This part looks like exactly what I want. I can step through the feature tree and every feature works, including the Unfold and Fold. If the part can unfold and fold, why would the flat pattern not work?
there are two issues why this part cannot be flat patterned.
The first issue is that you have removed the "fixed entity". In order to be able to create a flat pattern there has to be a "fixed entity". That is usually a face that is assumed as the fixed flat entity and the flat pattern unfolds surrounding bends from there. But for cylindrical and conical parts there is no flat face (except of maybe the sidewalls) and therefore SOLIDWORKS uses a linear edge adjacent to the bend:
With your diagonal cut extrude you have removed this fixed entity and with it there is no fixed entity from which the flat pattern feature can start to develop the flat pattern. You could work around this issue by placing the cut sketch not exactly on the vertex but keeping a very small linear edge instead.
The second issue is that SOLIDWORKS can only handle cylindrical or conical bends with angles < 360 degrees. Means, if you create a part that actually is more than 360 degrees, the flat pattern feature will fail. You have started with a cylindrical part that is almost 360 degrees, you have removed material with the diagonal cut and the angle is still less than 360 degrees. But with the next tab feature you have added some more material and internally that increases the overall bend angle to more than 360 degrees and therefore the flat pattern feature will fail.
So one solution would be to manually create a flat pattern config and to not fold the unfolded body back. With it, it looks like the flat pattern and you also can get the folded tube as well.
But this part can be also built with the lofted bend feature. It is a little bit more effort and it requires more calculations from our side but you can achieve your intended solution. As you can imagine we use a different algorithm to unfold a lofted bend component and this is why we can create the flat pattern there and not for "ordinary" sheet metal parts.
Hope this helps
SOLIDWORKS Product Definition Team
I certainly agree with Frank that you can make a flat pattern config which suppresses the fold feature and that may be the way to go with this. I did this with a Base-Flange and was able to flatten it. You may not deem this desirable since I did add a couple of bends, but wanted to show you another method. I have attached a 2015 file.
Thanks for the quick answers.
Frank: I knew there had to be something going on behind the scenes that I couldn't see. Thanks for the clear explanation. I did also create this part with a lofted bend between two 3D sketches based on helixes and then cutting to length, but I couldn't get the overall length to come out just right (artifacts of rounding?), and this way seemed more straightforward to me.
Dennis: I like your method too; thanks for the file.
As you both suggested, adding a configuration with the final fold suppressed, which had not occurred to me, will do what I need in this case (it just bugs me to have warnings pop up when I use the file).
Thanks & Regards
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