Cosmetic Threads PropertyManager

You can specify the following properties when inserting a cosmetic thread in a part, assembly, or drawing.

For shaded display of cosmetic threads, click Options . On the Document Properties tab, select Detailing. Under Display filter, select Shaded cosmetic threads.

To open the Cosmetic Threads PropertyManager:

  1. On a cylindrical feature (a boss, a cut, or a hole), select the circular edge where the thread begins.
  2. Click Cosmetic Thread (Annotation toolbar), or click Insert > Annotations > Cosmetic Thread.

Thread Settings

Circular Edges Select a circular edge in the graphics area.
  Standard Lets you set the dimensioning standard for the cosmetic thread.
  Type Lets you select the type of threads.
  Size Lets you select the size of the cosmetic thread based on the dimensioning standard you selected. Valid values for the selected edge are listed.
Minor Diameter, Major Diameter, or Conical Offset Sets the diameter for the dimension corresponding to the entity type with the cosmetic thread. You can use an equation by entering = (equal sign) and select global variables, functions, and file properties from a list.
  End Condition The cosmetic thread extends from the edge selected above to the end condition:

Blind

A specified depth that starts from the selected edge. To start the depth from a face or plane, click Start from a face/plane , select a face or plane, and specify the thread depth.

Through

Completely through the existing geometry.

Up to Next

To the next entity that intercepts the thread.

Depth Enter a value when the End Condition is Blind.
 
This functionality applies to new parts created in SOLIDWORKS 2022 and later.

For part templates (*.PRTDOT) created in SOLIDWORKS 2022 and later, you can retain the legacy functionality for Depth and feature ownership. In part templates, before you add cosmetic threads, click Tools > Options > Document Properties > Drafting Standard > Annotations and clear Apply new cosmetic thread behavior to new parts. This option is selected by default for new part templates and cleared for legacy part templates. This option is enabled for new part templates only; it is disabled for part documents.

If you use the Insert > Mirror Part command, the mirrored part inherits the cosmetic thread behavior from the base part. For example, if the base part is created in SOLIDWORKS 2021, the mirrored part inherits the legacy behavior for cosmetic threads from the base part.

 SOLIDWORKS measures Depth from the original location of an edge regardless of changes made by downstream features that relocate that edge. In the image below, the original thread depth is 80 mm from the edge of the cut extrude. If you add a second cut extrude that relocates that edge, the cosmetic thread retains the original thread depth of 80 mm.
Cosmetic thread original depth Before SOLIDWORKS 2022 SOLIDWORKS 2022 and later

Thread Callout

Type text to appear in the thread callout. If you selected a Standard, the thread callout is driven by the standard and cannot be edited.

Thread callouts are not used in certain dimensioning standards. If you define a cosmetic thread callout in the part or assembly but it is not displayed in the part, assembly, or drawing, you can display the callout by selecting Insert Callout from the shortcut menu.
Configurations Specifies the configurations to which the callout applies.
Cosmetic thread callouts are configurable only when Standard is set to None in the Cosmetic Thread PropertyManager.
Show type (Not available if you select None for Standard.) Includes the thread Type (such as Machine Threads or Straight Pipe Thread, selected above) in the callout.



Show type selected



Show type cleared

Layer

In drawings with named layers, select a layer.