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SOLIDWORKS Cosmetic Thread Display in Parts, Assemblies and Drawings

Article by Scott Durksen, CSWE created/updated July 20, 2016

There are many options and settings to adjust the display of a SOLIDWORKS Cosmetic Thread in the various environments.  Here is a breakdown of the options available that may be useful if you find that your Cosmetic Thread is missing.

Part Environment:

When you add a tapped Hole Wizard feature in a part, you should see the cosmetic thread dashed line around the hole as shown in the figure below:

SOLIDWORKS Cosmetic Thread visible

SOLIDWORKS Cosmetic Thread visible

First, verify that Hole Wizard feature is actually a tapped hole and that you’ve enabled the option to include the Cosmetic Thread.

Hole Wizard - Cosmetic Thread

Hole Wizard – Cosmetic Thread

Then right-click on the Annotations folder in the Design Tree and choose Details.

Annotations Details

Annotations Details

Ensure that BOTH ‘Cosmetic threads’ and ‘Display annotations’ are selected. Optionally you can also select ‘Shaded cosmetic threads’ if you want a graphical representation of the threads on the hole face.

Annotation Properties

Annotation Properties dialog

Under the View menu, choose Hide/Show and verify that ‘Hide All Types’ is deselected and ‘All Annotations’ is selected.

Hide / Show Annotations

Hide / Show Annotations

If your Cosmetic Thread display is shown as a solid line, this indicates your Document Properties are set to the ISO standard.

ISO Document properties

ISO Document properties

Changing to ANSI standard will display a dashed cosmetic thread.

ISO solid cosmetic thread

ISO solid cosmetic thread

Assembly Environment:

Within the assembly environment, you can show all of the SOLIDWORKS Cosmetic Thread annotations that are contained in each part file.  First ensure that the Cosmetic Threads are visible in the Part environment as per the section above.  Then within the Assembly environment, go to View > Hide/Show and ensure that ‘Hide All Types’ is deselected and ‘Component Annotations’ is selected.

Assembly - View Hide / Show

Assembly – View Hide / Show

If you’ve added Assembly Level features to the assembly (i.e. Hole Wizard features directly in the assembly), ensure you’ve also selected ‘Top Level Annotations’ in the View > Hide/Show menu.

Top Level Annotations display option

Top Level Annotations display option

And you’ll need to ensure that the same options are selected in Annotations > Details within the assembly.

Assembly - Details

Assembly – Details

These options only apply to assembly-level features with Cosmetic Threads

Annotation Properties

Annotation Properties

And again if you see a solid line for the Cosmetic Thread, this indicates the Assembly is set to the ISO standard.  This will force all cosmetic threads in the assembly to show as solid lines, even if the parts were set to ANSI standard.

ISO - Document properties

ISO – Document properties

Drawing Environment:

In terms of Cosmetic Threads being shown in drawings, by default drawing views of Part files containing cosmetic threads will automatically be inserted with the callout (if the hole callout option was selected in the Hole Wizard feature).

Drawing view - cosmetic thread with callout

Drawing view – cosmetic thread with callout

For assembly drawing views, the cosmetic threads will not be shown by default (both component-level and assembly-level features).  However you can import them into specific drawing views using Model Items from the Annotations tab.

Model Items

Model Items

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Scott Durksen, CSWE

Scott is a SOLIDWORKS Elite Applications Engineer and is based in our Dartmouth, Nova Scotia office.

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