Hide Table of Contents

Trim Entities

Select the trim type based on the entities you want to trim or extend. All trim types are available with 2D sketches and 2D sketches on 3D planes.

To trim a 3D sketch:

  1. Start the 3D sketch on a 2D plane.

  2. Then do either of the following:

    • Right-click and select 3D sketch on a plane.

    • Double-click a plane or sketch entity.

You can use any of the following trim options:

Power Trim

Use Power trim to:

  • Trim multiple, adjacent sketch entities by dragging the pointer across each sketch entity.

  • Extend sketch entities along their natural paths.

Arcs have a maximum extension length on either side of the arc. Once you reach the maximum extension length, the extension shifts to the opposite side.

To trim with the Power trim option:

  1. Right-click the sketch and select Edit Sketch.

  2. Click Trim Entities Sketch toolbar) or Tools, Sketch Tools, Trim.

  3. In the PropertyManager, under Options, select Power trim .

  4. Click in the graphics area next to the first entity, and drag across the sketch entity to trim.

  • The pointer changes to as it crosses and trims the sketch entity.

  • A trail is created along the trim path.

  1. Continue to hold down the pointer and drag across each sketch entity you want to trim.

  2. Release the pointer when finished trimming the sketch, then click OK .

Power trim - trim

To extend with the Power trim option:

  1. Follow steps 1 - 3 from the preceding procedure.

  2. Select anywhere along the sketch entity to extend.

  3. Click and drag the pointer as far as you want to extend the sketch entity.

  4. Release the pointer when finished extending the sketch entity, then click OK .

Power trim - extend

Return to trim options

Corner

Extends or trims two sketch entities until they intersect at a virtual corner.

To trim with the Corner option:

  1. Right-click the sketch and select Edit Sketch.

  2. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim.

  3. In the PropertyManager, under Options, select Corner .

  4. Select the two sketch entities you want to joined.

Depending on the sketch entities and their relative position to each other, the software extends or trims each entity to join them. A message appears when the operation cannot be completed.

  1. Click OK .

Corner

Return to trim options

Trim Away Inside

Trims open sketch entities that lie inside two bounding entities.

To trim with the Trim away inside option:

  1. Right-click the sketch and select Edit Sketch.

  2. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim.

  3. In the PropertyManager, under Options, select Trim away inside .

  4. Select two bounding sketch entities.

  5. Select the sketch entities to trim.

  The sketch entities you select to trim must either intersect each bounding entity once, or not intersect the two bounding entities at all.

  1. Click OK .

Trim away inside

Return to trim options

Trim Away Outside

Trims open sketch entities outside of two bounding entities.

The same rules that govern the Trim away inside option govern the Trim away outside option.

  1. Right-click the sketch and select Edit Sketch.

  2. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim.

  3. In the PropertyManager, under Options, select Trim away outside .

  4. Select two bounding sketch entities.

  5. Select the sketch entities to trim.

  6. Click OK .

Trim away outside

Return to trim options

Trim to Closest

  1. Right-click the sketch and select Edit Sketch.

  2. Click Trim Entities on the Sketch toolbar, or click Tools, Sketch Tools, Trim.

  3. In the PropertyManager, under Options, click Trim to closest .

The pointer changes to .

  1. Select each sketch entity you want trimmed or extended to the closest intersection:

  • To extend, select the entity and drag to the intersection.

  • To trim, select the sketch entity.

  1. Click OK .

Trim to closest

Return to trim options



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:   Trim Entities
*Comment:  
*   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:



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 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.