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Top Down Design Overview
Creating a Part in an Assembly
Editing a Part in an Assembly
Inserting a New Sub-assembly
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Creating a Part in an Assembly

You can create a new part in the context of an assembly. That way you can use the geometry of other assembly components while designing the part.

You can also create a new sub-assembly in the context of another assembly. See Inserting a New Sub-assembly for more information.

Before creating new components in the context of an assembly, you can specify the default behavior for saving the new components either as separate external part files or as virtual components within the assembly file. See Saving New In-Context Components.

To create a part within an assembly:

  1. Click New Part (Assembly toolbar) or Insert, Component, New Part.

  2. For externally saved parts, type a name for the new part in the Save As dialog box and click Save.

  3. Select a plane or planar face (while the pointer is ).

    Editing focus changes to the new part and a sketch opens in the new part. An Inplace (coincident) mate is added between the Front plane of the new part and the selected plane or face. The new part is fully positioned by the Inplace mate. No additional mates are required to position it. If you wish to reposition the component, you need to delete the Inplace mate first.

    The new part appears in the FeatureManager design tree. Externally saved parts appear with a name in the form Part n. Virtual components appear with a name in the form [Part n ^ assembly_name ].

For internally saved parts, instead of selecting a plane, you can click in a blank region of the graphics area (while the pointer is ). An empty part is added to the assembly. You can edit or open the empty part file and create geometry. The origin of the part is coincident with the origin of the assembly, and the part 's position is fixed .

  1. Construct the part features, using the same techniques you use to build a part on its own. Reference the geometry of other components in the assembly as needed.

If you extrude a feature using the Up To Next option, the next geometry must be on the same part. Use Up To Surface to extrude to a surface on another component in the assembly or a surface of an assembly feature.

  1. To return editing focus to the assembly, click to clear Edit Component (Assembly toolbar), or click in the Confirmation Corner.

To save a virtual component to its own external file, right-click the component and select Save Part(in External File). Alternatively, when you save the assembly, you can select to save the part either inside the assembly or to an external file.

Related Topics

Layout-based Assembly Design

Editing a Part in an Assembly

Configurations and In-context Components


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