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Sheet Metal Symbol in a file. How can i fix it?

Question asked by Ali Can Guler on Apr 11, 2018
Latest reply on Apr 13, 2018 by Ali Can Guler
  • Comment • 7

Hello;

At the attachment as you can see difference between sheet metal symbols. How i fix it? First picture is the correct one.

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                 Correct                                                  False

Problem.jpg

Frank Ruepp
Frank Ruepp Employee Apr 13, 2018 5:31 AM
Correct Answer

Hi Ali,

 

SolidAir  is right.  We did this architectural change with the 2013 release.  With 2010 we introduced Multi Body Sheet Metal architecture and this architecture required some overhaul since we became aware of issues related to the "old way" we did things.

Therefore we did this quality project in 2013 that introduced the top level sheet metal folder and the lower level sheet metal body defintion.  However both architectures are not compatible.  Means that any file created before SOLIDWORKS 2013 will rely on the old architecture and any file starting with SOLIDWORKS 2013 will use the new architecture.  There is currently no way how you can "update" a pre 2013 file to the new architecture (we are not offering this upgrade mechanism since there is a small chance that some files might get corrupted or would be unintentionally altered).

BUT:  You have to be aware that if someone creates a new (sheet metal) file with 2013 or later that is based on a template created in 2012 or earlier he will get the old architecture since it is saved with the template and we cannot update the architecture.

 

I have a feeling that some of the confusion arises from the different approach the new files use.  Basically we have two possible places where you can define your sheet metal defintion:

  1. At the folder level:

    Where you can define generic sheet metal parameters that get applied to all of the bodies underneath (depending on your selected options):
  2. Or at the body level:

    Where you can override the top level sheet metal folder defintion:



  3. The default behavior can be set up through the sheet metal settings of the document properties:

    There you can set up the default behavior whether the body sheet metal settings should retrieve the sheet metal folder settings or not.

  4. Let me explain the behavior with an example.  My part template has these sheet metal document properties:

    Means that my sheet metal body defintions will retrieve the sheet metal information from the sheet metal folder defintion.

  5. So I am creating my first sheet metal feature and with it I am setting the sheet metal parameters that will be propagated to the sheet metal folder:
  6. After I have created the feature the sheet metal folder defintion will inherit the parameters I defined in the feature:



  7. Now, when I create a new sheet metal body it will automatically inherit these sheet metal folder defintion:

    Since my document settings state that every new sheet metal body should inherit the sheet metal folder parameters.

  8. So if I would like to make changes to the sheet metal parameters of the second body I have to edit the body specific sheet metal parameters:


    Override the default parameters and set up new values for i.e. material thickness, bend radius, k-factor.

 

So to summarize:  There is a distinction between general sheet metal parameters applied to the sheet metal folder container and there are individual body specific sheet metal parameters for each (sheet metal) body.  You can set up the default behavior whether the default sheet metal parameters should be used or overridden by default with the sheet metal document properties saved with the template.

Any individual body specific sheet metal definition can be manually overridden at any time.

 

Hope this helps.

Kind regards

Frank

SOLIDWORKS Product Defintion Team

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