At the attachment as you can see difference between sheet metal symbols. How i fix it? First picture is the correct one.
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:
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.
SOLIDWORKS Product Defintion Team
I might be wrong but I believe this is the new way Solidworks shows the feature. It has the same feature inside a folder basically. I think this was added when the started offering multibody sheet metal parts.
As Casey Bergman stated, this is the new norm. Starting with SW2013 (not when SW started offering multi-body sheet metal parts though) the tree structure changed. Below is an excerpt from SW2013 What's New. You will need to get use to it because it is the same way in SW2018.
I want to disable this folder because sometimes affected my files. I can find any manuel about this. Do you know how can i do that?
I suppose you could suppress it (not recommended) or do not make your parts using sheet metal functionality. How is this folder affecting your files? All is does is group the sheet metal feature into a folder and limits or eliminates some functionality
I am using SW2014 and sometimes it is mixing thickness of the sheet. In the end it effect all assembly by that.
Thanks for reply SolidAir and Frank Ruepp.
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