Do it again & again & again – Design Library & a couple of Other Old Favourite Features #SolidWorks

Over the past couple of weeks I’ve spent a bit of time working, in SolidWorks, with a few new cabinet designs.   It’s reminded me of just how good, a few features that have been around for a few years, really are!

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The first of those would be Design Library.   Design Library has been around for as long as I can remember.  Which is why I’ll make a slightly embarrassing confession a little further on!  Once you have created something in SolidWorks you should never have to recreate it over again.   One of the reasons Design Library is so good is it take away the repetition and need to recreate the same sketch (or feature! But more of that later!)

Any sketch or annotation can be added to the Design Library.  Select “Add to Library” from the Task Pane.  Select the required sketch or annotation, name and select the Folder where you want it to live! 

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To use the sketch, start a new sketch on the require plane/ face and drag that sketch from the Task Pane.  The sketch come in as a block, add Relations/ dimensions to fully define.

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Swept Boss/Cut has always been a cool features and was greatly improved with the addition of Selection Manager.  Selection Manager has been around for a while now (I’ll say 2007 / 2008!) and greatly assisted in the creations of Sweeps and Lofts!

The sketch block forms the Profile so the Path needs to be created.   RMB in the Graphic area or Path Box and select SelectionManager. 

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In this case the outer edge is required for the Path.  As it’s an Open Group select this from the pop up box.    The individual sections can be selected (they will turn pink) You could continue to add each individual section you require or (as I recently discovered) after the first selection a small box shows.  If you select this box it will select the rest of the ”chain” (and displays pink).  Complete by accepting the selection with the tick.

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“Open Group” is shown and the Sweep is previewed.

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The Completed Sweep

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Remember the remark about the embarrassing confession! Well here it comes! For all the years I’ve been using the Design Library I never used or added a “Design” Feature!  That’s correct as well as being able to use sketches/ annotations you can use certain features!  You need to first create a “Base Feature”  (Extrude rectangle) The “features” required are the two Cut-Extrude circles. 

Select “add to Library” from the Task Pane.  Change the Options – File Type: to Analysis Lib Part.

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Select the required features (in this case the two Cut-Extrudes), name and add to the required Folder.  A Library Feature Part (sldlfp) will be created

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If you Open the create part (sldlfp), you’ll note there are Reference, Dimensions and Locating Dimensions Folders.  You can drag dimension that you wish to use into the Locating Dimension Folder

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To add the Library Feature Part into a part.  Drag from the Task Pane onto the face of the part.  A preview window opens and the Reference box shows question marks against the positioning reference. The highlighted reference (in the preview window – is blue) it can then be selected on the part (shown -Orange).  The Reference will change from the question mark to a tick!

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Select all references and the feature is positioned and complete.  

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For reducing time and saving on repetitive tasks you can’t go past Design Library and Selection Manager!   (and now I’m less embarrass for confessing my sins and having now had the opportunity to use Library Feature Part in Design Library)

Although I haven’t had a chance to try there has been some enhancement to the Library Feature for SolidWorks 2013. I believe that Library Feature can now be created from Multi-bodies and be added into Weldments.  Have a look at: 

http://www.solidworks.com/launch/model-creation.htm?scid=sm_tw_launch13_weldments

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