When you create a section view, you draw a line that defines where to cut the section view. A section view can also be created by specifying a line in a drawing sketch that is associated with the parent view.

In the following image, a section view was used to expose components for ballooning.

A view cutting line knows what types of views can be projected from it. Depending on how the line is created, it can define the type of section view or define a boundary for a partial view.

The length of the cutting line defines the extent of the section view. A cutting line that passes only partially through the model view results in a partial section view.

If you draw the view cutting line outside the parent view, it defines a plane from which to project an auxiliary view.

Note

In an assembly view, components can be excluded from sectioning. In the browser, right-click the component to exclude, and then select None.
When creating a child (dependent) view, the section attributes of the parent view are copied to the child view, but they are not associative. Section view attributes changed on the parent do not affect the child. You can modify the settings without affecting the parent view attributes.
Section and visibility settings are copied to projected views. All views provide independent control of section and visibility settings. Changes to settings only affect the view where the changes of the contents settings are made.
The section and visibility settings of a view affect the results of a breakout view operation.
Section views based on presentations show trails. You can turn visibility of one or all trails on and off.
If you used inferred or explicit constraints to place the view cutting line, you must edit the sketch to remove the constraints before you can drag the constrained points or line segments.

Define view cutting lines

As you draw a view cutting line, constraints to features and edges are inferred as you move the cursor. If you place a point while an inference line is displayed, the constraint is automatically applied.

After you complete the view cutting line, the available views preview as you move the cursor in the graphics window. After you place the view, it can be moved only within the limits of view cutting line constraints.

TipSelect Section View Preview as Uncut, in the Drawing tab in Application Options, to display the preview of the section view as uncut. This option controls the display of the preview of the model, and when enabled, increases the performance of the previews of section views.

Specify drawing sketch lines for view cutting lines

After you associate a drawing sketch with a view, you can use any line within the sketch that passes through the view geometry to specify the view section.

Align section views

A view defined by a view cutting line is usually aligned to the parent view. It can be moved within the alignment constraint. If you remove the alignment, the view can be moved freely in the drawing, and the view cutting line with its arrowheads and text label are displayed on the parent view.

Hatching in section views

Hatch patterns are automatically applied to section views when you create them. The active Hatch style defines the pattern, scale, shift, and other attributes of the hatch.

When multiple parts are cut in a section view, a specific hatch angle is applied to each section hatch. Default Section Hatch Angles are specified by Preset Values on the General tab of the Standard style pane. The final hatch rotation for cut views includes also the rotation angle defined in the Hatch style. If appropriate, use Style and Standard Editor to edit the default values of the hatch angle.

NoteThe default hatch rotation angles apply on creating section views. If the setting in the Standard changes, existing section views keep the hatch rotation angle as an object override.

To change the default hatch in cut views:

Edit the current Hatch style or select another Hatch style for the Section Hatch object in Object Defaults.
Change the default Section Hatch Angles on the General tab of the Standard style pane. Section Hatch Angles define hatch rotation for particular sectioned parts.
Load hatch patterns from an external PAT file and set them in the Hatch style.
Map materials to hatch patterns on the Material Hatch Pattern Defaults tab of the Standard style pane.

To edit properties of a hatch in a cut view, right-click the hatch and click Edit. Then change the hatch attributes in the Edit Hatch Pattern dialog box. All edits are kept as property overrides.

To change the Hatch style for a section hatch, select another style in the Style list box on the Annotate tab of the ribbon. The selected Hatch style is applied to the hatch object and all overrides are discarded.

By Material hatch pattern

You can map materials to hatch patterns. Open the Style and Standard Editor, click the active Standard style and open the Material Hatch Pattern Defaults tab. Then import materials or create a list of materials manually, and map hatch patterns to materials.

If material of a component is defined in the hatch pattern map, then the By Material hatch pattern is used whenever the component is cut. The By Material option is enabled for the component. Otherwise, the hatch pattern from the Hatch style assigned to the Section Hatch object in Object Defaults is used. The By Material option is disabled for the component.

TipTo enable the By Material hatch pattern for legacy drawings, map materials to hatch patterns in Styles and Standard Editor, and then select the By Material option for all hatch patterns in the drawing from either the Edit Hatch Pattern dialog box or from the Hatch right-click menu.

