Expand IntroductionIntroduction
Expand AdministrationAdministration
Expand User InterfaceUser Interface
Expand SolidWorks FundamentalsSolidWorks Fundamentals
Expand Moving from 2D to 3DMoving from 2D to 3D
Expand AssembliesAssemblies
Expand CircuitWorksCircuitWorks
Expand ConfigurationsConfigurations
Expand SolidWorks CostingSolidWorks Costing
Expand Design CheckerDesign Checker
Expand Design Studies in SolidWorksDesign Studies in SolidWorks
Collapse Detailing and DrawingsDetailing and Drawings
Detailing Overview
Setting Detailing Options
Model Items
Model Items PropertyManager
Expand eDrawings MarkupseDrawings Markups
Expand StyleStyle
Add or Update a Style
Expand AnnotationsAnnotations
Expand TablesTables
Expand Bill of Materials (BOM)Bill of Materials (BOM)
Expand Drafting StandardsDrafting Standards
Expand Print SettingsPrint Settings
Collapse DrawingsDrawings
Expand Getting Started in DrawingsGetting Started in Drawings
Expand Types of Drawing DocumentsTypes of Drawing Documents
Expand Standard Drawing ViewsStandard Drawing Views
Collapse Derived Drawing ViewsDerived Drawing Views
Drawing View Display State
Jump to Parent or Child View
Expand Projected ViewProjected View
Expand Auxiliary ViewAuxiliary View
Expand Detail ViewDetail View
Expand Modifying a Detail ViewModifying a Detail View
Crop View
Collapse Section Views in DrawingsSection Views in Drawings
Expand Inserting a Section ViewInserting a Section View
Expand Inserting a Section View with OffsetInserting a Section View with Offset
Section View PropertyManager
Additional Features of Section Views in Drawings
Creating a Section View Manually
Section Scope
Changing the Orientation of a Section
Expand Modifying Section ViewsModifying Section Views
Section View PropertyManager (Drawings)
Section Display Types
Troubleshooting Section Views
Expand Broken-out SectionBroken-out Section
Rotated Section Views
Part Cutaway Views
Assembly Cutaway Views
Expand Broken ViewBroken View
Expand Alternate Position ViewAlternate Position View
Position Schematic PropertyManager
Section Scope
Modify Section Line Properties
Section Display Types
Troubleshooting Section Views
Section View PropertyManager (Drawings)
Redrawing OLE Items in Drawings
Multiple Views PropertyManager
Convert View to Sketch PropertyManager
Expand Drawing View Alignment and DisplayDrawing View Alignment and Display
DrawCompare
Drawing Statistics
Printing Drawings
Send Mail
Expand Title Block ManagementTitle Block Management
Expand Dimensions in DrawingsDimensions in Drawings
Expand DFMXpressDFMXpress
Expand DriveWorksXpressDriveWorksXpress
Expand FloXpressFloXpress
Expand Import and ExportImport and Export
Expand Model DisplayModel Display
Expand Mold DesignMold Design
Expand Motion StudiesMotion Studies
Expand Parts and FeaturesParts and Features
Expand RoutingRouting
Expand Sheet MetalSheet Metal
Expand SimulationSimulation
Expand SimulationXpressSimulationXpress
Expand SketchingSketching
Expand Sustainability ProductsSustainability Products
Expand SolidWorks UtilitiesSolidWorks Utilities
Expand TolerancingTolerancing
Expand TolAnalystTolAnalyst
Expand ToolboxToolbox
Expand WeldmentsWeldments
Expand Workgroup PDMWorkgroup PDM
Expand TroubleshootingTroubleshooting
Glossary
Hide Table of Contents

Section View PropertyManager (Drawings)

To open the Section View PropertyManager:

Create a section view in a drawing and click Edit sketch in the PropertyManager, or select an existing section view.

