Hide Table of Contents

Broken View

You can use a broken (or interrupted) view in a drawing. Broken views make it possible to display the drawing view in a larger scale on a smaller size drawing sheet. You create a gap or break in the view using a pair of break lines. Reference dimensions and model dimensions associated with the broken area reflect the actual model values.

Broken views include the following functionality:

  • You can specify the gap between the break lines and the extension of the lines beyond the part geometry in Document Properties - Detailing.

  • Dimensions that cross the break lines are broken automatically.

  • You can lock break lines in place. After breaking the view, dimension the break lines to a known portion of the geometry. These dimensions are only for use in the drawing document and do not appear on a printed drawing.

  • You can specify the line font for the break lines in Tools, Options, Document Properties, Line Font.

  • You can display dimension lines with a zig-zag by selecting Show dimensions as broken in broken views in Document Properties - Dimensions.

  • You can apply the Break View and Un-Break View commands to multiple views.

  • You can use multiple break lines in a view using any combination of horizontal or vertical break lines. All breaks use the same gap and break line style.

  • Broken views of flat pattern sheet metal parts include bend lines.

  • You can combine a broken view with one or more section views to create a rotated section (revolved section) view.

To create a broken view:

  1. Select a drawing view and click Break (Drawing toolbar) or click Insert, Drawing View, Break.

  2. Set options in the PropertyManager:

    • Add vertical break line

    • Add horizontal break line

    • Gap size. Sets the amount of space between the gap.

    • Break line style . Defines the type of break line.

In views with multiple breaks, the Break line style must be the same.

A break line attaches to the pointer.

  1. Click in the view twice to place two break lines, creating the break.

    The view is displayed with a gap in the geometry. In addition to model geometry, broken views also support cosmetic threads and axes.

  2. Add additional break lines as necessary. To create horizontal and vertical break lines in the same view, add multiple breaks using horizontal and vertical directions.

  3. Click .

To restore a broken view to its unbroken state:

Right-click the broken view, and select Un-Break View.

The break lines remain in the view and you can delete them.

To modify a broken view:

  • To change the shape of the break lines, right-click a break line and select a style from the shortcut menu.

  • To change the position of the break, drag the break lines.

  • To change the width of the break gap, select a break line and type a value in the PropertyManager.

You can select an Area Hatch in a broken view only in its unbroken state. You cannot select an area hatch that crosses a break.

To align a break in a projected view with a break in the parent view:

  1. Right-click in the projected view and click Properties.

  2. In the dialog box, select Align breaks with parent.

  3. Click OK.



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:   Broken View
*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 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.