Sheet metal - Multiple Bends - Opposite Directions

[Anonymous]

Attached is an image of what I am trying to accomplish. I took what I knew of the sheet metal and applied it to a standard 3d model to see if i could convert and flat pattern. But inventor wasn't having any of my shenanigans.

I would like to be able to basically stamp or die cut a pattern into the sheet steel. Then fold the steel outer section one way and the inner section the opposite direction.

Outside of Inventor this is accomplished easily by multiple methods. But I am not able to accomplish this in Inventor. I have 2015 Inventor, 64bit. I will watch videos ort read, but apparently I am not using the right terminology as I am not finding anything that will work, including contour flange.

Thanks in advance.

[JDMather]

Can you attach your *.ipt file here?

Do you really want zero radius bends?

[Anonymous]

Certainly. It's a hack and slash 3d model converted to sheet metal.

[IgorMir]

Hi Brian,

It looks like the part will need to be welded at one corner after the folding. Here is a part for you to have a look at. IV 2010 file.

Cheers,

Igor.

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@Anonymous wrote:

Attached is an image of what I am trying to accomplish. I took what I knew of the sheet metal and applied it to a standard 3d model to see if i could convert and flat pattern. But inventor wasn't having any of my shenanigans.

I would like to be able to basically stamp or die cut a pattern into the sheet steel. Then fold the steel outer section one way and the inner section the opposite direction.

Outside of Inventor this is accomplished easily by multiple methods. But I am not able to accomplish this in Inventor. I have 2015 Inventor, 64bit. I will watch videos ort read, but apparently I am not using the right terminology as I am not finding anything that will work, including contour flange.

Thanks in advance.

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[mcgyvr]

Thats a cool one..

Obviously in the real world that could be made in 1 piece without any welding,etc..

But getting the dimensions "perfect" in Inventor for that to unfold will be tough I think..

I might have to actually try this one too..

[Anonymous]

I agree. In theory, it could or would be quite simple if the program allowed for multi-bend or multi-fold. Sort of like selecting multiple fillets at the same time. This would allow you to sketch the bend line on opposite surfaces to dictate bend direction. And then it would allow for a selection of joint locations which could be edited.

Another direction I was thinking would be form splitting. Basically I would create a positive or negative cutting form. Then, using something like emboss (but not emboss) I would apply it to the sheet metal. Because this is a cutting form, it would not create the side surface like emboss does but instead would split or cut the surface creating the finished look which would still unfold.

[Anonymous]

I appreciate the effort. But, using a weld in CAD could cause complications down the road. Mainly in regards to whom will read it. If by chance, someone opens the file and reads the weld, then it is possible for them to create the part as such which would be a problem.

The weld approach was considered just for the finished look but the possible complications were just too big to ignore. thanks again.

[mcgyvr]

I didn't spend much time but was able to get a model using all sheet metal tools (just one way to do it)..

It won't flatten once those 2 bends are added..

Obviously I made up dimensions... 

This is an interesting challenge.. 

If you can get the dimensions "perfect" I suspect it should unfold.. maybe not though..

[blair]

I think, Inventor gets confused because you have a Bend Up and and Bend Down at the same location on the Flat Lay-Out.

[Anonymous]

That sounds about right. Inventor does seem to get confused on things like this. But you would think that a software with sheet metal as a standard capability, it would  have a tool or function to do something of this nature.

But alas, there is probably an add on that costs extra that could do it.

[blair]

Possibly something like AutoPol might be able to do it. I haven't the time to run it though my Radan software as to see if it throws an error back.

[mcgyvr]

I still think Inventor can do it..

As I said the dimensions must be EXACT.. 

The part I posted clearly won't flatten as the dimensions are simply off. The middle section folded the other way is too long compared to the area it would fit into in the flat pattern..

I think I can do it with bend part maybe.. 

[mcgyvr]

Did it 3 different ways.. All that "should" flatten but Inventor just won't do it..

I don't think Inventor can flatten that geometry.. (maybe if you mess with k factors on specific bends)

HOWEVER.. It doesn't matter.. You can usable dimensions for the flat pattern without having it modeled exactly like that..

I think modeling it just like this attached (for flat pattern calculations) should be sufficient..

Then just add the bend back in

[hosford]

I think the reason Inventor will not unfold this model is more basic than you guys are thinking.

In order to make this part, three four bends must be made simultaneously, think about how you would do that in real life.

[Anonymous]

It's 2 bends in real life done in one shot. I understand there is a myriad of reasons inventor is not able to do this. It boils down to programming. The software may not be able to validate this because it is not programmed to do so.

From a programming standpoint, you would need to have a swag function that allows you to dictate directions and dimensions 1 at a time until the software feels it is fully constrained. In this way, it would allow for a robust creation without immediate failure due in part to, to many dimensional inputs.

From a production standpoint on the floor, I can do this in 2 steps using different methods.

1. Laser cut outer profile & inner single line cuts.

2. use a forming die in either a press break or any other type of press.

depending on how thick the material is, you could form the metal using cross link foam and a push bar as well.

[blair]

My "old" guys on the shop floor would give it to a "newbie" and stand back and watch for a while.

Build a 2-piece die to do it in real life.

[hosford]

I would say if you feel it is only two bends, and possible to do in a press brake, model the tooling required.

Probably an easier way would be model and dimension the part as it goes from flat to fully formed. (change the bend angles)

[WHolzwarth]

It can be done, but zigzag angle needs to be different than main angle. 2016 file attached

Walter

[IgorMir]

Hi Blair,

No, it has nothing to do with the bending up or down, really. The inner part has three bends and the outer part has just one. Hence the inner part will always be shorter by two bend allowances. And that's clearly seen on the flat pattern of the part I have posted. By trying to make it as one piece the plastic deformation will be introduced to the item. And Inventor doesn't deal with that type of deformation as we know. That's if two inner faces has to be parallel to corresponding parent faces. If not - then some calculation will require to determine the length of inner cut-out.

Cheers,

Igor,

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@Anonymous wrote:

I think, Inventor gets confused because you have a Bend Up and and Bend Down at the same location on the Flat Lay-Out.

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[blair]

All that would happen then is the inner bent portion won't have faces that are parallel to the main outer body because of the k-factor, either way it's beyond Inventors functionality.