Section Line

PM_line_settings.gif Flip direction You can also reverse the cut direction by double-clicking the section line.
PM_label.gif Label Edit the letter associated with the section line and section view.
  Font To choose a font for the section line label other than the document's font, clear Document font and click Font. If you change the section line label font, you can apply the new font to the section view label.

Section View

Partial section Creates a section view that is limited by the length of the section line if the line does not span the entire view.
Display only cut faces Shows only the faces cut by the section line.
  Complete section
drw_section_complete.gif
Partial section
drw_section_partial.gif
Display only cut faces
drw_section_surface.gif
Auto hatching Crosshatch patterns alternate between components in assemblies, or between bodies in multibody parts and weldments. The hatch patterns alternate when sectioning an assembly.
auto_hatch.gif
Display surface bodies Shows a section view of surface bodies from a parent view of a model. You can apply annotations such as notes and dimensions to the cross section of the surface. This setting persists across sessions.
surface_section_view.png
Hide cutting line shoulders hide-cutting-lines.gif
Foreshorten view foreshortened1.gif
Toggle Alignment Click to change the alignment of the section view.
toggle-alignment-1.gif
toggle-alignment-2.gif

Section Depth

Lets you set the depth of a section view to a distance you specify. This control is only available for section views whose cutting line consists of a single line segment.

Distance section views apply to components, not features.
To set a distance, do one of the following:
  • Set a value for Depth dim_lin_d.png.
  • Select geometry, such as an edge or an axis, in the parent view for Depth Reference select_edge_faces_vertex.png.
  • Drag the pink section plane in the graphics area to set the depth of the cut. All components between the section line and section plane will be shown in the section view.
Preview section_view_distance.gif

Import annotation from

Import annotations Select Import annotations to all selected types of annotations to be imported from referenced part or assembly documents.
Select annotation import options:
  • Design annotations
  • DimXpert annotations
  • Include items from hidden features

Display State

For assemblies only. Select a display state of the assembly to place in the drawing.

The hide/show display_pane_column_hideshow.gif display state is supported by all display styles. Other display states (display mode display_pane_column_display_mode.gif, color display_pane_appearance.gif, etc.) are supported by Shaded with Edges Tool_Shaded_With_Edges_View.png and Shaded modes Tool_Shaded_View.png only.

Display Style

Use parent style Clear to select style and quality settings different from those of the parent view.

Click a display style.

Select High quality or Draft quality to set the display quality of the model. This is available only when Display quality for new views is set to Draft quality. If you select High quality, these options do not appear again.

Scale

Use parent scale Applies the same scale used for the parent view. If you change the scale of a parent view, the scale of all child views that use the parent scale is updated.
Use sheet scale Applies the same scale used for the drawing sheet.
Use custom scale Applies a scale that you define. If you select User Defined, type a scale in the box below in the following format: x:x or x/x. Select Use model text scale to maintain the geometry used in the annotation views in parts.
The pre-set options in Use custom scale differ based on the dimensioning standard.

Dimension Type

Dimensions in drawings are either:
True Accurate model values.
Projected 2D dimensions.

The dimension type is set when you insert a drawing view. You can view and change the dimension type in drawing view PropertyManagers.

The rules for dimension type are:
  • SolidWorks specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.
  • If you create a projected or auxiliary view from another view, the new view uses Projected type dimensions, even if the original view used True type dimensions.

Cosmetic Thread Display

The following settings override the Cosmetic thread display option in Tools > Options > Document Properties > Detailing, if there are cosmetic threads in the drawing view.

High quality Displays precise line fonts and trimming in cosmetic threads. If a cosmetic thread is only partially visible, High quality shows only the visible portion (it shows precisely what is visible and what is invisible.)
System performance is slower with High quality cosmetic threads. It is recommended that you clear this option until you finish placing all annotations.
Draft quality Displays cosmetic threads with less detail. If a cosmetic thread is only partially visible, Draft quality shows the entire feature.

More Properties

See Drawing View Properties.



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:   Section View PropertyManager (Drawings)
*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 2014 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.