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Drawings · Lesson 8

Annotations in SOLIDWORKS drawings

Annotations are everything on a drawing that is not a view or a dimension: centre marks and centrelines on holes, notes, surface finish and weld symbols, datum targets, revision tables and thread representations. Notes can link to custom properties, so a material or part number shows up automatically and updates with the model.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Drawing view with center marks, centrelines, a linked note, a surface finish symbol and a weld symbol

Where to find it

Annotation tab → Note, Center Mark, Centerline, Surface Finish, Weld Symbol, Tables

Common annotations

Annotation Use
Center Mark Single, linear or circular marks on holes and arcs
Centerline Axes of holes and cylinders in side views
Note Text, optionally linked to properties ($PRP, $PRPSHEET …)
Surface Finish Roughness symbols; ISO 21920 support added in 2025–2026
Weld Symbol Weld type, size and length; also from weld beads via Model Items
Datum Feature / Datum Target Datum references for GD&T — see GD&T
Revision Table Revision history, linked to the Revision property
Cosmetic threads Thread display; ISO shows a solid line, ANSI a dashed line

Since 2026, magnetic lines also align notes, weld, GD&T, surface finish and revision symbols.

Step by step

  1. 1

    Add centre marks and centrelines

    Annotation → Center Mark, click the hole edge in the front view. Then Centerline and Ctrl-select the two hidden lines of the hole in a side view.

    Center mark on a hole in the front view and a centerline between hidden lines in the side view
    Center marks on circles, centrelines between hidden lines of holes.
  2. 2

    Add a linked note

    Note, click Link to Property, choose Model found here, pick the Material property, and place the note near the view. It reads the material from the part.

  3. 3

    Make it automatic next time

    In Document Properties → Detailing, under Auto insert on view creation, tick center marks for holes, then re-save your drawing template.

Common mistakes

  • Typing values into notes that should be linked — they go out of date when the model changes.
  • Centerlines showing solid after an update — in SOLIDWORKS 2025 SP3 centrelines follow the layer line style; set them back to Per Standard.
  • Cosmetic threads missing in assembly drawings — insert them with Model Items, and turn on Cosmetic threads in Detailing.

Lesson 8 of 14 in the drawings course.

Practice

Add a centre mark to the hole and a note linked to the part's Material property. Check: change the part's material from 6061 aluminium to another material — after a rebuild the note shows the new material without editing it.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

How do I add a center mark in SOLIDWORKS?

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Annotation → Center Mark, then click a circular edge. Single, linear and circular center marks are available, and they can be inserted automatically when views are created.

How do I link a note to a custom property?

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Create a note, click Link to Property, pick the source (this drawing, the model in a view, or the model found here) and the property.

What do $PRP and $PRPSHEET mean in notes?

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$PRP reads the drawing's own properties; $PRPSHEET reads the model shown in the view chosen in Sheet Properties.

How do I add a revision table?

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Annotation → Tables → Revision Table. The first revision creates a Revision custom property; numbering can be letters or numbers.