How to make sheet metal lofted flange connected to other geometry?

[John.Derewianka]

Hi,

Former Creo user here, although I've been using Inventor for the last 3 months and getting the hang of it.

However... I just can't figure out how to model this one particular sheet metal part in Inventor.

The bulk of the part is a shape that blends from an oval-ish profile on the bottom to a circular profile on the top.

For that part of it, the lofted flange tool (with a rip down the side) works just great:

However, I need the circular cross-section at the top, to then continue straight up and form a short cylinder (illustrated by the yellow sketch below):

All of my attempts to add onto this base geometry have thus far failed, so far I've tried:

-Creating a contour roll on the top of the loft (doesn't work as it doesn't connect the roll to the slightly non-flat top edges of the loft).

-Cutting away a tiny slice of the top surface of the loft to create a flat top surface for a contour roll (the contour roll then doesn't work as then the top profile isn't perfectly circular).

-Starting out with the cylindrical shape and then building the loft on top of that (again, non-connected geometry).

-Building a loft on top of the loft (again, non-connected geometry).

-Modelling as a solid object and then converting to sheet metal (problems with making it a flattenable sheet metal part, although this is the path I'm currently playing around with more).

-Extending the edge on the top surface using a 'ruled surface' (doesn't quite get the shape I need as it basically just continues to extend the loft/blend transition).

I know Inventor has to have a way to create this geometry as a sheet metal part somehow - I'm pretty sure this is something I could have done in Creo with the extrude sheet metal wall command - but at this point my limited Inventor expertise has left me scratching my head, and all the tutorials I could find using the lofted flange didn't give any insight as to how to add to the created loft geometry.

Any insight as to how to model this part would be appreciated! (At this point, the only solution I've been able to come up with is modelling the part as a normal 3d part, not sheet metal, which is far from ideal.)

Thanks!

-John

[SharkDesign]

I'm real life I'd make this as two parts and weld together. 

You can also just extrude a ring on top and some fillets as long as the radius and thickness match your sheet metal rule.

[John.Derewianka]

Thank you James!

It does seem like a potential part for a 2 piece & weld design, however it's an existing part currently being made as a one-piece part (I'm going through and bringing some old 2D Autocad flat patterns into the 3d world).

Your suggestion of extruding and then using fillets to clean up the boundary worked well:

I'm not getting a perfect flat pattern (not perfectly flat, I should say) but it's the best I've gotten (certainly better than a straight-up 3d part):

Appreciate the help, thanks!

-John

[BDCollett]

If you are on Inventor 2022, you could do a combination of the two and modify one state to have the extra added on when the bottom section is unfolded. 

Then you would have a flat pattern and a 3D model that represent what you want. 

It would be interesting to see how this is made, I assume the reason you can't actually model it flat is in real life there would be some forming involved to get that shape.

[JDMather]

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@John.Derewianka wrote:

....however it's an existing part currently being made as a one-piece part...

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Can you Attach image of real world part?

[John.Derewianka]

Yes (although as a shiny sheet metal part it's hard to show detail):

It uses the short cylindrical section to mate up with another part.

And yes, @BDCollett  I believe you are correct, it's a formed part, although there shouldn't be too much actual stretching other than bending (although I'm sure there is at least a little). Unfortunately I am still on 2021, so I can't try that method just yet.

@SharkDesign, I appreciate your suggestion above. I thought it was working for me, but it turns out when I tried to add other small features in (slots/tab, etc.), Inventor would just freeze up and eventually give an error message of not being able to solve the sheet metal faces.

I appreciate all the thoughts. The current path I'm going down is to model the part up as a solid part (fairly easy to model the geometry that way), and then using the unwrap tool to get a flat pattern that I hope is going to be close enough (basically treating the bend calculations as negligible since it's a fairly thin part in respect to its size). If anyone has any better ideas, I'm certainly still all ears. This likely will prove sufficient for forming the part. (If not, I'm leaning heavily towards letting the supplier figure out how they want to make a flat pattern 😂).

Thanks guys,

-John

[SBix26 · Accepted solution]

The only thing I would suggest in addition to your proposed solution is to offset a surface (use Thicken tool) about midway through the thickness (closer to the inside than the outside, I think, because the material will stretch more than it will compress), and use this surface for the Unwrap operation.  That should get you really close to "reality".

This would be akin to manually creating the neutral surface (neither compressed nor stretched) that Inventor sheet metal unfolding creates virtually.

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Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[John.Derewianka]

That is a great idea @SBix26, thanks!

[IgorMir]

Hi John
Here is one more way of doing it. Please see the attached. Files are in IV2020 format.

Cheers,

Igor.

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@John.Derewianka wrote:

I appreciate all the thoughts. The current path I'm going down is to model the part up as a solid part (fairly easy to model the geometry that way), and then using the unwrap tool to get a flat pattern that I hope is going to be close enough (basically treating the bend calculations as negligible since it's a fairly thin part in respect to its size). If anyone has any better ideas, I'm certainly still all ears. This likely will prove sufficient for forming the part. (If not, I'm leaning heavily towards letting the supplier figure out how they want to make a flat pattern 😂).

Thanks guys,

-John

[cadman777]

Although I can't view your 3d model in my older Inventor, this subject has been raised a number of times in this forum.

The way I understand this type of request is, Inventor is incapable of flattening it no matter how you make this part in Inventor. Instead, you would need to use an Inventor add-on (don't know if one exists), or some kind of specialty software to do it (which typically are very expensive). I read an informative thread on ship/boat hulls, b/c that's what is commonly attempted in Inventor using with doubly curved surfaces.

I doubt any of the mid-range modelers can do it, even SW which was designed as a surface modeler.

I'm curious if Creo can do it?

I typically use Rhino3D to do complex surfaces that Inventor can't do. But this kind of surface is even impossible to do in Rhino, b/c Rhino is primarily a NURBS surfacing program. Some new commands have been added to approximate flattened complex surfaces since Rhino6, but they still aren't accurate for production. Back during Rhino3 I bought an add-on (very expensive!) called Expander. it did this very accurately. But that was back in 2003, and they 'expanded' their repertoire since then and dropped the add-on. Now their software is way above my pay grade to buy. Besides that, even if you had a software to do it, you still would have to do the R&D involved with figuring out the parameters that you need to use with that software for each part you flatten. So there's really nothing easy or simple about doing this, at least not in my experience.

[John.Derewianka]

Thanks for the idea Igor! I see it hinges on using the unwrap tool as well. I was unaware you could import a single solid from a multibody part into another part; a very helpful concept to know!

[John.Derewianka]

Good to know, thanks @cadman777.  I don't have access to Creo anymore to check - I know the process I would follow to model this part in Creo sheet metal, and I think it would work, but I can't confirm unfortunately.

[IgorMir]

Yes, it does. Since the part is not a Sheetmetal part in Inventor's sense but a formed part instead. Hence - a different approach in modeling.
Cheers,

Igor.

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@John.Derewianka wrote:

Thanks for the idea Igor! I see it hinges on using the unwrap tool as well. I was unaware you could import a single solid from a multibody part into another part; a very helpful concept to know!

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