Cross hatch clipping

Select the Cross Hatch Clipping option on the Drawing tab of the Document Settings dialog box to break hatching around drawing annotations in cut views.

Notes:

To enable clipping around user-defined symbols, select the Symbol Clipping option for individual symbol instances.
The cross hatch clipping is not supported for datum targets and in isometric views.

TipHatching is clipped on the bounding box of note text. If appropriate, change the size of the bounding box to resize the clipped area.

Set styles for section view annotations

The default appearance of the section line, arrows, and label text style is specified in the View Annotation style. To change the default settings, click Manage tab Styles and Standards panel Styles Editor and edit an existing or create a new a view annotation style.

To change the default properties of the section view label, choose Manage tab Styles and Standards panel Styles Editor, select a Standard style and open the View Preferences tab on the Standard style panel.

Change existing section views

After you place a section view, you can change the definition of the view, or even the type of view, by dragging the elements of a view cutting line in the graphics window.

Drag a point to shorten or lengthen a line segment.
Drag a line segment to move it, and shorten or lengthen adjoining line segments.
Drag an arrowhead to change its direction or the length of the landing.
Drag a point to change the angle of a line segment.

As you change the view cutting line, the dependent view updates to reflect the new view definition.

Inheritance of the section and breakout cut

Isometric projected views created for section views inherit the section cut by default. Orthographic projected and auxiliary views support the inheritance of the section, but it is switched off by default.

Isometric projected views created for views with a breakout inherit the breakout cut by default. Orthographic projected and auxiliary views do not support inheritance of breakout operations.

TipTo switch on or off the inheritance of the section or breakout cut, right-click the view, and select Edit View. Open the Display Options tab of the Drawing View dialog box, and select the appropriate options in the Cut Inheritance section.

Create slice operations with section views

You can create a section view with some sliced components and some sectioned components depending on their browser attribute settings.

You can optionally choose to override browser component settings and slice all parts in the view according to the section line geometry. Components that are not crossed by the section line do not participate in the slice operation.

Procedures

Create section views

On the ribbon, click Place Views tab Create panel Section to create a full, half, offset, or aligned section view from a specified parent view. A section view is automatically aligned to its parent view.

In the following image, a section view was used to expose components for ballooning.

You can define the view cutting line while Section View is active or create sketch geometry to use for the view cutting line.

To change the depth of a section view, right-click the section view or cutting line, select Edit Section Properties from the menu, and then change the setting in the dialog box.

When creating section views of presentations with trails, the trail is visible in the drawing view. If appropriate, right-click a view or a single trail and select Show Trails to turn trails on or off.

When you either sketch a multi-segment section line or select a view sketch containing a multi-segment section line, you can specify the method of the section view, projected or aligned.

TipTo place the view without alignment to the parent view, press Ctrl as you move and place the preview.

Create a section view

On the ribbon, click Place Views tab Create panel Section.
Select an existing view to use as the parent view.
Click to set the start point for the view cutting line, and then click to place additional points for the line. The number and location of points on the view cutting line determine the type of section view.
Right-click, and then select Continue to complete the view cutting line.
In the dialog box, edit the view identifier and select the scale. Click Toggle Label Visibility to change the label visibility. Click Edit View Label to edit the view label in the Format Text dialog box.
Set the display style.
Set the section depth for the view.
Select the method of the section view, projected or aligned, if possible.
Move the preview to the appropriate location, and then click to place the view. You can place the view only within the alignment indicated by the view cutting line.
Show Me how to create a section view

Show Me how to override the default section view alignment

Create a section view defined by sketch geometry

Select an existing view to use as the parent view.
On the ribbon, click Place Views tab Sketch panel Create Sketch to open a drawing sketch associated to the view.
Create sketch geometry to define a view cutting line, and then close the sketch.
On the ribbon, click Place Views tabCreate panel Section.
Select the view cutting line you defined in the sketch.
In the dialog box, edit the view identifier and select the scale. Click Toggle Label Visibility to change the label visibility. Click Edit View Label to edit the view label in the Format Text dialog box.
Set the display style.
Set the section depth for the view.
Select the method of the section view, projected or aligned, if possible.
Move the preview to the appropriate location and click to place the view. You can place the view only within the alignment indicated by the view cutting line.

