sheet metal

[precision]

How can I bend the part attached with out bending the whole flange that protrudes beyond the bend.

I tried all fashions of bounding the bend line to stay to the projected part edge.

Thank You

[SBix26]

Oops-- works much better this way.  I've changed the dimensions so it's 5" inside and 1 mm bend radius (where is that specified?).  Now I get to a K-factor of .34, which is much more within normal limits.

Revised file attached (2021 format).

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Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[cadman777]

Nice work!

Bend Radius: Go back to 'MESSAGE 10 OF 41 - precision  in reply to: JDMather'

I'm curious how you accomplished it.

I see your model tree, but can't open your file b/c I'm on Inventor 2010.

[SBix26]

Hope that makes it reasonably clear...

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Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[cadman777]

Thanx for sharing!

Nice and simple.

I just tried it, and it didn't work.

Reason: The relief radius is .004" above the bend line.

Note: I'm working with the Blank the OP posted recently, which has a different profile around the circular hole.

To get it to work, I had to fudge the relief radius to .129" from .125".

Now it works, but with a Refold error, and it's not exactly the same as the Blank.

It's a few thousandths off all the way around.

[SBix26]

Yep, I don't think the drawing is complete and consistent.  There are things that are over-dimensioned, and things that are under-dimensioned.  I, too, couldn't make the part work with 1/8" reliefs, mine are 7/32".  This is more consistent with the visual from the drawing, but not what the OP specified.

I'm wondering whether a similar technique could be used starting with the blank as the OP wanted to do.  What if I split off the "ears" from the part, made the bend, then unfolded it and combined the ears back to it, then re-fold?  I'll try it and let you know...

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Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[SBix26]

I was able to successfully update my model with the 1/8" relief radius (mine was formerly 7/64", not 7/32" as I erroneously wrote).

However, I was not able to start with the blank, separate it into two solids, make the fold, unfold, combine the solids back into one, then re-fold.  Ended up looking like the OP's original problem with the folded ears-- unless I moved the relief radii just slightly down (.006").  Then it works. 

So, the procedure was to use Direct Edit>Move by .006" on the side with the 180° relief, and sketch and cut the other side to match.  Then it looks as it's supposed to, and measures exactly as the drawing shows.  2021 file that illustrates this procedure is attached.  Note that splitting the solid and later recombining is not necessary.  It works exactly as the OP desired, as long as the reliefs begin within the bend zone, not in the flat.

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Sam B
Inventor Pro 2022.0.1 | Windows 10 Home 20H2
LinkedIn

[cadman777]

Sam,

Thanx for clarifying, I appreciate it.

Not that I'm trying to belabor this topic, but .... 👺

I think there's confusion in this thread b/c the OP changed his mind part-way through.

Although I began with the original 2d drawing, he changed it to the flatpattern STEP file seen in 'MESSAGE 23 OF 46 - precision in reply to: cadman777'.

I wonder if that Blank will work the same as the 2d drawing?

Or maybe my version of Inventor won't work like yours?

Just wondering is all.

My version of Inventor doesn't have DirectEdit. Bummer!

Either way, seems like an awful lot of 'pain and suffering' to go through to make such a simple part!

[johnsonshiue]

Hi Folks,

I have taken this issue on and off for a few days. I don't have much to add except acknowledging what experts already mention. The tricky area here is the bend relief transition. To get the exact shape by modeling folded body isn't easy. You can get close but not exact. So, it largely depends on the need. If you want the flat pattern, you already have it. If you want to see the folded shape, you may as well start with the flattened body and add folds.

Many thanks!

[cadman777]

I agree with you Johnson: "on and off for a few days".

At this point, I'm finished 'massaging' this part. Suffice to say it's impossible to make on my version of Inventor, and I can't see what others have done due to the backward compatibility issues.

If this was my customer, I would tell them I tried to make this 30 different ways, and no matter what I did, it can't be made in my software the way they want it. So I'd present some concessions after discussing the essentials, and then offer a few simple, repeatable, easy to repeat solutions.

This reminds me of a job I had many years ago trying to make some crazy sheetmetal weldments that I finally made with the hybrid use of 3 different software programs. That was after 180 hours of work! The customer wanted it real bad, so I gave it to them, just the way they wanted it!

[johnsonshiue]

Hi Chris,

The only thing 2010 would not do in this case is the ability to define multiple solid bodies in sheet metal. On 2014 and later, multi-solid body may help a bit. You can get the bend transition by creating a trapezoid-shaped face on the side as a body and a long narrow face at the top. Then use Bend command to connect the two. Using this approach can get the nice bend transition.

However, it is like a hack. I don't think it is worth the effort to get around the problem this way just for the bend transition. Folding the flattened body will get there quicker.

Many thanks!

[cadman777]

You're right, I don't have sheetmetal multi-bodies in 2010.

But I probably wouldn't use them anyway.

I rarely used multibody parts over the years as well.

On one job I made some sheetmetal body armor for JK Jeeps using that same method you mention. After making one thickened surface, if the edges are 'tight' between the first surface and the adjoining surface, upon thickening the adjoining surface, a sheetmetal bend automatically forms between the two sheetmetal surfaces. I created most of the bumpers and fenders using that method. But first I had to create a 3d network of flat surface wireframes to thicken. Also I can use the bend command between two separate sheetmetal parts in 2010 if need be. But if I had my Drothers, I'd make sure Fold had better interpolability with the sheetmetal module. I have to say that the developers did a very nice job of adding some nifty undocumented (hidden) functions to the basic commands in Inventor 2010!