Part; Flat Pattern.

[Anonymous]

I'm a ProEngineer user of 10 years but just started at a new company that has Inventor/Sheet Metal package that I'm teaching myself, they've never used it before.

I started my current project by creating a sheet metal part and set the material thickness at the beginning. When I was finish the part flat pattern worked just fine.

The next thing I did was start an assembly and insert my initial part to create additional parts of it because of the unusual geometry. Now the assembly is complete and I open the other parts individually but the flat patter doesn't work.

If I convert the part to a model and then back to a sheet metal part I get the message "For proper unfolding the model should have uniform thicknes..." but I can't find where to set this in the part file or the assembly.

Is this something I should've done at the beginning of my assembly creation and can it be fixed at this point?

[JDMather]

You could have selected sheet metal template when creating additional sheet metal parts in the context of the assembly.
Easy fix. Open (or double click to edit) the parts and go to Convert>Sheet Metal. Then set the thickness in sheet metal styles. If you have trouble figuring it out zip and attach what you have so far.

It sounds like you already know how to convert to sheet metal. The first tool in the sheet metal panel bar is the Styles. You can use the styles editor or uncheck to override the thickness. I suspect you created your parts using standard features - you must be very carefull to maintain constant part thickness.

As a beginner you might want to go through these documents (there are slight differences - so go through both)
http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf
http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

These should save you a lot of frustration when things are a bit different than in Pro/E.

Edited by: JDMather on Jan 6, 2009 8:57 AM

Edited by: JDMather on Jan 6, 2009 9:13 AM

[Anonymous]

I'm going to attach what I have so far and it's the back and front parts that I'm having trouble unfolding. I did use standard features to create these part but they're essentially very simple and when creating the base solid off the assembly I projected the geometry of the asm and them offset it to achieve what I hoped would be uniform thickness. I'd really appreciate you taking a look at it for me.

Maybe, because of having no training with this package, I'm not understanding the concept of designing with it. Am I correct in assuming that when ever possible you should use the sheet metal features in your part and stay away from standard features?

Thanks for the help.

[Anonymous]

You are correct that whenever possible you should only use SM
features. You can use part features but you should have experience as to what
you can and can't do before you start dabbling in that area.

I took a look at your part and the reason its not flattening
is because of the way it was drawn. In order for a part to flatten all the
corners must be tangent. You can't have a non-tangent bend. If you look at your
part especially the back part, you will notice that the one corner is sharp and
not tangent. IV cannot unfold this. IN order to fix this you could either redraw
the part so that it is tangent, or you could add a fillet on the inside and
outside in order to create that tangent. The fillet would of course have to be
the same as your bend radius on the inside and the bend radius plus your
material thickness on the outside

style="PADDING-RIGHT: 0px; PADDING-LEFT: 5px; MARGIN-LEFT: 5px; BORDER-LEFT: #000000 2px solid; MARGIN-RIGHT: 0px">

"Deadhorse" wrote in message
title="news:6099136@discussion.autodesk.com CTRL + Click to follow link"
href="news:6099136@di......

I'm
going to attach what I have so far and it's the back and front parts that I'm
having trouble unfolding. I did use standard features to create these part but
they're essentially very simple and when creating the base solid off the
assembly I projected the geometry of the asm and them offset it to achieve
what I hoped would be uniform thickness. I'd really appreciate you taking a
look at it for me. Maybe, because of having no training with this package, I'm
not understanding the concept of designing with it. Am I correct in assuming
that when ever possible you should use the sheet metal features in your part
and stay away from standard features? Thanks for the help.

[JDMather]

You do not have a bend along the red edge shown in attached - this means you material is not uniform thickness.

The best way to model something like this is with a surface that you then Thicken.

[JDMather]

Even on your Top part that did flatten if you go to wireframe view mode and look at the edges you will see double lines indicating the that the cuts are not perpendicular to the flat. This will make the part more expensive to manufacture. Using Thicken of a surface body will eliminate this problem.

For this design I would
Model the Base as a single solid part.
Then start a new sheet metal part and exit sketch mode.
Select Derived Component and set to Body as Work Surfaces.
Thicken appropriate faces for Top. (some sheet metal parts are easier using the standard features)

Repeat for Front and Back. (be sure to add tangent to edge indicated earlier)

Post back if you have trouble figuring it out. Edited by: JDMather on Jan 6, 2009 12:40 PM

[Anonymous]

Guys-

Thanks for on your help on this. Could some one take a look at this part I created today and tell me why this one won't unfold, I was very careful to make sure it's uniform thickness.

[Anonymous]

Your thickness appears to be uniform, but it doesn't match the thickness defined in your sheetmetal style. Change the style thickness to match your part thickness and it unfolds.

[Troy_Grose]

I would not model it the way you created the part. See attached for how I would model it (using the sketch you created) There is no reason to even go into the part features for this part. SM features will do everything. Also stay away from adding fillets to corners where you can just use the bend tool. This way when you change the thickness in the styles dialog, everything updates correctly.

[Anonymous]

Not 100% sure on your design intent (as your original sketch was not completely constrained) ... but here is yet another way of creating the part (as you can see by the attached part).

1) Create a sketch of the flat pattern

2) Add construction lines for the bend locations

3) Add bends

- - - - -

Advantages:

a) Flat pattern is identical to your original sketch -- always able to unfold.

b) Failures when applying bends highlight potential manufacturing problems.


Disadvantages:

a) Achieving specific dimensions for formed part may require iterative tweaking of flat pattern.