TipYou can use an unconsumed model sketch as a section line.

Create aligned section views

When you either sketch a multi-segment section line or select a view sketch containing a multi-segment section line, you can specify the method of the section view, projected or aligned.

If one or more segment angle is non-perpendicular, the default method is set to Aligned. If all segment angles are exactly 90 degrees, the default method is set to Projected.

Select an existing view to use as the parent view.
On the ribbon, click Place Views tab Sketch panel Create Sketch to open a drawing sketch associated to the view.
Create sketch geometry to define a view cutting line, and then close the sketch.
On the ribbon, click Place Views tabCreate panel Section.
Select the view cutting line you defined in the sketch.
In the dialog box, set the label, scale, display style, and section depth for the view. If you do not change these settings, the default settings are assigned.
In the Method area, set the preferred projected method.
Move the preview to the appropriate location and click to place the view. You can place the view only within the alignment indicated by the view cutting line.

To change the projected method, select the section view, right-click and select

Edit Section Properties.

TipYou can use an unconsumed model sketch as a section line.

Create a slice operation with a section view

On the ribbon, click Place Views tabCreate panel Section.
Select an existing view to use as the parent view.
Click to set the start point for the view cutting line, and then click to place additional points for the line. The number and location of points on the view cutting line determine the type of section view.
Right-click, and then select Continue to complete the view cutting line.
In the dialog box, set the label, scale, display style, and section depth for the view. If you do not change these settings, the default settings are assigned.
- Make sure "Include Slice" is checked. This setting creates a section view, with some components sliced and some components sectioned, depending on the Browser attribute settings.
- Make sure "Include Slice" is checked. This setting creates a section view with some components Sliced.
- Optional: Check "Slice All parts" to override Browser component settings and slice all parts in the view according to the Section line geometry. Components that are not crossed by the Section Line do not participate in the Slice operation.
  Note Since this view is essentially a true zero-depth Section View, the Section Depth fields are grayed-out when this option is checked.
Move the preview to the appropriate location, and then click to place the view. You can place the view only within the alignment indicated by the view cutting line.

Note(Cut Inheritance):

Isometric projected views created for section views inherit the section cut by default.
Orthographic projected and auxiliary views support the inheritance of the section, but it is switched off by default.
To switch on or off the inheritance of the section cut, right-click the child view, and select Edit View. Open the Display Options tab of the Drawing View dialog box, and select the Section option in Cut Inheritance.

Edit section view properties

You can edit the depth of an existing Section View, as well as include or exclude a Slice operation in the view.

Change the depth of a section view

Right-click the section view or cutting line.
Select Edit Section Properties from the context menu.
Change the section depth settings in the dialog box.
- In the Depth Control, select Full to create the section view to all geometry beyond the cutting line.
- Select Distance to specify a distance of viewing in model units beginning from the cutting line, and enter the depth distance in the Distance field.
  Note Set the section depth to zero to revert to the smallest available section depth. This section is not a true zero-depth section. The actual value is 0.000012.

Include a Slice operation in an existing Section View

Make sure "Include Slice" is checked. This setting creates a section view, with some components sliced and some components sectioned, depending on the Browser attribute settings.
Optional: Check "Slice All parts" to override Browser component settings and slice all parts in the view according to the Section line geometry. Components that are not crossed by the Section Line does not participate in the Slice operation.
NoteSince this view is essentially a true zero-depth Section View, the Section Depth fields are grayed-out when this option is checked.

Exclude an existing Slice operation from a Section View

Make sure "Include Slice" is not checked. This setting removes existing Slice operations from the view.

Note(Cut Inheritance):

Isometric projected views created for section views inherit the section cut by default.
Orthographic projected and auxiliary views support the inheritance of the section, but it is switched off by default.
To switch on or off the inheritance of the section cut, right-click the child view, and select Edit View. Open the Display Options tab of the Drawing View dialog box, and select the Section option in Cut Inheritance.

