not able to flat pattern in creo 2.0 sheetmetal

[rohit_rajan]

not able to flat pattern this sheetmetal part in creo 2.0..the unique this is that it does unbend..but does not flat pattern. i have also attached the part file below.

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[DavorGranic]

Flattens fine on my Creo 2.0. Im on M030 if that helps. Tho i use macro for create flatten form. i don`t go to flat pattern preview. And you are right my flat pattern preview won`t flatten it. Just pull out create flat pattern button on ribbon and it should work. Seems like some kind of bug.

[rohit_rajan]

mine is M010......and in M010 in flat pattern ...removing "merge colocated side surfaces" in "options tab" does the trick...but it still does not flatten in the new flatten preview option.

[DavorGranic]

Can you maybe update your Creo to M030?

I can send you flat part if its any use.

[rohit_rajan]

i would not be able to update to M030 immediately....but as i said i was able to flatten it with the flat pattern option once i removed the option "merge colocated side surfaces" ....thank you very much.

[TomD.inPDX]

Flat 1 and Flat 3, the .25 dimension extending the feature is what is causing the problems (4 places). Just removing this extension will cause other failures, however so be prepared to do some work.

[TomD.inPDX · Accepted solution]

Change the Relief on Flat 1 and 3 to Rectangular

[rohit_rajan]

thanx it worked. but as i have said before the part used to flatten with the unbend option..but not with flat pattern. do these two options work differently?

[TomD.inPDX]

I noticed that also. It seems the two features look at the feature creation process differently. The unbend/bend seems to look at the feature's definition in the feature tree where flatten looks at the geometry.

I am happy you have it working.