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Drawings · Lesson 9

Tolerances and precision in SOLIDWORKS drawings

A tolerance tells the manufacturer how far a size may vary. In SOLIDWORKS you set it on the dimension itself, in the Tolerance/Precision section of its PropertyManager: the tolerance type (for example bilateral), the upper and lower values, and the number of decimals for the value and for the tolerance. Defaults live in Document Properties, and dimension styles let you reuse settings.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Dimension with a stacked bilateral tolerance on a hole in a drawing view

Where to find it

Select a dimension → PropertyManager → Tolerance/Precision

Where tolerance and precision are set

Level Where
One dimension PropertyManager → Tolerance/Precision, or the dimension palette
Document default Document Properties → Dimensions → Primary precision
Reusable Dimension styles (.sldstl): add, save and load
Template Defaults saved in the drawing template
Holes Hole Wizard Type tab → Tolerance/Precision (2019+)

The precision dialog sets decimals separately for primary, dual and angular values, for the value and for the tolerance. Leading and trailing zero display is set in Document Properties. Form and position tolerances use GD&T. Tolerances on 3D annotations can drive machining strategies in SOLIDWORKS CAM.

Step by step

  1. 1

    Select the hole dimension

    On the plate drawing, click the Ø20 dimension.

  2. 2

    Choose a tolerance type

    In Tolerance/Precision pick Bilateral from the tolerance type list, enter +0.10 as the upper and 0.00 as the lower value.

    Tolerance/Precision section with Bilateral selected, upper +0.10 and lower 0.00
    Choose the tolerance type, enter the limits, set the decimals.
  3. 3

    Set precision

    Set the value precision to .12 (two decimals) and the tolerance precision to Same as nominal. The dimension now reads Ø20.00 with +0.10 / 0.

  4. 4

    Save it as a style

    With the dimension selected, use Add or Update a Style in the PropertyManager to save these settings for reuse.

Common mistakes

  • Overriding precision on single dimensions, then changing Document Properties and wondering why some do not follow. Set overridden dimensions back to *Document* precision.
  • Tolerances so tight they cannot be made — ask your machinist what the process holds.
  • Forgetting a general tolerance note for dimensions without their own tolerance.

Lesson 9 of 14 in the drawings course.

Practice

Give the Ø20 hole a bilateral tolerance of +0.10 / 0 with two decimals. Check: the dimension shows Ø20.00 with +0.10 and 0 stacked beside it, and Model Items in a new drawing view imports the tolerance because it is stored in the model.

Sources

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

Frequently asked questions

How do I add a tolerance to a dimension in SOLIDWORKS?

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Select the dimension and open Tolerance/Precision in the PropertyManager. Choose the tolerance type, enter the values and set the precision.

How do I change the number of decimals?

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Set the precision in the dimension's PropertyManager, or change the default under Document Properties → Dimensions → Primary precision.

Can Hole Wizard holes carry tolerances?

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Yes. Since SOLIDWORKS 2019 the Hole Wizard Type tab has Tolerance/ Precision settings, and the values appear in the hole callout.

Where do tolerances on drawings come from?

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Tolerances added to model dimensions travel to the drawing with Model Items; tolerances added in the drawing stay in the drawing.