Hide Table of Contents

Multibody Parts Versus Assemblies

Multibody parts should not replace the use of assemblies.

A general rule to follow is that one part (multibody or not) should represent one part number in a Bill of Materials. A multibody part consists of multiple solid bodies that are not dynamic. If you need to represent dynamic motion among bodies, use an assembly. Tools such as Move Component, Dynamic Clearance, and Collision Detection are available only with assembly documents.

Saving an Assembly as a Multibody Part

You can save an assembly as a multibody part document. This enables you to save complex assemblies as smaller part documents to facilitate sharing files. For example, you have a design of an intricate motor assembly and a potential customer wants to know if it fits in their frame. You can save the motor assembly as a part document and send the part file to potential customers without risking design integrity or transmitting a large assembly document file.

To save an assembly as a multibody part document:

  1. Open an assembly document.
  2. Click File > Save As.

    The Save As dialog box appears.

  3. Set the Save as type to Part (*.prt, *.sldprt).

    A set of options appears at the bottom of the dialog box.

  4. Select one of the following:
    • Exterior Faces to save the exterior faces as Surface Bodies .
    • Exterior Components to save the visible components as Solid Bodies .
    • All Components to save all components as Solid Bodies .
      Components that are hidden or suppressed are not saved when you select All Components.
  5. Click Save.

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Multibody Parts Versus Assemblies
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2015 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.