can create a series of standard right angle flanges (clockwise) to get your 360 degree part modifing the last joining flange length to come just short of the lower offest radius.

[Anonymous]

I appreciate the tips so far, my request for a feature is only highlighted by the recommended hoops people jump through to make these features.  I would like to see this as a placed feature, similiar to a Hem, that can be assigned from a dialog box by selecting an edge and a surface to fold it under, plus some dimensional parameters for overlap and offset...etc.