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Am I Doing This Right?

Question asked by Bill Schmid on May 16, 2014
Latest reply on May 19, 2014 by Bill Schmid

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I work with many sheet metal parts on a daily basis, although I've had very little formal training in SolidWorks. Most of the the legacy parts I work with are structured like this:

an extrusion
couple cuts or holes
a sheet metal feature that converts the part to sheet metal
flatten bends
process bends

But when I create a new part, starting with an extrusion, I get this:

an extrusion
a cut
a sheet metal feature that converts the part to sheet metal
a convert solid feature
an unfold feature
a fold feature
and a flat pattern feature.

Did SolidWorks change the way it creates sheet metal models, or am I doing something wrong? It seems like the old way was better, but I don't see anything in the menus that look like they'll create parts the old way.

Thanks!

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Patrick O'Hern May 16, 2014 5:16 PM
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Solidworks has changed the way sheet metal parts are made (starting in SW 2013). I believe the changes were mostly to improve how it handles multibody sheet metal parts (the changes are required even if you only have one body).

Why not just create your part using the sheet metal tools to begin with, rather than using Convert to Sheet Metal?
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- Roland Schwarz @ Patrick O'Hern on May 19, 2014 8:41 AM
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  Why not just create your part using the sheet metal tools to begin with, rather than using Convert to Sheet Metal?
  Because sometimes that actually makes things more difficult. Especially true for Z-brackets designed in-context that have interfaces on both sides of the sheet.
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Erik Bilello May 16, 2014 8:24 PM
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Bill,

It looks like you may be dealing with very legacy parts. The original way to make a sheet metal part was to make a uniformly thick part and then apply the sheet metal feature. That produced a feature tree like you describe. Eventually it became possible to create a Base Flange/Tab as the first feature which eliminated the need to "convert" a part to sheet metal. This is also when the sheet metal toolbar came along, with the ability to select an edge and insert a flange, and all the other handy features. The convert to sheet metal functionality was not removed because it is still sometimes necessary (imported parts that need to have flat patterns created, flat parts created with Extruded Boss/Base that get revised to have flanges, etc.)

I have seen SW 2013 texts that still teach the convert to sheet metal method, but I practically never see a reason to model that way anymore. My rule is to always use the sheet metal Base Flange/Tab to create sheet metal parts, even ones that aren't going to have bends and don't need a flat pattern. Parts have a habit of changing and that flat "plate" becomes a "bracket" with a flange or two.

So, I agree with Patrick, use the sheet metal tools from the start whenever you can.
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- Bill Schmid @ Erik Bilello on May 19, 2014 7:39 AM
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  Thank you Patrick and Erik. I tried the base flange method. I do see an advantage to being able to sketch a thin rather than a uniform thickness sketch. But at the same time, I'm going to miss being able to slide the end of part marker back one feature to see the flat pattern. Yes, I can resume and suppress the Flat-Pattern1 feature, but it's more clicks. I suppose it's just getting used to a new process.
  
  The product line I'm working with is a very mature product. It's design is very well established. The shapes change very little. So most of what I'm doing is taking an existing design and applying new dimensions. That's how we have some of those very legacy parts.
  
  We are currently on 2010 with an upgrade to 2013 expected in the near future. Our CAD upgrades are somewhat governed by what works with and what's been tested with whatever version of SmarTeam we're using. Once the upgrade happens, I plan on getting training to bring me up to date.
  
  Bill
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  - Erik Bilello @ Bill Schmid on May 19, 2014 10:44 AM
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    Bill,
    Check out the other buttons on the sheet metal tool bar. The show flat-pattern button is the forth one up from the bottom (just above the two greyed out ones) in the image I posted.
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    - Bill Schmid @ Erik Bilello on May 19, 2014 11:00 AM
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      Erik,
      
      Yup, found it! Thanks. I really don't use the sheet metal menu that much because the shapes of the sheet metal components I use don't change much - only their dimensions. Consequently I'm not that familiar with it. But, after experimenting with it earlier this morning, I noticed the Flatten button. That seems to do whatever is necessary to the model tree to get to the flat state. Whether it's rolling back before the Process-Bends feature or unsuppressing the the Flat-Pattern feature. So that's actually quicker than the manual roll-back method I was used to using. I just need to re-train myself to use it.
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