Modify hatch patterns

Hatch patterns are automatically applied to section views when you create them. The active Hatch style defines the pattern, scale, shift, and other attributes of the hatch.

Modify the hatch pattern for an area in a section view

You can modify the hatch pattern for any area after placing a section view.

In the graphics window, select the hatch pattern to change.
Right-click and select Edit from the menu.
Change attributes of the hatch pattern in the Edit Hatch Pattern dialog box:
- Select By Material to use the hatch pattern assigned to the material of the cut part.
- Select a hatch pattern from the Pattern list.
- Set the hatch Angle, Scale, Shift, and Line Weight.
- Select Double to create a crosshatch.
- Click Color and select a new color in the Color dialog box.
To use a hatch pattern that is not available in the Pattern list, select Other in Pattern. Then add the hatch pattern using the Select Hatch Pattern dialog box.
Click OK to close the Edit Hatch Pattern dialog box.

TipTo change the Hatch style for a section hatch, select another style in the Style list box on the Annotate tab of the ribbon. The selected Hatch style is applied to the hatch object and all overrides are discarded.

Use the By Material hatch pattern in section views

In the graphics window, select the hatch pattern to change.
Right-click and select Pattern from the menu.
If the material of the corresponding component is defined in the hatch pattern map, the By Material option is available. Select the By Material option to apply the hatch pattern defined for the materials of the component, or cancel selection of the By Material option to use the default hatch pattern defined in the hatch style.

Change the default hatch in cut views

Use the Style and Standard Editor to:

Edit the current Hatch style or select another Hatch style for the Section Hatch object in Object Defaults.
Change the default Section Hatch Angles on the General tab of the Standard style pane. Section Hatch Angles define hatch rotation for particular sectioned parts.
Load hatch patterns from an external PAT file and set them in the Hatch style.
Map materials to hatch patterns on the Material Hatch Pattern Defaults tab of the Standard style pane.

Hide or display hatching for parts in section views

You can hide the hatch pattern for a part in a view.

In the graphics window, select the part in the view.
Right-click the hatched area, and then select Hide to suppress the hatch display or clear the check mark from Hide to show the hatching.

Hide or display hatching for section views

You can hide or display all hatching in a section view.

In the graphics window or in the browser, select the section view.
Right-click and select Edit View. The Drawing View dialog box is displayed.
Open the Display Options tab, and clear or select the Hatching option.
Click OK to close the Drawing View dialog box.

Create a breakout

You can remove a defined area of material to expose obscured parts or features in an existing drawing view.

To create a breakout, place the view, and then create an associated sketch with one or more closed profiles to define the boundary of the breakout area.

NoteThe active Standard and the Hatch style assigned to the Section Hatch object in Objects Default determines the default hatching in breakout views. You can change the setting using Style and Standard Editor.

TipTo associate a sketch with a drawing view, select the view, and then click Place Views tab

Sketch panel

Create Sketch and create the sketch.

There are four ways to define the depth of the breakout area:

From a point in the model

You can specify a starting point for the breakout area and measure the depth of the area from that point.

On the ribbon, click Place Views tabModify panel Break Out.
In the graphics window, click to select the view, and then click to select the defined boundary.
NoteThe boundary profile must be on a sketch associated to the selected view.
In the Break Out dialog box, click the arrow next to the Depth type box and select From Point.
Click the select arrow, and then in the graphic window click the start point for the depth. You can specify the point in any view of the model.
In the Depth value box, enter the depth of the breakout.
When the view is fully defined, click OK to create the view.

Show Me how to create a break out using From Point method

In a sketch associated to a projected view

You can specify the depth for the breakout using geometry on a sketch associated to a dependant projected view.

Project a view from the base view.
Create a sketch associated to the projected view and add geometry to define the depth for the breakout.
On the ribbon, click Place Views tabModify panel Break Out.
In the graphics window, click to select the view, and then click to select the defined boundary.
NoteThe boundary profile must be on a sketch associated to the selected view.
In the Break Out dialog box, click the drop-down arrow next to the Depth type box and select To Sketch.
Click the select arrow, and then in the graphic window click to select the sketch geometry associated with the projected view.
When the view is fully defined, click OK to create the view.

