Fold feature not on line

[Cadkunde.nl]

Hello,

I have a question about the fold feature.

Screenshots are in Inventor 2016, but its the same in 2022.

When using the fold feature to fold part from a line.

The face of the folded side is not in line with the sketch.

And I wonder why that is.

Its for a configurable model which changes thickness and material (and kfactor) of the plate.

After some calculating I found a formula for the offset from the line to the face.

angle = 90 degrees (1/4)

r = Radius to Bend centerline =Bendradius + Thickness * kFactor 

Offset = 2 * pi * r * 1/4 - r

Why is this offset? We expect the face to be in line with the sketchline. Whats the reason this is different

It's difficult to calculate this deviation. Because also kFactor is in it. You can't make a parameter equation. kFactor has to be found with ilogic, and changed on any update to be accurate.

Many thanks

[JDMather]

Is there a logical reason that you cannot model in finished form rather than using Fold?

[Cadkunde.nl]

Well the previous screenshots are from a test part.

The real model is made from a derived sketch.

Ofcourse you could make an extra plane and sketch to create it.

But we wanted to avoid over complicating the base sketch with the fold feature

[johnsonshiue]

Hi! This has come up from time to time. Basically, you already have the flat sketch but you want to create the folded part. The reason why the folded part may not 100% align the flat sketch is because of the K factor.

Inventor Sheet Metal workflow was designed to create the folded part and then generate the flat pattern for laser-cutting. In a sense, you are doing the reverse.

In your case, I would simply change the default K factor from 0.44 to 0. In this way, the flat length can be measured easily (K = 0 for inside length; K = 1 for outside length).

Many thanks!

[Cadkunde.nl]

Setting kfactor to 0 might do the trick since only 1 bend in this situation.

But if this question arises time to time. There are a lot more who try it, see result, and try other approach. Discarding this feature. Technically what inventor does is correct. But as a user your expectations are different, and you can really look weird at this for a while.

As a user you select a line and expect the bend to be on that line much like making flanges. Your first thought is not deviation from kfactor.

If there was a checkbox to ignore kfactor for the feature or something, user would have an option to get what they expect. Im sure this feature is used more often

Kfactor cant be adressed in parameters and in sketches without ilogic hassle.

Thx for reply

[johnsonshiue · Accepted solution]

Hi! You may create a custom unfold rule with K factor set to 0. Then either use it as a default unfold rule or use it on a per bend basis (override).

Many thanks!

[Cadkunde.nl]

Ye well the problem is solved, we changed kfactor and works.

But it took a lot of (unneccesary) time figuring out, and we couldnt solve it alone.

I think the fold feature is a great function that many engineers avoid.

Only because fold is missing buttons that the flange feature has.

99% of all flanges I have seen are created with the 1st or 3th button in the bend position group.

Flange works perfectly, Fold is preferred to be avoided as hinted by JDMather response.

Solely for missing buttons that make sense for the engineer point of view.

[JDMather]

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@Cadkunde.nl wrote:

Fold is preferred to be avoided as hinted by JDMather response.

Solely for missing buttons that make sense for the engineer point of view.

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I recommend avoiding Fold for two reasons:

1. Most engineers I have experience with have no real understanding of bend allowance and have not done proper calculations in creating their flat that they want to Fold. 

2. The customer is paying for the finished form - what are the dimensions in finished form.  Why not model in finished form to fit the assembly?  (I challenge anyone who insists of Fold to Measure their result.  Do the resulting measurements make logical sense.)

I have seen cases where Fold is appropriate tool, but in most cases it is incorrectly used.

[Cadkunde.nl]

I'm sorry, didnt mean to know your reasons as to why fold should be avoided.

I meant it more like this:

Flange works perfectly, Fold is preferred to be avoided as hinted by JDMather response.

Solely for missing buttons that make sense for the engineer point of view.

Instead of:

Flange works perfectly, Fold is preferred to be avoided as hinted by JDMather response.

Solely for missing buttons that make sense for the engineer point of view.

I agree fully with your reasons though.

Actually the buttons I mention in Flange that i see missing in Fold are more about finished form and not having to consider bend allowances.

[johnsonshiue]

Hi! I would not say Fold is something to avoid. It is just counter to what Inventor Sheet Metal is built for. As I mentioned earlier, the objective of designing a Sheet Metal part is focusing on the folded shape (an enclosure or a bracket). Then Inventor generates the Flat Pattern for you as the final deliverable.

Fold feature works the other way around. Essentially, you already have the Flat Pattern and you want to get the folded shape. That is tricky, because in theory, your design is done. You can cut the sheet using the Flat Pattern you already have. There is no need to fold it up.

Setting K factor to 0 is kind of like a hack in my opinion. It is because the K factor should never be 0 or 1, unless the sheet is extremely thin or extremely thick. Neither is the primary target in Sheet Metal design.

Many thanks!

[Cadkunde.nl]

Though I understand the reason now, I'm just saying it doesnt have to be the other way around only.

It could work both ways, same as flange.

99% of the time you work from folded result in mind. What now is called a hack could be a button how to calculate result.

But ye i stop ranting about it and for me its solved now. Thanks a lot