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Working on Large Assemblies without Hardware

The idea of large assemblies in SOLIDWORKS is different for everyone as your perspective is usually based in some way on your hardware and hardware performance. At some point in the assembly creation, things start to seem slow and sluggish. In many cases, the assemblies are populated with thousand’s of pieces of hardware.


So this begs the question, “Can I make it so all the hardware is easily added and removed and only viewed as I need it?” Well, of course you can or I wouldn’t have enough content to write this blog post!

The answer to this question can be used as a technique for selecting groups of components in an assembly and then hiding, showing, suppressing or unsuppressing them as you continue to work on other parts of an assembly. Let’s take a look how this is done.

What is hardware?  Your definition of hardware may be different than other teams using SOLIDWORKS.  But let us get something clear… it is not only describing files created using the Toolbox add-in. In some cases, hardware can be a standard component that has been added from a library. It may also be purchased or even manufactured in bulk internally. In any case, you can define what you want to call hardware.

How do I  create an assembly view that I can work in that is free of any “hardware?” By using the “Select” and “Advanced Select” tools in SOLIDWORKS.


If we look at the select consolidated menu, you will see several predefined selection tools. One of them is called “Select Toolbox.” Now this may seem a bit confusing considering my previous statement about hardware not being toolbox-related. When the Toolbox add-in is used to create hardware, it automatically creates a custom property called “Isfastener” and sets its value to “Yes.” The property name “Isfastener” is used as the selection criteria when “Select Toobox” is selected.


That’s great! But how do we use that same technique for our definition of “hardware,” or something not created using the toolbox add-in When SOLIDWORKS is installed, it places a utility called sldsetdocprop.exe in the installation directory. Typical path is C:\Program Files\SolidWorks Corp\SolidWorks\Toolbox\data utilities. With this utility, you can set the “IsFastener” custom property to “Yes” on your hardware library. Just select the directories or files you would like to set the property on.


Open an assembly and activate the menu command for “Select Toolbox.” All files in the assembly that have the “IsFastener” property will be selected.


Now you can right click to choose whether you hide, show, suppress or unsuppress all the “Hardware.”


Do not let your team get slowed down by assemblies with lots of hardware. Using “Select Toolbox,” you can hide or show them very quickly and reduce the amount of data you are working on within the assembly environment.

Within the “Advanced Select” feature, you can set up advanced component selection criteria using custom properties other than ”IsFastener,” like maybe “IsSheetMetal” or “IsPurchased.” All you have to do is set the property in each file to take advantage of this very useful selection technique.

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