Show Me how to create a break out using To Sketch method

Use a hole feature in the view

You can specify the depth for the breakout using a hole feature in the selected view.

On the ribbon, click Place Views tabModify panel Break Out.
In the graphics window, click to select the view, and then click to select the defined boundary. The boundary profile must be on a sketch associated to the selected view.
In the Break Out dialog box, click the arrow next to the Depth type box and select To Hole.
Click the select arrow, and then in the graphic window click to select the hole feature. The depth is defined by the axis of the hole.
NoteIf the hole feature is hidden, click Show Hidden Edges to show it temporarily.
When the view is fully defined, click OK to create the view.

Show Me how to create a break out using To Hole method

By the depth of a part

You can specify one or more parts to break out of the selected view to expose the obscured parts or features.

On the ribbon, click Place Views tabModify panel Break Out.
In the graphics window, click to select the view, and then click to select the defined boundary.
NoteThe boundary profile must be on a sketch associated to the selected view.
In the Break Out dialog box, click the arrow next to the Depth type box and select Through Part.
In the graphic window click to select part. The depth is defined by the depth of the part.
When the view is fully defined, click OK to create the view.

Show Me how to create a breakout using Through Part method

TipTo change the boundary area definition, open the sketch and make the changes. To edit the depth definition, right-click the view in the browser and select Edit Definition.

Note(Cut Inheritance):

Child isometric projected views, created for views with a breakout, inherit the breakout cut by default. To switch off or on the inheritance of the breakout cut, right-click the child view, and select Edit View. Open the Display Options tab of the Drawing View dialog box, and select the Break Out option in the Cut Inheritance section.
Orthographic projected and auxiliary views do not support inheritance of breakout operations.

References

Section View

Creates a full, half, offset, or aligned section view from a specified parent view. You can also use Section view to create a view cutting line for an auxiliary or partial view. A section view is aligned to its parent view.

In the following image, a section view was used to expose components for ballooning.

NoteIf you create a sketch in the drawing, it is not possible to make additional views from this sketch.

Access:

Ribbon: Place Views tab

Create panel

Section

NoteThe default setting for sectioning of standard parts is set in the Application Options dialog box. You can override the setting on the Options tab of the Drawing view dialog box.

View/Scale Label

Specifies the view label and scale.
View Identifier	Edits the view identifier string.
Scale	Sets the scale of the view, relative to the part or assembly. Enter the scale in the box, or click the arrow to select from a list of commonly used scales. You can enter a scale that is not on the list. The new scale appears above a line in the list and is available until you close Autodesk Inventor. It is not added to the scale list from the Standard style.
	Displays or hides the view label.
	Edits the view label text in the Format Text dialog box.

Style

Sets the display style for the view. The default display style for a section view is Hidden Line Removed. To change the display style, click a command.
	Sets the display to show hidden lines.
	Sets the display to remove hidden lines.
	Sets the display to a shaded rendering.

Section Depth

Depth Control	Controls the section depth. Select Full to create the section view to all geometry beyond the cutting line. Select Distance to specify a distance of viewing in model units beginning from the cutting line.
Distance	Sets the distance of the section. NoteSet the section depth to zero to revert to the smallest available section depth. This is not a true zero-depth section. The actual value is 0.000012.

Slice

Include Slice	When checked, the Section View is created with some components sliced and some components sectioned, depending on their Browser attributes.
Slice All parts	When checked, the Browser attributes are overridden and all components in the view is sliced according to the Section Line geometry. Components that are not crossed by the Section Line does not participate in the resulting view. The Section Depth fields are disabled when this option is checked. NoteThis option is only available when Include Slice option is checked.

Method

Specifies the method of projecting the section view when you either sketch a multi-segment section line or select a view sketch containing a multi-segment section line.

Projected

Created projected view from the sketch line.

NoteThis option is set as default if all segments are exactly 90 degrees.

Aligned

When checked, resulting section view is perpendicular to the line of projection. Body cut lines do not display in the resulting view.

Aligned option is not available for a child (dependent) view.

NoteThis option is only available when Include Slice option is checked.

