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Insert Part

Use Insert Part to insert a base part into another part document. When you insert a part into another part:

  • The part you insert becomes a solid body.

  • If the inserted part contains mate references, you can use them to position the inserted part. A Body-Move/Copy feature is added to the FeatureManager design tree.

  • You can move and rotate the body after you place it.

To insert a part:

  1. With a part document open, click Insert Part (Features toolbar) or Insert, Part.

  2. Browse to a part document and click Open.

    The Insert Part PropertyManager appears.

  3. Under Transfer, select any combination of the following:

    • Solid bodies. Inserts the solid bodies.

    • Surface bodies. Transfers surfaces.

    • Axes. Transfers the axis information.

    • Planes. Transfers all planes from the original part.

    • Cosmetic threads. Transfers cosmetic threads.

    • Absorbed sketches. Inserts absorbed sketches from the inserted part.

    • Unabsorbed sketches. Inserts unabsorbed sketches from the inserted part.

    • Custom properties. Transfers all custom properties that have been defined for the inserted part.

    • Coordinate systems. Inserts the coordinate system of the inserted part into the derived part. You can use the coordinates of the two parts to create a mate by selecting Locate Part under Launch move dialog and aligning the axes of the coordinate systems.

    • Model dimensions. Imports model dimensions of the inserted part into the derived part.

    • Hole wizard data. Transfers data about the source part's Hole Wizard holes, so that the data is available in drawings of the derived part.

All transferred elements of the inserted part are placed in folders under the inserted part in the FeatureManager design tree.

  1. Under Locate Part, select Launch move dialog to define a location for the inserted part in the Locate Part PropertyManager.

  2. Optionally, if you want to independently edit the features of the inserted part without affecting the original part, under Link, click Break link to original part.

You can also break the link to the original part later by listing the derived part's external references and selecting Break All.

Once you break the link to the original, you cannot restore it.

  1. Click .

After you insert a part, you can move, copy, rotate, or mate it using Move/Copy Bodies (Features toolbar).

To change the configuration of the inserted part:

  1. Right-click the part and select List External Refs.

  2. Select a configuration in Configuration Name, and click OK.

You can also control the configuration with a design table. See Base Parts in Configurations.

Related Topics

Derived Parts

 



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Web Help Content Version: SOLIDWORKS 2012 SP05

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