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Configurations and In-context Components

You can have more than one instance of an in-context component that is geometrically different in an assembly. To accomplish this, you must have the following:

  • A driving part with more than one configuration.

  • A sub-assembly with more than one configuration.

  • A driven part with more than one configuration. The driven part is built in the context of the sub-assembly referencing the different geometry in the two configurations of the driving part.

When you create components in the context of an assembly, the software saves them inside the assembly file, and you can immediately begin modeling. Later, you can save the components to external files or delete them. See Virtual Components Overview.

This example shows how to place geometrically different instances of the same component into an assembly.

  1. Create a cylindrical part named tube.

  2. Create two configurations of tube named large and small, each with a different diameter for the cylinder. (For information on creating configurations, see Creating a Configuration Manually.)

  1. Create an assembly named pipes, and insert tube into pipes.

  2. Create two configurations of the assembly pipes, named large and small. Specify the large configuration of tube for the large configuration of pipes, and the small configuration of tube for the small configuration of pipes. (For information on specifying component configurations, see Component Configurations in an Assembly.)

  3. Click New Part (Assembly toolbar) or Insert, Component, New Part, and create a part named plug in the context of the assembly.

To rename the in-context component, right-click it and select Rename Part.

  1. Select the face on the end of tube for the sketch plane.

  1. Select the outer edge of the face, then click Convert Entities on the Sketch toolbar, or click Tools, Sketch Tools, Convert Entities.

    A circle that references the outside diameter of tube is added to the sketch.

  1. Exit the sketch, then extrude a boss from the sketch.

  1. Click Edit Component (Assembly toolbar) to return to editing the assembly.

 

  1. Open plug in a separate window.

  2. Create two configurations of plug, named large and small.

  3. Return to the pipes document window, and activate the small configuration of pipes.

  4. In the FeatureManager design tree, right-click the component plug and select Component Properties.

  5. In the dialog box, under Referenced configuration, select small. Make sure Change properties in is set to This Configuration, then click OK.

    The diameter of the small configuration of plug (the driven part) is now defined by reference to the diameter of the small configuration of tube (the driving part).

  6. Activate the large configuration of pipes, and repeat steps 9 and 10 with the large configuration of plug.

Assigning the same names to the configurations in the driving part, the driven part, and the sub-assembly is not required, but helps you to keep them organized.

  1. Create another assembly, called plumbing, and insert two instances of the sub-assembly pipes. Set one instance of pipes to the large configuration and the other to the small configuration.

You now have two instances of the driven part, plug, that are geometrically different in the same assembly.

Related Topics

Component Configurations in an Assembly

Creating a Configuration Manually

Creating a Part in an Assembly



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