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Document Properties - Detailing

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

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.  
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.  
Always display text at the same size Select to display all annotations and dimensions at the same size, regardless of zoom.
This option is disabled for drawings, which always zoom the text height.
 
Display items only in the view orientation in which they are created (Parts and assemblies only) Select to display annotations only when the model has the same orientation as when the annotation was added. Rotating the part 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.
 
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
  • Center marks - fillets
  • Center marks - slots
  • Centerlines to add centerlines to model faces with parallel edges.
    Centerlines are not inserted automatically if the model is in Large Assembly Mode, 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.

Selected

Cleared

View break lines Enter:
  • Gap to set the distance between break lines in a broken view
  • Extension to set length of the break lines beyond the model geometry in a broken view


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