Hide Table of Contents

Offset Entities

Offset one or more sketch entities, selected model edges, or model faces by a specified distance. For example, you can offset sketch entities such as splines or arcs, sets of model edges, loops, and so on.

You can offset finite lines, arcs, and splines. You cannot offset fit splines previously offset splines, or entities that would result in self-intersecting geometry.

If the original entity changes, then the offset entity also changes when you rebuild the model.

To create a sketch offset:

  1. In an open sketch, select one or more sketch entities, a model face, or a model edge.

  2. Click Offset Entities (Sketch toolbar) or Tools, Sketch Tools, Offset Entities.

  3. In the PropertyManager, under Parameters, set the following:

When you click in the graphics area, the Offset Entity is complete. Set the Parameters before you click in the graphics area.

  • Offset Distance . Set a value to offset the sketch entity by a specified distance. To see a dynamic preview, hold down the mouse button and drag the pointer in the graphics area. When you release the mouse button, the Offset Entity is complete.

  • Add dimensions. Include the Offset Distance in the sketch. This does not affect any dimensions included with the original sketch entity.

  • Reverse. Change the direction of a one-directional offset.

  • Select chain. Create an offset of all contiguous sketch entities.

  • Bi-directional. Create offset entities in two directions.

  • Make base construction. Convert the original sketch entity to a construction line.

  • Cap ends. Extend the original non-intersecting sketch entities by selecting Bi-directional, and adding a cap. You can create Arcs or Lines as extension cap types.

  1. Click or click in the graphics area.

An Offset Entities relation is created between the new sketch entity and the selected entity. If the original entity changes, the new entity updates to maintain the offset.

If you are creating a component or feature in the context of an assembly and Do not create references external to the model is selected in Tools, Options, External References, then the sketch relations described above are not created. See Controlling Creation of External References.

To change the size of a sketch offset:

Double-click the offset’s dimension and change the value. In a bi-directional offset, change the dimensions of the two offsets individually.

Related Topics

Convert Entities



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:   Offset Entities
*   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 2010 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.