I am stuck with a CAD design, bend a model or sketch into curved body.

[Cave_Master]

I need to “bend” a 3D model or sketch onto a curved body.   I don’t believe there is a way to directly do this in Fusion, but I am wondering if any of you “gurus” can think of a work around or a way to fake it this time.

Here is the situation - We are a snowski manufacturer.  All our engineering, design, and manufacturing is done here in house.   Although we are producing a 3 dimensional product, our CAD is mostly 2D.   

We do some 3D CAD which we then machine on a 3 axis router. Other than that, most of our tooling is created using 2 and 2.5 axis strategy.  On the engineering end we have never drafted a 3D model of a pressed ski.

Right now I am in a situation where I need to machine a ski after it is taken out of the press.  This means that I will have to model a 3D, pressed ski. From that I will design some hold fixtures and finally create 3D milling operations.  My biggest holdup right now is determining how to create this 3D geometry.

To give an idea of our build process, we prepare all the components in a flat plane - ie the plastic base, wood core, composites, etc…  These are all put into a press with epoxy. Once the epoxy cures, the components are molded together in the shape of the mold.

My hope is that I can use the existing CAD geometry for our mold and our flat shape to make either a 3D model (preferred), or a 3D sketch on the mold (also will be greatly helpful).   To better illustrate my situation I will provide examples that I do have CAD data for and an example of a pressed ski, to which I am trying to model in Fusion.

Ski press - this is where the flat components are pressed with an epoxy and come out with the press profile.

Ski press - this is where the flat components are pressed with an epoxy and come out with the press profile.

CAD for the ski press, what I hope to use to “bend” the sketch or 3D model.

CAD for the ski press, what I hope to use to “bend” the sketch or 3D model.

CAD for the ski shape, what I hope to “bend” into the mold.

CAD for the ski shape, what I hope to “bend” into the mold. 

Pressed SkiPressed Ski

Here are some pressed skis, this is what I am trying to create in CAD.

I hope this makes sense.  I know there is no direct way to do this in Fusion but I am open to just about any idea or method someone has to make this happen.

Thank you!

[davebYYPCU]

Yep, I came across the same thing, because I was of the impression that the shape of the ski in flat view, was not actually symmetric, (end to end), I had to make two ends, from the origin, outwards.  After refolding the cut plate, my flat folding face is still there, I have used split body to cut and remove the flat section off the plate to bring it back to centre both sides, then combine joined the two halves.

The difference I see in the movie was that you at first tried all in one go, your error means that the original flat section used to make the fold was cut off by the intersect extrude.

Might help...

[Cave_Master]

I will try tomorrow when I’m in the office. Will this work with a body of
varying thickness?

[davebYYPCU]

That's what I did in my file,

after the fold, unfold processes? yes you can, 

but not if you want to refold again.  Sheet metal was just a means to the end.

Might help....

[Cave_Master]

I have been banging my head to the wall, trying to get this to work.  I have been creating my flange, flattening it, running an intersect operation and then Fusion fails every time I try to refold the flattened sheet metal.

Deconstructing both your model, @davebYYPCU  and yours @wmhazzard, trying to figure out what you are doing differently and I am emulating your process.  I just couldn't figure out what I was doing wrong until I finally looked at the sheet metal from the side, it isn't going fully flat.  

You can see in the video, I create my flange.  I use the flat geometry I placed in the middle of the mold as the reference to flatten from.  When I have "unfold all bends" selected then Fusion selects 4 bends and as you can see it doesnt fully flatten.  When I deselect "unfold all bends" I am only able to select 2 bends.  So the other 2 bends are only selectable by Fusion.  Either way manually selecting the two doesnt lead to a flat body, but a different body than the first way.

[Cave_Master]

Additionally if I segment out the mold piece and create a flange only with the pieces that wouldnt flatten out, I get an error saying there is nothing to unfold.  

Screencast will be displayed here after you click Post.

6ceaf2b9-3255-4785-9328-1beec825c990

[davebYYPCU]

I suspect your geometry.

you have 5 segments in the flange, segment 1 and 5 work correctly.

I suspect the segments 2 and 4 are lines, and not tangent arcs to the segment 1, 3. and 5, for that behaviour.

The second post today makes no sense, my end.

Might help....

[Cave_Master]

OK so if you look at the screenshot, sections 1 and 5 are actually ellipses.    Section 2 and 4 are normal arcs and section 3 is a flat piece I added to reference in unbend.

Everything seems tangent.  It behaves like a watertight sketch, will extrude, etc...

[davebYYPCU]

I can't see any tangent icons.  Extrude works, but would it work as a rail in loft (Not G1 continuous)

Mine worked, yours must be different.

Might help....

[Cave_Master]

Ah, I see.   I added the tangent constraints to the drawing.    I am now having better luck with bends and unbending, however I am having issues now that I didn't have before.

When using the flat section I put in the middle of the mold, I get an error when trying to refold faces, "Error: curve is broken into two discontinuous pieces" .  But when I use a different flat section at the very end of the mold then it does work the way it is supposed to.  If I cant figure out how to unfold from the middle then I can probably figure out a work around but ideally I would like to unfold from the middle of the mold.

Here is a screencast - https://knowledge.autodesk.com/community/screencast/e2f4dd74-bd94-4a0d-b85b-a260de373495

[davebYYPCU]

I cant take you further with that, you will find that you can't refold after cutting the front of the ski off, has to be from the centre.  Only thing to check, is if the fold, top or bottom surface makes a difference, otherwise you have found a bug, that AD will want to sort out. 

Might help.....

[Cave_Master]

Interestingly when I select the bottom face it wont refold, but I do get a different error so that is something -   Error: There was a problem combining geometry together.
If attempting a Join/Cut/Intersect, try to ensure that the bodies have a clear overlap (problems can occur where faces and edges are nearly coincident).

I am going to put a post over on the support forum as this seems like it could be a bug.   If you are interested in following.  Also this is the first time I have used the sheet metal tab in Fusion so I am new to the work flow there, I could be missing something.

[davebYYPCU]

Basically, you are on the same track, didn’t see anything unusual - you are doing the same operation as I did, but you get an error when I didn’t.

Use my file, edit with your dimensions, while your file is investigated.

Might help...

[Cave_Master]

Thanks.      I am suspicious of the ellipses wreaking havoc.

I have had issues in the past with sketches not solving due to problems with ellipses.  One of the AutoDesk engineers basically told me that "Fusion sketch solver struggles with trimmed ellipses" and if I can use a different curve such a spline instead.  Also it was mentioned that circular arcs used to have many of the same issues but have been solved.  Ellipses since are used less, hasn't had the attention, so some of these problems still persist.

This was in the context a sketch, not sheet metal, but since the sheet metal is driven by the sketch I am suspicious here.    My next move (if my other thread doesnt get some ideas) is to redraw the mold without ellipses.

[davebYYPCU]

Yep, ok,  you got it, ellipse should work, but change them out for tangent arcs

the face of my mould is tangent arcs, and that is likely a requirement for the unfolding.  

Whilst an an ellipse is a cylinder sliced on an angle - curve, the elliptical curve might not work in fold / unfold.

@karina.harper , am I close?

Might help.....