{"id":1276,"date":"2017-09-13T11:21:17","date_gmt":"2017-09-13T09:21:17","guid":{"rendered":"https:\/\/cadbooster.com\/how-to-use-virtual-parts-solidworks\/"},"modified":"2023-07-23T16:18:32","modified_gmt":"2023-07-23T14:18:32","slug":"how-to-use-virtual-parts-solidworks","status":"publish","type":"post","link":"https:\/\/cadbooster.com\/nl\/how-to-use-virtual-parts-solidworks\/","title":{"rendered":"How to use virtual parts (and when to avoid them)"},"content":{"rendered":"

Virtual components are awesome.<\/p>\n

You can create hundreds of these models without creating a single file.<\/p>\n

You can dramatically improve your design speed by not having to come up with a name for each file.<\/p>\n

Just make sure you are aware of the trade-offs.<\/p>\n

In this post, you\u2019ll find<\/h3>\n
    \n
  1. How to add a new virtual part or assembly<\/a><\/li>\n
  2. Make virtual: what does it do?<\/a><\/li>\n
  3. Convert a virtual part to a normal part<\/a><\/li>\n
  4. InPlace mate and other mate options<\/a><\/li>\n
  5. Where are virtual parts stored?<\/a><\/li>\n
  6. When does SOLIDWORKS save a virtual model?<\/a><\/li>\n
  7. When you should use virtual components<\/a><\/li>\n
  8. When you should not use virtual components<\/a><\/li>\n
  9. Closing remarks<\/a><\/li>\n<\/ol>\n

    How to add a new virtual part or assembly<\/h3>\n

    Virtual components are assembly components (parts or subassemblies) that you can quickly add, edit and delete. They don’t need to be named or saved. You can recognize them by the circumflex symbol: part1^<\/span>assembly2.<\/p>\n

    You can only use virtual components in assemblies. You create a new one by selecting Insert<\/em> > Component<\/em> > New Part \/ New Assembly<\/em> or by clicking\u00a0these buttons in the Command Manager:<\/p>\n

    \"solidworks<\/p>\n

    (You can change a setting so that new parts are not virtual, which means you have to select a filename after creating one. Go to System Options<\/em> > Assemblies<\/em> > Save new components to external files.)<\/em><\/p>\n

    SolidWorks now prompts you for a reference plane, without really telling you. The plane you select coincides with the Front Plane of the new part.<\/p>\n

    After you select the front plane location, SOLIDWORKS goes into Edit Component<\/em> mode and it starts a new sketch on the Front Plane. It also adds a mate. The type of mate depends on what buttons you click in what order. More on that below.<\/p>\n

    Make virtual: what does it do?<\/h3>\n

    You can turn a standard part (that is, a part with a file name) into a virtual part.<\/p>\n

    Just right-click it (in the tree or in the modeling area) and select Make Virtual<\/em>.<\/p>\n

    \"solidworks<\/p>\n

    Convert a virtual part to a normal part<\/h3>\n

    You might use virtual components in the concept phase. In the next phase, you will have to convert all virtual models to normal files.<\/p>\n

    You can do this by right-clicking the part\/assembly and selecting Save Part(in External File)<\/em>.<\/p>\n

    InPlace mate and other mate options<\/h3>\n

    When you add virtual parts to an assembly, SOLIDWORKS helps you by fixing them in space. You can create three types of mating schemes:<\/p>\n

    Option 1: Fixed<\/h4>\n

    This is the default behavior. SOLIDWORKS fixes the part until you give it a better option. If you abort the process of assigning the front plane, the fixed relation remains. It’s not really a mate though.<\/p>\n

    Option 2: No mates<\/h4>\n

    This happens when you have selected the option ‘No External References’ in the Sketch toolbar before creating the new virtual model.<\/p>\n

    \"solidworks<\/p>\n

    This option is only available in Edit Component mode<\/em>. That means you might have to go into that menu once, just to make sure your next virtual part will be created without mates.<\/p>\n

    No mates are added whatsoever when you disable external references, so the part can freely float in space. In previous SOLIDWORKS versions, a fixed icon (f) appeared before the new part’s name when editing the first sketch. That icon disappears after you exit that sketch and return to the assembly.<\/p>\n

    Option 3: InPlace mate<\/h4>\n

    You have apparently not selected the option No External References<\/em> before creating the virtual part.<\/p>\n

    An InPlace mate will automatically replace the fixed relation when you select a front plane. That plane can either be a plane in the assembly or a face of another part.<\/p>\n

    InPlace mates are special mates for virtual parts and they appear in very few situations. I even wrote a short article<\/a> about them.<\/p>\n

    InPlace mates lock your part in place with regards to another part or assembly. You cannot edit InPlace mates, you can only delete them and replace them with a set of proper mates. I advise you to do just that, don’t leave them lingering around in your assembly.<\/p>\n

    \"solidworks

    When you try to edit an InPlace mate, you’ll receive this message.<\/p><\/div>\n

    \r\n

    Ditch the Toolbox, once and for all<\/h2>\r\nStart using the fastener library that actually follows the standards<\/span>\r\n
    \"\"<\/div>\r\n
    \r\n
    \r\n