2013 Convert to Sheet Metal Fail

[stevec781]

I wanted to trim this part so I copied a face from another part as a composite SURFACE using Copy Object.  Got the error message in the picture.

Deleted the copy object feature, and made the cut using an extrude, still wont convert.

Deleted everything except the initial derived component, still wont convert.

Did a full shut down and reopen - still wont convert.

Part is a write off which means down stream parts that reference it will also fail when I overwite it.

And was a waste of time as split feature wouldnt let me select the copied face as the split tool anyway

[jletcher]

Suppress the Cabin Master.ipt and try...

[JDMather]

This doesn't answer the question to why it is claiming it is multi-body, but I think I would change the technique if the flat pattern sides are supposed to be perpendicular to the flat face.

   The original without the extruded cut wasn't quite right either.

[stevec781]

The geometry is correct, you have highlighted a never ending frustration of Inventors inablity to create production ready flat patterns when there is a chamfer or hole that is not perpedicular - It should square up the edges like its competitors do.

Suppressing the first feature will leave nothing.

There are 2 problems

1.  the addition of a copied surface made it think there was 2 solid bodies,

2.  it still thinks this after the surface was deleted.

[jletcher]

Suppressing the first feature will do nothing but suppress it. It will still keep everything you have.

 Is the Cabin master.ipt a multi-body?

 Did you try it?

 I don't have 2013 loaded waiting for 1st SP on 2014 to load it...

[Anonymous]

It's not "Inventors inability to create production ready flat patterns", it's the user not using the right tools. If you extrude Sketch5 as a surface and then Split and then Thicken/Offset the unwanted material you will have a part with edges that are perpendicular to the material face.

This does not however fix you initial problem for which I have no answer.

[ic198]

Not sure if this solves your problem, but if you are just trying to convert to sheet metal so you can get the flat pattern, attached is a solution. Thicken the inside surface of your mullion, creating another solid body. Dervie this into another part (Outer Mullion Fail2.ipt). This new part will convert to sheet metal and can be flat petterned, while the original should still work in your downstream parts.

I never use Copy Object, as I find the results unpredictable at best. If I want to copy a surface and use it in another part I use a Thicken/Offset in surface mode with a 0mm offset, then derive this in to the new part. Seems to work every time.

[stevec781]

The part is correct, too correct.  If it was fibreglass it would be a perfect model.  It is mathematically perfect but not all real world manufacturing needs accuracy to 1 thou, especially sheet metal.  Yes there are other longer ways to model it to get around inventors limitations.

Here is the screen shot of trying to suppress it.

Brendan, of course further modeling can work around it, but by definition a flat pattern is a 2D pattern and should never contain lines representing the 3rd dimension of thickness.  I have used other programs that understand this. 

IC198, this was just a quick edit and I was being lazy so I used copy object.  I normally never use it.  But it should work.

All other similar parts, derived from the same master part, flattened ok, but I still have to run my macro that cleans up the flat patterns before I nest them.

But back to topic, adding a surface to a part should not prevent it from being converted to sheetmetal.  Must surely be a bug.

[Anonymous]

Flat pattern is flat pattern. What I and JDMather were pointing out is that the way your model is you would end up with a chamfered edge in the flat pattern. All edges in flat patterns should be perpendicular to the metal face.

I note that you 'still have to run my macro that cleans up the flat patterns'. If modelled with the correct tools this NEVER needs to be done. I cut my own plasma parts and I ship the DXF files out to a laser cutter and neither of us has to clean up the files. They just work.

Good luck with your part.

[ic198]

I always cut first and thicken last to create sheet metal parts. If you expect Inventor to straighten up your edges, which face would you want as the flat pattern- that larger face, which means you're going to bevel the edge after cutting, or the smaller face, so you're going to fill the gap with weld? And how is Inventor going to know which?

I'm not sure if this will help, but if you delete everything from your part, including the derive, it will then convert to sheet metal. I'm guessing you could then derive in the part again and it should all work fine- hopefully including the downstream parts, though I can't check this.

[Anonymous]

I agree with ic198 that Derive and then Split and Thicken/Offset might be the best option. Like the other posters have mentioned I also rarely use the Copy Object tool. But I do use a hell of a lot of Derive/Split/Thicken to make sheetmetal parts. All valid and predictable tools in the SM environment.

[stevec781]

I am not disputing what you guys are saying, and I normally use surface, thicken etc as you are suggesting - I rarely use the sheet metal commands.  But the nature of what I do means I often have unexpected design changes, as I did this time, and what should have been a quick cut turned into a mess.

As for flat patterns, all I am saying is that other programs can deal with it.  From memory they gave the largest outline.  When you are dealing with slivers often less than 1mm, inside or outside doesnt matter for parts that require weld prep in any case.  And when dealing with hundreds of parts, the extra steps required by Inventor start to add up, and increase the chance of them failing when edits are made.

[JDMather]

---

@stevec781 wrote:
 

As for flat patterns, all I am saying is that other programs can deal with it. 

---

Just to clarify -

The flat pattern is correct for the geometry you created.  It is the folded part that does not match real-world geometry of a part that is folded from a flat sheet with edges cut normal to the flat face.

[stevec781]

I agree, the flat pattern is too correct.  As designers we create the part and then flatten it for cutting.  During the flattening process we square it up.  We dont start with a flat sheet and fold up a part, we start with a part and flatten it for production.

[JDMather]

So as designers we need to create the correct as-folded geometry for the software to create the correct flat pattern.

[stevec781]

No, we dont have to model the bend reliefs, these are required for production and the software adds them for us, and it would be nice if it cleaned up unwanted lines from chamfers and angled cuts as well.  In some cases the flat pattern even contains hidden lines, that's just ridiculous.

It should just project the data from 1 face, or a chain of connected faces, selected by the user.

There are many cases in my industry, where editing the part to suit the flat pattern would cause problems in the drawings.  If I squared up this hole in the model, then my drawings would be incorrect as I would have no chamfer to dimension, so the clean up must be done in the flat pattern, or after export, where hidden lines are included.

Part

As Exported

[JDMather]

---

@stevec781 wrote:

There are many cases in my industry, where editing the part to suit the flat pattern ...

---

Edit the part to suit the real world finished form, not to suit the flat pattern.  The flat pattern will reflect a correctly modeled finished part.

I am obviously lost here, so I'll bow out now (for real this time).

[ic198]

With the part you have drawn, what is it you would like Inventor to do in making the flat pattern? If, as you suggest, it were to simply take one face your fabricators would have to grind away one edge, while filling the other with weld, to get the end result part you have modelled. I'm guessing you want either the smallest hole created by the two ellipses (you're grinding both edges) or the largest hole (filling both edges with weld) but I don't know how you'd explain this to Inventor- it would be a neat trick if this could be done, with options to say what Inventor should do for every feature.

[stevec781]

JD, I'm not trying to wind you up, maybe I just cant explain it that well.  I understand you have access to other programs, if you are curious you could create a part with an angled cut and see how they handle the cut and subsequent flat pattern creation.  It's just 3 features, the base and 2 cuts.

ic198, back to the OP, it would have been nice if I could have created any type of flat pattern without having to completely delete everything and start again just because I copied a surface, but I would also like Inventor to at least match the capabilities of its competitors.

[johnsonshiue]

Steve,

The broken link part is somewhat corrupted. There seems to be an extra solid body lingering in the database leading to sheet metal conversion failure. Certainly, something was not right resulting in this behavior. If you know how to reproduce it from scratch, please let me know asap.

In the meantime, I am able to salvage the part (see attached) and convert it to a sheet metal part. Please take a look and let me know if more information is needed.

Thanks!