Hide Table of Contents

FeatureXpert

The FeatureXpert, powered by SolidWorks Intelligent Feature Technology (SWIFT™), manages fillet and draft features for you so you can concentrate on your design. See also Xperts Overview.

When you add or make changes to constant radius fillets and neutral plane drafts that cause rebuild errors, the What's Wrong dialog appears with a description of the error. Click FeatureXpert in the dialog to run the FeatureXpert to attempt to fix the error.

The FeatureXpert can change the feature order in the FeatureManager design tree or adjust the tangent properties so a part successfully rebuilds. The FeatureXpert can also, to a lesser extent, repair reference planes that have lost references.

Supported features:

  • Constant radius fillets

  • Neutral plane drafts

  • Reference planes

Unsupported items:

  • Other types of fillets or draft features.

  • Mirror or pattern features. When mirror or pattern features contain a fillet or draft feature, the FeatureXpert cannot manipulate those features in the mirrored or patterned copies.

  • Library features. Fillet or draft features in a library feature are ignored by the FeatureXpert and the entire Library feature is treated as one rigid feature.

  • Configurations and Design Tables. The FeatureXpert is not available for parts that contain these items.

To toggle activation of the FeatureXpert:

  1. Click Options (Standard toolbar) or Tools, Options, System Options.

  2. Select or clear Enable FeatureXpert.

  3. Click OK.

To add features using the FeatureXpert:

  1. Open a part to which you want to add fillets. In this example, you want to add a fillet to two faces.

  2. Click Fillet (Features toolbar) or Insert, Features, Fillet/Round.

  1. In the PropertyManager:

    1. Select Constant radius for Fillet Type.

    2. Set the Radius value.

The radius value you set affects whether you can add the fillet without the FeatureXpert.

  1. Select the two red faces for Edges, Faces, Features and Loops .

  1. Click .

The What's Wrong dialog appears. The fillet error is highlighted in the dialog with a description why the fillet is failing. The fillet cannot be applied as an individual fillet for geometric reasons.

  1. In the dialog, click FeatureXpert.

The FeatureXpert creates multiple fillets instead of one fillet that contains both faces. The FeatureManager design tree displays the fillets.

To change features using the FeatureXpert:

  1. Open a part containing fillets you want to change.

In this example, the entire part is filleted with a .1 inch radius fillet.

  1. Edit the fillet feature.

  2. In the PropertyManager, change the Radius to .25.

  3. Click .

The What’s Wrong dialog appears. The fillet error is highlighted in the dialog with a description why the fillet is failing.

  1. In the dialog, click FeatureXpert.

The FeatureXpert dialog reports on the progress. In this example, the FeatureXpert creates individual fillets as necessary, and places them in the proper order in the FeatureManager design tree to allow the model to solve.



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

 
*Email:  
Subject:   Feedback on Help Topics
Page:   FeatureXpert
*Comment:  

Print Topic

Select the scope of content to print:



x

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
x

Web Help Content Version: SOLIDWORKS 2012 SP05

The search functionality within the web help is in a beta test phase and you may experience periodic delays or interruptions in its performance. These are the normal and ordinary features of a beta test and shall not under any circumstances give rise to any liability on the part of Dassault Systèmes SolidWorks Corporation or its licensors. The topics within the Web-based help are not beta topics; they document SOLIDWORKS 2012 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.