Bending/Rolling Sheet Metal With Features from a Flat Pattern "Face".

[IST-WK]

In the real world, sheet metal of varying thickness and features exist that can be formed by pressing, bending, rolling or formed using other tools of the industry.  In Autodesk Inventor - apparently - the only sheet metals that exist are flat sheets that can be flanged, etc., or sketched profiles that can be "contour flanged" or "rolled contour flanged" into existence.

I would like to see Autodesk engineers make the sheet metal environment more robust, and be able to shape sheets in the software, like one can in the real world, by rolling, pressing, bending, and free-forming.

The example I am using here is a piece of 304SS Perforated Sheet Metal, which needs to be bent, and then rolled into shape.

Autodesk Inventor apparently doesn't like holes in sheet metal where bending and forming are concerned.  I've drawn the flat pattern of the part in question, and made a sheet metal "face" out of it, then added the hole pattern as laid out by the manufacturer of the particular piece of commercially available perforated 304SS.

Now, the idea, is to create a part that looks like this:

Currently, if you take the "Flat Pattern" file and try to fold or bend it at the blue line, Inventor has no idea what to do with this, let alone try to roll it into an inside diameter of 1.625".  I put Flat Pattern in quotations here because this is not an actual flat pattern derived from a rolled part.  This is a flat sheet, with the features I need (The perforated hole pattern), that I want to bend (The round area),  and then roll (the rectangular area).

It would be REALLY nice if Inventor could pull this off.

Regards,

William Kumler

Impossible Bend and Roll.ipt

[mikeh4]

If I'm understanding your correctly you want to be able to form perforated sheets.  You should be able to fold/roll perf'd panels of your drawing your bend line correctly 

In your 1st image I pretty sure your issue is the blue line sketch has to end on the edges of the part.  The end points of the blue line have to be constrained to to the edges of the part.  That should let it fold even with the perforations.  See Attached file and edit the fold feature and check out the bend line sketch.  Guess I can't add an attachment to someone elses Idea.  I could email direct to you but provided some images.

As for the 2nd feature of rolling it you should be able to that with the same resolution as above it's just that you have to do it in 2 folds by sharing the bend line sketch and fold it twice for 180 degrees.

I don't thing the issue is the perforations it's the combination of the 2 feature of a bend and roll on the same section of material.  If you use solid sheet, no perforations you'll have the same issue.

Curious what step you do 1st bend then roll or roll then bend?  I think the issue is in the final part where the bend is.  That is not simply a bend it is material being stretched and thinned out because your bending in 2 directions so in terms of the material it's more equivalent to stamping which is pulling and stretching the material in 2 directions.  I think for the software to do that they would need the mathematical equations needed to calculate that.  Throwing the perforations into it really complicates that.  Any way to provide the match for that?  I don't know how to do that math, but to bend or roll independently that's easy math.

Have you tried to unroll create a flat of your finished model image 2?  My guess is it won't unfold that for the reasons in the paragraph above in stretching material in 2 directions.

Not negating your idea, just sharing some thoughts.

Regards

[IST-WK]

Hi @mikeh4 ,

I agree that there is some seriously complex mathematics involved in coding this kind of operation, but that's what Autodesk pays their engineers for! 😉

As for the question about what step I would take first bending then rolling or rolling then bending?  I would bend the sheet first, then roll it to the desired diameter over a mandrel or tube of the desired diameter.

I made an edit to the original file I attached, and shortened the "neck" of the area I wish to perform the bend operation at, and then extended the blue fold line out to the projected edges of the sheet metal's rectangular area, and attempted to fold it with the same result:  Nothing.

I tried to use both construction and actual linetypes for the sketch entities, but there is no fold operation:

Maybe I'm doing it wrong?   Inventor 2023.1 Professional refuses to bend this part.

Edit - Okay, so I projected the edges of the "neck" and trimmed the bend line to them:

This resulted in the bend operation performing successfully:

I suppose now I need to figure out how to roll it properly.

[mikeh4]

If you can post it I can give it a try.  Looking at the last image I'd try to put a sketch on your flat face and draw a bend line down the center of it and extend it to the bottom of the tangent of the bend and see if you can do a fold feature?  my guess is a fail, but that's what I'd try.

[IST-WK]

I suppose this is a teachable moment! 😁

Okay, so after playing with the sketch a couple of times, I was able to achieve the desired result...   Albeit with one glitch that maybe Autodesk can try and solve???

This is the sketch:

...and after bending twice using the sketch as a shared sketch, and the fold option set to "start of bend", this is the result:

Here is the "glitch" I am referring to:

While it's very small, and you really have to zoom-in to see it, it's there... and I suppose that Inventor is interpreting the bends the best that it can without failing the operation entirely.  Adjusting some sketches might yet yield a cleaner result, but, I guess that in the end, I learned something today.  😆

I appreciate your help, and thoughts on this @mikeh4 .  *cheers*

[mikeh4]

Awesome - To be honest I had my doubts that it would not do the roll, expected a error couldn't build, or just wouldn't give you a result.  But ya if they could blend that out with like a loft that would be sweet.  I wonder too if the perforations were shifted if it might throw some errors like if a perf hole landed on the bend leg which would be on the left side of your red oval in the last pic.  Another way to put it is if the circle landed on the edge of the bend.

Your welcome

[IST-WK]

So, after making this part the "correct" way using the above methods, I discovered something that is...   well...  bizarre.

I cleaned up the "glitch" using a bunch of different fillets just ro make it look nicer.  But then, when I told Inventor to make a flat pattern out of this part, it did something totally unexpected since I started out with a flat pattern to begin with.

Here is an Isometric view of the Flat Pattern that Inventor 2023.1 created from this part:

...and here's the Front View:

Bizarre, right?  Notice that in the design heirarchy, I have taken all of the fillets out of the equation by moving the EOP to the last bend.  One would think that the result of the "Flat Pattern" command would be to take the part back to the result of the first 4 operations, as that is the actual flat pattern.  Instead, it created this.

@johnsonshiue    What do you think is causing this?    I've attached the part file for you to inspect

[Edit] It seems I cannot upload the current version of this part file to this discussion...  [/edit]

Thanks!