Coming (Very) Soon! New Sheet Metal Features!

[excitive]

I am on the Experience Design team for Fusion 360, and I would like to share an update about a new feature we have been working on. It adds new capabilities in the versatile set of Sheet Metal commands of Fusion 360.

Currently, the primary way of creating Sheet Metal parts in Fusion 360 is by creating flanges, which requires you to pull the edges off of a sheet and set parameters to get it to desired shape. With this new command - Bend, you will be able to easily bend the existing material along a sketch line. It will be a great aid for those who need to bring in an existing flat pattern in formats like DXF and create sheet metal components out of it.

Following animation gives a sneak peek into the easy workflow for Bend:

Bend in action

As you can see above, we have taken extra care to make the experience as simple as possible. For example, the bend side - i.e. which side of the bend line will be bent v/s which will remain stationary - is determined automatically depending on where the user clicks on the body. The side where you click remains fixed and the other side bends.

As soon as a face is picked, the selection automatically moves to next item and Fusion waits for the bend line to be clicked. This means that once you have a sheet metal body and bend lines ready, it will take only four clicks to create a bend.

Another cool thing about this command is how smart it is. The bend lines need not precisely touch the edges of the face. Our developers have worked hard to make it smart enough that even if the bend line is partially covering the face, it understand whether to bend it or not. This is particularly useful in DXF imports where coordinate precision is not guaranteed.

Stress Test

Additional options are provided for direction (up or down) and angle. Bend also takes care of creating necessary bend reliefs, which you can disable if necessary. Override mechanisms will let you alter certain properties of sheet metal rules.

Bend command UI

We are super excited to see what our customers do with this. Do you think this will be a good addition to Sheet Metal features in Fusion 360? What improvements should we make in upcoming updates? Please feel free to share your comments and ideas, with any feedback once you have played with it.

Bend comes out soon in the March 2019 update of Fusion 360.

Cheers!

[TheCADWhisperer]

I am able to open the latest attachment.

[Anonymous]

New bend bend tool is great thank you.

Just wondering why the inability to set a bend angle of exactly 180 deg. (It will let me do 179.99999... deg)

[excitive]

Hello @Anonymous

We are working on Hemming functionality separately and integrate it with existing Sheet Metal commands in Fusion. Once we're done with that, you'll be able to create hems easily. The current logic for Bend is more optimized for bend angles that are not 180º and hence it is blocked. You will have Hem soon! 🙂

[Anonymous]

Nice one! Any idea when developable shapes will be possible for boat building applications?

[excitive]

Hi.! Can you please share little more details on what specifically you are looking for? We can help you identifying features and workflows to accomplish that. Thanks!

[chrisplyler]

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@excitive wrote:

Hi.! Can you please share little more details on what specifically you are looking for? We can help you identifying features and workflows to accomplish that. Thanks!

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I'll bet he's looking for compound curves, such as might be formed by stamping, hammering, rolling on an English Wheel, etc. Which I'll assume is probably the very last thing the Fusion team will work on after it can wash dishes for us.

[TheCADWhisperer]

See Unwrap command - Autodesk Inventor Professional 2020.

https://help.autodesk.com/view/INVNTOR/2020/ENU/?guid=GUID-8126E8EE-422A-4DEF-9B14-513D87BD4122

[Anonymous]

A developable shape is a curved shape present in the form of most boat hulls that has been  created from a flat sheet. They are called developable shapes because despite them being curved over multiple planes, without distorting or compressing the sheets of steel or alloy, they can form the desired shape. There are a lot of CAD programs out there with this ability but fusion does not.

Google: "In mathematics, a developable surface is a smooth surface with zero Gaussian curvature. That is, it is a surface that can be flattened onto a plane without distortion. Conversely, it is a surface which can be made by transforming a plane. In three dimensions all developable surfaces are ruled surfaces."

[Anonymous]

As mentioned clearly, im looking to create developable shapes, common in boat building (google it). This is the complete opposite of what you are calling "compound curves" which are formed. Please don't post silly assumptions before reading, more often than not it leads people in an ill advised direction when trying to get support on a function. 

[chrisplyler]

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@Anonymous wrote:

As mentioned clearly, im looking to create developable shapes, common in boat building (google it). This is the complete opposite of what you are calling "compound curves" which are formed. Please don't post silly assumptions before reading, more often than not it leads people in an ill advised direction when trying to get support on a function. 

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I did not say that you are looking for compound curves. I said that I'LL BET you are looking for compound curves. If I was wrong, that's fine.

I'm going to keep posting 'silly assumptions' when I think they might be helpful. Deal with it. Occasionally my assumptions are going to be wrong. And when they are wrong, somebody corrects me and nobody runs off in any ill advised direction.

[safiredesignengineers]

Hi  is it possible to use this new bend feature to check that a part can be bent in a brake press without hitting tools or stops etc...  i.e can i import my male and female press tools and modeled stops into the same cad file so that when i use the bend tool i can see if it hits the tooling etc?

[TheCADWhisperer]

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@chrisplyler wrote:

Bump is right, right? Now the seeming hesitation has me wanting a response too!

