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SOLID WORKS ClubSOLID WORKS Club

Drawings · Lesson 7

Dimensions in SOLIDWORKS drawings

Drawing dimensions come from two places. Model Items imports the dimensions you used to build the model — they are driving, so editing them changes the part. Dimensions you add in the drawing with Smart Dimension are reference (driven) dimensions and show in grey by default. Chain and ordinate dimensions, hole callouts and the dimension palette help you lay them out cleanly.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Dimensioned drawing views of a plate with black model dimensions and grey reference dimensions

Where to find it

Annotation tab → Model Items, Smart Dimension (flyout: chain, ordinate), Hole Callout

Dimension tools in drawings

Tool Use
Model Items Import model dimensions, hole callouts, annotations
Smart Dimension Reference dimensions; Shift-click circles for edge dimensions
Chain Dimension (2020+) Dimensions end to end
Ordinate Dimension Zero point plus distances — good for hole series
Hole Callout Full hole specification from a hole edge
Dimension palette / Auto Arrange (2011+) Spacing and alignment of selected dimensions

Precision and tolerances are set per dimension or in Document Properties — see tolerances. Fully defined sketches give the cleanest Model Items — see fully defined sketches.

Dimensions turned dangling? See drawing errors — Reattach and views that don't update.

Step by step

  1. 1

    Import the model dimensions

    On the plate drawing, Annotation → Model Items. Source: Entire model, tick Import items into all views, and Marked for drawing. Click the tick.

    Model Items PropertyManager with Entire model source and Marked for drawing selected
    Model Items brings in the dimensions used to build the part.
  2. 2

    Move dimensions to the right views

    Drag dimensions to tidy them. Shift + drag moves a dimension to another view; Ctrl + drag copies it.

  3. 3

    Add what is missing

    The hole position came from relations, not dimensions, so add it with Smart Dimension — from an edge to the hole centre. It appears grey: a reference dimension.

  4. 4

    Arrange

    Select several dimensions; the dimension palette appears. Use its auto-arrange to space them evenly.

Common mistakes

  • Expecting dimensions that were never in the model — fully defined sketches give complete Model Items; relations give no dimensions.
  • Changing an imported dimension by accident — it changes the part.
  • {'Over-dimensioning': 'the same size in two views. Show each size once, in the view that shows it best.'}

Lesson 7 of 14 in the drawings course.

Practice

Import Model Items into the mounting plate drawing. Check: you get five dimensions — 100, 60, 20, Ø20 and R5 — and the hole position, held by relations in the sketch, has to be added as a reference dimension.

Sources

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

Frequently asked questions

How do I import dimensions into a SOLIDWORKS drawing?

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Annotation → Model Items. Choose the source (entire model or selected feature), the dimension types and whether to import into all views.

Why are some drawing dimensions grey?

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Grey dimensions were added in the drawing and are driven (reference). Black ones were imported from the model and drive it. The colours can be changed in System Options → Colors.

What are chain dimensions?

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A string of dimensions placed end to end with one command, added in SOLIDWORKS 2020 in the Smart Dimension flyout.

How do I add a hole callout?

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Annotation → Hole Callout, then click a hole edge. Hole Wizard holes show their full specification, such as countersink and thread.