Hide Table of Contents

Locate Part PropertyManager

Use the Locate Part PropertyManager to move and rotate a part that you insert into another part.

The part you insert becomes a solid body. You can move and rotate the body after you place it. The part into which you insert the body becomes a multibody part.

To access the Locate Part PropertyManager, with a part document open, click Insert > Part and select a part to insert. In the Insert Part PropertyManager, under Locate Part, select Locate part with Move/Copy feature and click .

Click Translate/Rotate at the bottom of the pane to specify parameters to move or to rotate the body. A preview of the moved body appears.


Delta X, Delta Y, Delta Z Set values to reposition the body.
Translation Reference Locates the part using selected references. Select one of the following:

A linear edge

Defines the translation direction along which the inserted part moves. Set a value for Distance .

A vertex

Defines the starting vertex for the part translation. Select a vertex for To Vertex .

A Coordinate System

Defines the starting point for the part translation. Set values for Delta X, Delta Y, and Delta Z to reposition the part.

Distance Moves the part by this value in the direction of the edge selected for Translation Reference . Type a negative number to switch the translation direction.
To Vertex Moves the part in the direction and distance defined by the selected vertices.


Rotation Reference Defines the rotation axis using selections and values. Select one of the following:

A linear edge

Defines the edge as the rotation axis. Set a value for Angle .

A vertex or coordinate system

Defines the origin to use for the rotation. Set values for X Rotation Angle, Y Rotation Angle, and Z Rotation Angle.

Angle Sets the rotation angle around the selected edge for the inserted part.
X Rotation Origin, Y Rotation Origin, Z Rotation Origin Set values for the coordinates of the rotation origin (the point that the body rotates about). The default values are the coordinates of the origin of the part document.

A square appears in the graphics area to show the location of the rotation origin.

X Rotation Angle, Y Rotation Angle, Z Rotation Angle Sets the rotation angle around the selected axis.

Mate Settings

If Mate Settings is not displayed, click Constraints at the bottom of the PropertyManager. Select a mate type. All the mate types are always shown in the PropertyManager, but only the mates that are applicable to the current selections are available.

Entities to mate Select two entities (faces, edges, planes, etc.) to mate together. One entity must be from the body you are inserting into the part.
  Add Click to add the mate after selecting a mate type and setting parameters below.
  Undo Click Undo to clear selections.
Distance Select Flip Dimension to change the direction.
  Mate Alignment Select one of the following:


Places the body so the normal or axis vectors for the selected faces point in the same direction.


Places the body so the normal or axis vectors for the selected faces point in opposite directions.


The Mates box contains all the mates in the mate set (all the mates added while the PropertyManager is open). When there are multiple mates in the Mates box, you can select one to edit that mate.

In multibody parts, you can apply multiple sets of mates to the same body. Mates specified within different sets can conflict with each other. For example, you can apply a perpendicular mate between two faces in one set, and in a different set, apply a parallel mate between the same two faces.


Show preview When selected, a preview of a mate occurs when you make enough selections for a valid mate.

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:   Locate Part PropertyManager
*   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 2013 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.