Document Properties - Detailing

You can specify document-level drafting settings for detailing options. Available for all document types.

To open this page:

With a drawing open, click Options (Standard toolbar), select the Document Properties tab, and then select Detailing.

Options

Display filter

Select annotation types to display by default or select Display all types.

Point, Axis, and Coordinate System

Set font and display options for reference geometry names and labels for points, axes, and coordinate systems.

This option is not available for drawings.

Hide names	Hides reference geometry names for points, axes, and coordinate systems.
Name font	Sets the font for the names of points, axes, and coordinate systems.
Label font	Sets the font for the labels of coordinate system arrows.

Always display text at the same size

Select to display all annotations and dimensions at the same size, regardless of zoom.This also applies to 3D Views in MBD.

This option is disabled for drawings, which always zoom the text height.

Text scale

For part and assembly documents, clear Always display text at the same size to select a scale for the default size of annotation text. To set a custom text scale, select Custom, then enter the first and second value of the custom scale. For example, enter 3 and 10 to set the scale to 3:10.

If you specify Text scale in a 3D View, the text size applies to the 3D View in published 3D PDF files.

Display items only in the view orientation in which they are created

For parts and assemblies, select to display annotations only when the model has the same orientation as when the annotation was added. Rotating the model or selecting a different view orientation removes the annotation from the display.

Display annotations / Display assembly annotations

Select to display all annotation types that are selected in the Display filter. For assemblies, this option applies to the annotations that belong to the assembly and to the annotations that are displayed in the individual part documents.

Use assembly setting for all components

Select to match the display settings for all annotations to the settings for the assembly document, regardless of the settings for individual part documents. Select Display assembly annotations in addition to this option to display different combinations of annotations.

Hide dangling dimensions and annotations

For parts or assemblies, select to hide:

Dangling dimensions and annotations in referenced drawings that result from deleted features
Dangling reference dimensions that result from suppressed features

For drawings, select to hide dangling annotations.

Highlight associated elements on reference dimension selection

For parts or assemblies, select to highlight elements associated with selected reference dimensions.

Ctrl + select multiple dimensions to highlight referenced elements of all selected dimensions.

Specify the color used to highlight the referenced elements. To specify the highlight color, from the Tools menu, click:

Options > System Options > Colors. Under Color scheme settings, edit the color for Selected Item 1.

The feature does not support the following dimensions:

DimXpert or sketch dimensions, such as angular running dimensions and ordinate dimensions.
Cosmetic threads
Feature dimensions
Blocked highlights for silhouette edge endpoints.
Referenced edges or points blocked for break view and Detailing mode legacy dimensions.

Show DimXpert when viewing component annotations

For assemblies, select to view component-level DimXpert annotations.

It may be required to set other display controls to view DimXpert annotations.

Use model color for HLR/HLV in drawings

Select to view the model colors of a part or assembly in a drawing in HLR/HLV. This setting overrides colors in Tools > Options > System Options > Colors. However, any assigned layer overrides this setting.

Link child view to parent view configuration

Select to link child views, for example, a projected view, to the parent view configuration. If linked, changing the parent view configuration changes the child view.

Hatch density limit

For drawings, controls the maximum number of hatch lines created within a hatch pattern.

Import annotations

Clear From entire assembly to import only top-level assembly annotations.

Select to import annotations for all components, which might impact performance.

Auto insert on view creation

Select:

Center marks - holes -part
Center marks - fillets -part
Center marks - slots -part
Dowel symbols -part
Center marks - holes -assembly
Center marks - fillets -assembly
Center marks - slots -assembly
Dowel symbols -assembly
Connection lines to hole patterns with center marks
Centerlines to add centerlines to model faces with parallel edges.
Centerlines are not inserted automatically if Large Assembly Settings is enabled, or if the number of components exceeds the threshold for large assemblies, even if this option is selected.
Balloons to add balloons to all visible components, without duplicates in multiple views
Dimensions marked for drawing to add dimensions to models, without duplicates in multiple views
The dimensions are indicated in the part sketches as Mark for drawing.

Cosmetic thread display

Select High Quality to determine if cosmetic threads should be visible or hidden. For example, if a hole (not a through hole) is on the back of a model, and the model is in a front view, the cosmetic thread is hidden. You can set the display for each drawing view individually in the Drawing View PropertyManager under Cosmetic Thread Display.

Area hatch display

Select Show halo around annotations to display space around dimensions and annotations that belong to the drawing view or a sketch and are on top of an area hatch.