Cannot unfold sheetmetal... 2

[Uka]

I am pretty new to "Sheet metal".

I am using SW2003 and trying to "flatten" a sheet metal part. But it gives me an error, saying "Warning: This part contains features that cannot be unbent."

I just don't understand why it is giving me an error because the part is pretty simple and doesn't seem like it cannot be unfolded...

Does anyone have an idea??? Please?

Thanks,

Uka

 

[MadMango]

Check to see if any flanges are over-lapping themselves.
Make sure there are only linear bends in the model.

Ray Reynolds
"There is no reason anyone would want a computer in their home."
Ken Olson, president, chairman and founder of Digital Equipment Corp., 1977
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[Uka]

Flanges are not being over-lapped, and bend lines are all linear...

The part is close to symmetrical. The tab feature on one side can be unfolded, but the other side tab cannot be unfolded. Both tabs have the same bend radius and everything. The only difference is that the tab that cannot be unfolded has a thru hole and slot feature...

Uka

 

[CorBlimeyLimey]

in your first post you metion "flatten" & in the second you say "unfold"! Which are you actually trying to do?


If you suppress, either or both the thru hole & slot feature, can you then flatten the part?

from Barrie, Ontario.

24 hours in a day ... 24 beers in a case ... coincidence?
faq559-863

 

[JNR]

The hole is not on the bend is it? You would haveto decide (even on the real part) if you want the hole to be circular after the fold or before.

In the first case you would have to machine it afterwards, so you would do the cut afterwards in SW also.



Barrie: I takes you a whole HOUR to finish a beer?!!!!



John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

Forget rich and famous - I want to be rich and unknown.

 

[TheTick]

If you are making an extruded cut through sheet metal, be sure you have the "normal cut" option checked.

 

[Dennyd]

If you are modeling the part as a fully featured part and then making it sheetmetal at the end (my personal preference) you should be careful with the following:
a. Make sure all thicknesses are exactly the same. (I've seen instances where someone made the thickness .062", .0625", and .063" all in the same part.)
b. Do not model the bends. Leave all bends sharp and let the radiused bends come from the sheetmetal function.
c. Watch how flanges/tabs hang off of edges.
d. Be sure to create the flanges normal to their flange face, not normal to a face it is bent from. This makes the edges perpendicular to their face, as they should be.
e. Holes and cuts cannot intrude into a bend tangenecy. (I suspect this might be your particular problem.) This is easy to look at by suppressing the holes and then executing "Insert Bends". If you need a hole or cut to span a bend tangency SWX models the deformed hole beautifully, but you have to create the hole on the flattened sheet by creating the feature between the flat pattern and the process bends feature created by the sheetmetal function.

If you are having trouble flattening a feature then simplify it to investigate.

- - -Dennyd

 

[Uka]

Thank you everyone!!

(CorBlimeyLimey - I meant flatten...)

I am going try to investigate some more to see what is causing this problem.

 

[CorBlimeyLimey]

The simplest way to check what is causing the problem, would be to suppress all but the base feature, then check to see if Flatten[ works. If it does, then "un-flatten" the part, then unsupress the next feature & try Flatten & so on.
Let us know what caused the problem when you find out.

from (the City of) Barrie, Ontario.

OK, so….what's the speed of dark?
faq559-863

 

[SBaugh]

I do it differently than you do CorBlimeyLimey. I Unsuppress the Flat-pattern and let it error. I then suppress about 4 features at a time to see if the flat-pattern flattens. If it does then I know the problem is within the last 4 features. I then unsuppress them till it bends up.

Either way works - It's just what you find to be more efficient for you.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

SBaugh
That's one of the best & worst things about SolidWorks. There are several ways to do most things, some just become personal preference. I personally like having the choices, but sometimes it is expedient to just have the "Right" way to do it, "Cut & Dried".

from (the City of) Barrie, Ontario.

OK, so….what's the speed of dark?
faq559-863