SolidWorks: Virtual Components

Chances are, you’ve needed to create an assembly with numerous components with irrelevant geometry such as wires, glue, or oil. Giving each individual wire a part number can be overwhelming and unnecessary when searching for files in your directory. With SolidWorks Virtual Components, you are given the ability to create parts that exist only within an assembly. This feature is also very useful when in the early stages of a design and parts are being made on the fly for unofficial revisions and it is not determined whether or not they will require a part number.

NOTE 1: As the virtual parts are only existent in the assembly file, corruption of this file will result in the loss of all corresponding virtual components.

NOTE 2: As the virtual parts are only existent in the assembly file, you will not be able to search for them within your file directory. Also, if you use PDM the virtual components will not show up in the “Bill of Materials” or “Contains” tabs.

To create a virtual part, open a new assembly and under the “Insert Components” drop-down, select “New Part”

You will then be prompted to select a plane which will coincide with your virtual part’s front plane. You will notice that the names of all virtual parts are in brackets. You can now carry out your modeling practices as you would with any in-context, or top-down, model. When you attempt to save the assembly, you should be prompted with the following pop-up.

By saving internally, you are keeping the files virtual, meaning the only place they exist is within the assembly file. By choosing to save externally you will be given the option to choose the path where the files will be saved (the default being where the assembly is saved). Once saved externally, a new SolidWorks part file will be created with all the features carried over from the Virtual Part. The part file will have whatever name the virtual part had in the feature tree. To cut down on potential steps it is advised that if you use virtual components, to name a part to the desired name in the feature tree before saving externally. Once saved externally you have the option to leave all external references or go into the file and break all external references and define the part internally. If you would like to save individual virtual parts externally, right-click on the part in the feature tree and select the “Save Part(in External File)” option.

This process can also be reversed. To do this, just as with above, right click on the part file and select the “Make Virtual” option.

Once a part is made virtual, its link with the original part is broken. Therefore, any changes or deletion of the original file will not affect the assembly file with the virtual file. An example of using this feature is with parts made of a flexible material such as rubber. For example, an O-ring. You can have a default orientation (round) saved. Now this file can be brought into an assembly, made virtual, and changed to fit the shape of the housing groove, leaving the original O-ring template file untouched. The properties will come from the template file, ensuring your BOM shows the proper data.

You can also create virtual sub-assemblies. This is done with the same method as creating a virtual part. You can add parts by editing the assembly or by dragging and dropping part files from the feature tree onto the sub-assembly. It should be noted that dragging and dropping a file from the feature tree into a virtual sub-assembly will not make the part virtual.

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