Why is my flat pattern failing on the idw

[carstenandersen]

Hi

Why is my is my flat pattern failing in my idw(not in the part)?

As soon as my cut out pattern gets to close(11-12 mm) to the lower edge of this sheet metal frustrum, the flat pattern will not show up in my drawing. Please advice on whats wrong.

ipt and idw attached.

Tia

Carsten

Inventor 2016 R3, Windows 10 1709

[CCarreiras]

Hi!

There's nothing wrong with the drawing, you're just not picking the right line to create the dimension.

Turn on the "Hidden lines" in the drawing and select both external lines and you will get the real value.

[carstenandersen]

Sorry, but the problem is that the FLAT PATTERN is failing to show - see the model tree.

[Cadmanto]

When I opened it I got the main views in your drawing.  I added the flat pattern and edges came in dashed lines.  When changing it to solid the view disappears.  If I make it a shaded view, it reappears without the line edges.

What I did notice is if in your model I suppress the Refold feature, the part shows the flat fine in the drawing.

I leads me to this conclusion, to get around what you have, if you create a view rep or make an ipart out of this, one view showing the rebuild suppressed and the other not.  You can show these 2 different reps in your drawing.

Why is this doing this?  No clue!!!  Never used the rebuild command and never seen this before if I am being honest.

Hope this makes sense.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[carstenandersen]

Thank you for your suggestion.

If you suppress the Refold feature - yes it will be shown flat because the flat pattern will not have to be calculated.

We have 40 Inventor seats dedicated to Sheet metal design for our machines - 95 percent of our products is sheet metal, produced in a highly automated design and production setup. therefore we don't (can't)do in workarounds.

The strange thing in this case is that if you increase the distance fro the edge to about 12 mm or so, the flat pattern will be ok. But we cannot design our machines according to Inventors limitations.

[Cadmanto]

No, I get it.  This may not be a limitation as much as it is trying to figure out why and what the solution is.

While I have done a fair share of sheet metal design, nothing to the extent you are describing.  So, I get your position in not wanting work arounds.

I did some more searching and found this thread.  See if it offers anything that could help you.

https://forums.autodesk.com/t5/inventor-forum/inventor-flat-pattern-wont-display-in-idw/td-p/7297443

Also, something I forgot about.  When I would have flat pattern issues, I would delete the flat pattern in the model and recreate it.  Quite often it would fix my issue.

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2018

[CCarreiras]

If you use contour roll instead of revolve, it works well for me.

It's better to use the sheet metal tools than solid tools to achieve flat pattern with no issues.

[CCarreiras]

[johnsonshiue]

Hi! Something is interesting with the flat pattern. For some reason, the orientation is invalid. If you open the part and do Rebuild All (Manage -> Rebuild All), the drawing view will be corrected. Do you know how to enter such state again?

Many thanks!

[carstenandersen]

Hi Carlos

The original file that the user gave to me for troubleshooting was in fact made with  Contour Roll. So in my solving of the issue i tried most things and found out that it fails on both Revolve and Contour Roll. The part that I uploadet to the forum is a simpler edition. Ex. the original file had similar cut outs at the top end which works just fine(Flat-pattern-wise) on the top edge.

Generally I don't use Contour Roll much because I think it can create shapes that you cannot produce in real life.

Thanks for you input

/Carsten

[carstenandersen]

Did you make a pattern of the cut out? That's where it goes south.

/Carsten

[carstenandersen]

Hi Johnson

The Rebuild All function does not help me. Did you try it with my model and with a pattern of the cut out close(<11 mm) to the edge?

/Carsten

[CCarreiras]

Yes, you're right about the circular pattern, i also think that the problem is there...

...But since i have version 2019, i couldn't send you the file later, so i didn't make big changes. My advice would be to change the pattern source, maybe build the cut in the middle of the part, and create the pattern from there.

Regarding the cutout, it was just an advice to avoid errors in sheet metal, not for this one in particular, but again, with different inventor versions, i couldn't say much more.

[johnsonshiue]

Hi! I did try it on 2016 and Rebuild All worked for me. Have you installed the latest updates to 2016? I can double-check it on 2016 and post the fixed files.

Many thanks!

[carstenandersen]

Hi Johnson

We are running

Inventor Professional 2016 64

Build: 236, Release: 2016.2.9

A set of fixed files for further investigations will be highly appreciated.

Thanks

/Carsten

[johnsonshiue]

Hi! Carsten,

I was wrong. I can reproduce the behavior using your file on 2016 but not on 2017 and later. It seems to have been fixed on 2017 but not on 2016 unfortunately. The behavior has something to do with the patterned extrusion cut breaking up planar reference of the Unfold/Refold.

Many thanks!