Convert Sheet Metal to "Normal" Part?

[rokahn]

I wanted to remove the non-planar parts of a folded sheet metal part. I first tried suppressing or deleting the bend feature but even though subsequent features should have been independent (i.e. holes in the base flange), all subsequent features had to be deleted when I wanted to remove the bend. I tried to move these features above the bend but that wasn't allowed. Any ideas on how to remove a bend but keep subsequent features?

Now that I've rebuilt the features I wanted and suppressed the bend, I'd like to convert the entire part into a "normal" part instead of sheet metal. How can I do this? If I don't manage to convert it to a normal part, what differences between the two part types should I be aware of?

Thanks for any help,

 

[CorBlimeyLimey]

As you mentioned the “base flange” I assume the part was modeled with SW2001+ (or higher), using the revamped sheet metal creation feature. Instead of deleting or suppressing the bend, go back to the base flange sketch & alter it to reflect what is required, then close the sketch. Subsequent features should not, but may still be lost or corrupted & need fixing or replacing. This is probably due to part faces being renamed by SolidWorks. Refer to faq559-871 in this forum for a better explanation.

If the part is not too complex, it may be simpler to remodel it from scratch.

A sheet metal part cannot, to my knowledge, be converted back to a “normal” part. This is because some features created while in the sheet metal mode are simply not recognized in the “normal” mode. You will not lose anything by leaving the part as sheet metal, in fact you probably gain, by being able to do more with sheet metal than with the normal. (eg. Flat layout, louvres, dimples, etc)

Happy New Year.



CorBlimeyLimey
Barrie, Ontario
faq559-863

 

[DanielGraham]

have you tried the unfold command. seems that is the function that you are trying to do. that is a better option than deleting bends.

 

[Mandrake22]

You didn't mention what your final intent is, but you could always save the part as SAT or Parasolid.

 

[TheTick]

A sheet metal part is "initiated" with 3 consecutive features: Sheet-Metal1, Flatten-Bends1, Process-Bends1. (Feature names may vary slightly if renamed or redone.)

Once all sheet-metal specific features have been removed, remove those features and your part will be "normal" again.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[SBaugh]

That is the Old style of Sheet metal - Base-Flange is the new and improved style. It only consists of Base-Flange, and Flat Pattern Everything that you do like cuts, extrusions, etc... is in between each of these features.

rokahn,
I guess you could try building your file with the old style Sheet metal, because with Base Flange, it is the parent of all following Features. But I don't think it's going to matter, because the Old Style is going to be the parent and if you delete that then your going to lose all children after that.

If you have a child feature it will always require the parent. Remove the Parent, and you will remove the child. "I first tried suppressing or deleting the bend feature but even though subsequent features should have been independent (i.e. holes in the base flange), all subsequent features had to be deleted when I wanted to remove the bend."

Those holes are children to base flange because you probably used the face to start your hole. That makes your hole a child of that face and that face is defined by the Base flange. The Base flange is defined by the intial sketch.

If your not wanting a Sheet Metal part anymore, you could just build what you need to over in a new part and copy out your sketchs from the old and paste them in the new part.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[TheTick]

Good point, Scott.

Because of the natre of most of our products (stamped hinges) most of our models start as "normal" parts and have sheetmetal features added later in the modeling process.

 

[rokahn]

Thanks for the help everyone.

I was trying to avoid losing the relations in the sketch (which are lost during copy-paste) but that appears to be the only way to do it if I want to convert to "normal" part. As Scott surmised, I'm running a recent version of SW (2004) so sheet metal parts are indicated by three features in the feature tree:
"SheetMetal" at top
"BaseFlange" second
"Flattened" at bottom
Flattened cannot be deleted and I presume the rest can't either so that's not a way to convert to a normal part.

Scott,
I understand that features/entities which relate to parents must be deleted when the parent is removed but there was not apparent relation between a series of features and a "SketechedBend" sheet metal operation. Yes, all features relate to the initial "BaseFlange" feature but it seems that SW treats all features which are created after a "SketchedBend" operation as children of that feature. Oh well...

Thanks again,
Rocky

 

[JNR]

Just a note about suppressing to clarify.

When you suppress a feature it is treated as if it is NOT THERE, period - just as if you DELETED it (At least, in that configuration) . That is the whole point of suppression. Therefore when you suppress any parent, it's children will be (in fact logically must be) suppressed also.

Be naughty - save Santa a trip.