Detailing Mode

You can use Detailing mode to open large drawings quickly. The model data is not loaded, but you can add and edit annotations within the drawing.

Detailing mode is useful if you need to make minor edits to drawings of large assemblies or drawings with many sheets, configurations, or resource-intensive views.

Detailing mode is available for all drawings. You can use limited Detailing mode if you saved drawings in previous versions of SOLIDWORKS or in SOLIDWORKS 2022 without model data. If you open a drawing in limited Detailing mode, the window title displays file name - sheet name [Detailing - Limited]. (Limited Detailing mode is an automatic mode - you cannot specifically select it.)

Creating Dimensions and Annotations

In Detailing mode, you create dimensions and annotations just as you would in Resolved mode.

Exception: You cannot create dimensions or annotations that require model information, such as hole callouts, cosmetic threads, or links to model properties.

If a drawing is open in Detailing mode and you change and save an associated part or assembly, then an out-of-date message appears.

The Resolve Drawing tool always appears in the CommandManager so you can resolve the drawing at any time.


You can save your changes to the existing drawing file without exiting Detailing mode. Saving in Detailing mode does not require a special save format.

  • If you save the drawing in Detailing mode, and then close it and reopen it, you can continue to edit the items you created in Detailing mode.
  • If you save the drawing in Resolved mode, the dimensions and annotations you created in Detailing mode are resolved and saved. Then if you close the drawing and reopen it in Detailing mode, the ability to edit the resolved dimensions and annotations is limited. You can only change their position or delete them.

Capabilities Available in Detailing Mode

You can create the following dimensions and annotations:

  • Notes, including notes with leaders
  • Linear and circular note patterns
  • Surface finish symbols
  • Revision symbols
  • Revision clouds
  • Locations labels
  • Balloons
  • Magnetic lines
  • Weld callouts
  • Geometric tolerances
  • Datum feature symbols
  • Datum target symbols
  • Radial and linear dimensions, including use of the Smart Dimension tool
  • Ordinate dimensions
  • Angular running dimensions

In addition, you can do the following:

  • Drag standard views (such as front, top, back) from the View Palette to the drawing.
  • Change the position, rotation, and labels of drawing views.
  • Copy or cut drawing views and paste them onto the same or other sheets within the same drawing.
  • Within annotations, add links to the displayed values of dimensions and other linkable annotations.
  • Insert sketch blocks.
  • Add general, revision, and hole tables. You cannot add other table types.
  • Select displayed geometry, such as model edges and sketches. Use Select Other to find other selectable items. You cannot select model faces in any drawing views.
  • Save the file as a PDF/DXF file, or print as a PDF.


You can specify Document Properties - Performance options to affect Detailing mode.


  • You cannot create new drawing views.
  • You cannot create centerlines, center marks, or hatching.
  • You cannot use the Undo tool.
  • Draft quality section views cannot be selected or exported to DXF/DWG.