Edit Hatch Pattern

Modifies the hatch pattern for an area. When you create a section view, hatching is automatically applied using the defaults specified by the active drafting standard.

Access:

Ribbon: Place Views tab

Create panel

Section

Right-click the hatch pattern area in a cut view, and then select Edit.

By Material	If selected, the hatch pattern corresponds to the mapping between materials and hatch patterns defined in the Standard style. TipTo change the mapping, open the Style and Standard Editor. Then change the settings on the Material Hatch Pattern Defaults tab of the Standard style pane.
Pattern	Selects the hatch pattern. Click the arrow and choose a hatch pattern from the list. Select Other to add a hatch pattern to the Pattern list. Then add the hatch pattern using the Select Hatch Pattern dialog box.
Angle	Rotates the hatch pattern by the specified angle. Enter the desired angle.
Line Weight	Sets the thickness of the hatch lines. Click the arrow, and then choose the thickness from the list.
Scale	Sets the distance between lines in the hatch. A scale of 1 uses the original distance specified in the hatch pattern. A scale of 0.5 results in line spacing that is one half of the original distance.
Shift	Shifts the hatch pattern to offset it slightly from the original hatch pattern position. Enter the distance for the shift.
Color	Changes the color of the hatch lines. Click Color, and then select the color.
Double	Creates a copy of the specified hatch pattern perpendicular to the first hatch pattern.

Edit Section Properties

Edit the depth of an existing Section View. Include or exclude a Slice operation in an existing Section View.

Access:

In a drawing file, click a Section View to select, then right-click to display the context menu.

Section Depth

Depth Control	Controls the section depth. Select Full to create the section view to all geometry beyond the cutting line. Select Distance to specify a distance of viewing in model units beginning from the cutting line.
Distance	Sets the distance of the section. NoteSet the section depth to zero to revert to the smallest available section depth. This is not a true zero-depth section. The actual value is 0.000012.

Slice

Include Slice	When checked, the Section View is created with some components sliced and some components sectioned, depending on their Browser attributes.
Slice All parts	When checked, the Browser attributes are overridden and all components in the view is sliced according to the Section Line geometry. Components that are not crossed by the Section Line does not participate in the resulting view. The Section Depth fields are disabled when this option is checked. NoteThis option is only available when Include Slice option is checked.

Method

Specifies the method of projecting the section view when you either sketch a multi-segment section line or select a view sketch containing a multi-segment section line.

Projected

Created projected view from the sketch line.

NoteThis option is set as the default if all segments are exactly 90 degrees.

Aligned

When checked, resulting section view is perpendicular to the line of projection. Body cut lines do not display in the resulting view.

Aligned option is not available for a child (dependent) view.

NoteThis option is only available when Include Slice option is checked.

Break Out

Removes a defined area of material to expose obscured parts or features in an existing drawing view. The parent view must be associated to a sketch that contains the profile defining the breakout boundary

Access:

Ribbon: Place Views tab

Modify panel

Break Out, and then click to select the parent view.

Boundary Profile	Selects the sketch geometry to define the breakout boundary. When the Profile command is selected, click the sketch profile to select it.
Depth Selector	Selects the geometry to define the depth of the breakout area. Click to select the arrow, and then click the geometry in the drawing view.
Depth Type	Selects the method for defining the depth of the breakout. Click the arrow next to the box and select the Depth Type from the list. From Point sets a numeric value for the depth of the breakout. To Sketch uses sketched geometry associated with another view to define the depth of the breakout. To Hole uses the axis of a hole feature in the view to define the depth of the breakout. Through Part uses the thickness of a part to define the depth of the breakout.
Depth	Specifies a numeric value for the depth of the breakout. Available only when the Depth Type is From Point.
Display	Select Show Hidden Edges to display the hidden edges in the view temporarily. You can pick a point on the hidden line geometry to define the depth of the breakout. Clear the check box to omit hidden lines in the view. Select Section All Parts to section parts that are not currently sectioned in the breakout area. Clear the check box to omit non-sectioned parts from the view.

Inventor

Community Scoring

Tag Tags0

Page statistics

Section views

Table of contents

Show Me how to override the default section view alignment

Comments0