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@chrisplyler 

I have a challenge and a box of doughnuts for you.

Model the part from attached drawing from a flat using Sheet Metal Fold Bend functionality.

I'll make it easier for you - do the easier Example 2.

Set timer before starting (just for fun, the doughnuts are not contingent on time).

[chrisplyler]

Oh, sure, make me edit the default rules. Thanks.

Okay, I tried it. I see your point. Well, I see a problem that I assume was your point. What a giant mess!

There should be the ability to designate the bend lines as "outside" or "inside." Using the "start" "center" "end" options doesn't seem to do the same thing. As it stands, you'd have to do a whole lot of K-factor math to figure out where you need to put your bend lines to get the desired result. What a nasty implementation.

Even my suggestions would only solve the problem for the first set of bends out from the center. Dimensioning the SECOND bends out from center, dimensioned from the first bends, wouldn't be out-to-out anyway. It would still be a mess.

[excitive]

@chrisplyler @TheCADWhisperer 

Let me get this reviewed by the team, in the meantime it'll be great if you can elaborate more or share some "expected v/s encountered" kind of example, as this looks like pretty specific issue.

Cheers!

[TheCADWhisperer]

@excitive 

Find someone experienced in sheet metal.

I am messing with  challenging you.

Nobody designs by bending up a flat sheet (try it - I already provided a trivially simple example in Post 32, I can simplify it even more if it is still too challenging).  The proper way to model a sheet metal part is to model in finished form and then calculate (or have software calculate for you) the correct Flat Pattern.  (That is exactly how you generated your example file.)

If you try to model in the reverse direction (design the flat pattern first and then bend) you must be very familiar with bend allowance calculations (and use them).

I have a box of doughnuts for you too if you can generate proper solutions to my previous challenge (without cheating).

The solution is possible, just not easy.

I am sure there are cases where this workflow is valid, I am simply prodding to use some critical thinking about a problem that has come up on all of the MCAD forums over the years.  Model in finished form using 21st century tools.  We left behind the 2D drawing board last century.

Edit:  I attached simplified example and expected result after Bending from starting flat.  (I forgot to put width of 20mm, but that doesn't go across bend so is not impacted by bend allowance calculation.)

[chrisplyler]

Had to figure out the Bend Deduction on my own, and then set the sketch up to account for it. The desired out-to-out lengths are overlapped by the Bend Deduction value. I used symmetries for the other half.

Then I bent it up.

And finally, I projected the body and checked for all desired dimensions.

So this is pretty much like the real world. If you're designing a flat pattern with a pencil on paper, or just scribing your flat sheet metal, this is exactly what you have to do. But I've read that the fancier programs like Inventor and Solidworks have the ability to set it up for you somehow.

[TheCADWhisperer]

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@chrisplyler wrote:

But I've read that the fancier programs like Inventor and Solidworks have the ability to set it up for you somehow.

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Fusion 360 will do it for you - if - you model in finished form.

Sheet metal houses do not even want your Flat Pattern unless you:

1. Work very closely with them to validate your digital prototype (bend allowance/deduction table or k-factor)

2. or you are doing the work in-house and #1 communication from above exists.

The customer is paying for the finished form that will cleanly assemble as designed to finished dimensions.

For completing the challenge - I owe you a box of doughnuts next time I get to TX. (Or you can come to PA to collect.  Hmmm, I will be in Kauai end of the month if you would like to collect on the challenge there.  )

[chrisplyler]

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@TheCADWhisperer wrote:

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@chrisplyler wrote:

But I've read that the fancier programs like Inventor and Solidworks have the ability to set it up for you somehow.

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Fusion 360 will do it for you - if - you model in finished form.

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If you model in finished form, there is nothing to do. You can force out-to-out dimensions to be what you want without any bend deduction calculations.

I like the Old Fashion type doughnuts.

PS - When you said the challenge was difficult, was the lack of some type of automatic bend deduction setup the hurtle you were thinking of? Or did you work out some other solution yourself?

[TheCADWhisperer]

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@chrisplyler wrote:

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Or did you work out some other solution yourself?

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I've been teaching the old-fashioned hand calculations for more than 20 yrs.

I understood the problem before I posted anything.

[Phil.E]

@TheCADWhisperer 

I don't think anyone would describe this as the best way to make new sheet metal designs. I hope that you aren't getting that impression from the way this is presented in Fusion. This is a data re-use workflow, because flat patterns are useful if you already have them, but useless if you need a 3D model that will behave in parametric fashion in Fusion, unless you use this tool to remake the model.

To address a couple of your points:

• Many customers do their own in house sheet metal. This is not for people who send jobs out to fabricators. It's well understood that sheet metal houses will always reverse engineer the customer model, and why they would do that.
• This functionality was devised as a data re-use workflow for customers migrating to Fusion.
• These customers would have: loads of flat patterns and also know the K factors and sheet metal rules used to make them.
• If you aren't one of these, don't use this tool, there is way too much guesswork for uninformed designers to workout, as you have mentioned.