Dimensions and Tolerances

Overview#

Dimensions state the size and location of features. In Fusion drawings they are measured from the model geometry shown in the view; they are driven by the model, not the other way around. Tolerances tell the manufacturer how much variation is acceptable.

Good dimensioning is about completeness without redundancy: every feature is fully defined once, in the view that shows it most clearly, with dimensions placed outside the views where possible.

Where to find it#

Drawing workspace toolbar, Dimensions panel. Autodesk lists these tools:

• Dimension: creates a linear, aligned, angular, radius or diameter dimension depending on what you select.
• Auto Dimension and Tidy Up: automatic dimensioning (Baseline, Chain, Ordinate, Overall, Symmetric, Symmetric with baseline strategies, with a Density slider) and automatic rearranging.
• Individual tools: Ordinate, Linear, Aligned, Angular, Radius, Diameter, Jogged Radial, Arc Length, Curve Min Max, Baseline, Chain.
• Editing tools: Arrange Dimensions (stack or align), Match Dimension (copy format), Flip Arrows, Dimension Break.
• Hole and thread callouts are made with Hole and Thread Note in the Text panel (see annotations page).

Autodesk gives no keyboard shortcut for the Dimension tool. You can dimension only orthogonal views, not isometric ones.

Step by step: basic dimensions#

1. Choose Dimensions > Dimension.
2. Select edges, points or an existing dimension. Fusion creates the relevant type (linear, aligned, angular, radius or diameter) from the selection.
3. Move the cursor to position the dimension and click.
4. Double-click the dimension to open the Dimension dialog for representation, units, precision, tolerance and inspection settings.

Selecting a diameter edge in a side view of a cylinder or hole adds the diameter symbol automatically. If you need a specific type, use the dedicated Radius or Diameter tool. Use object snaps so dimensions attach to precise locations.

Step by step: dimension sets#

• Baseline: select an existing linear dimension, then select points; each new dimension measures from the same base point.
• Chain: select an existing linear dimension, then select points; each new dimension starts at the end of the previous one. Chains accumulate tolerance, so use them only when sequential accuracy is what matters.
• Ordinate: define the origin (0,0) in the view, then place dimensions in X or Y from it. ASME puts the value beside the dimension line, ISO on top of it. Deleting the origin deletes its ordinate dimensions; Autodesk suggests baseline or chain when you need very many.

Dimension types#

Tolerances#

Double-click a dimension to open the Dimension dialog. Its Tolerance section (enabled by a check box) offers four types:

Yes, Fusion has an ISO fit selector. For a Fit you choose whether the base system is Hole or Shaft, the fit type, and a preferred fit class (or Custom, adjusting the limit sizes). Show Fit controls display (Tolerance class, Fit stack no line, Fit stack line, Fit stack diagonal) and Show Tolerance the form (Tolerance class only, with deviations, or with limits).

The Representation icons in the Text section add parentheses (Reference Dimension), an underline (Not To Scale) or a box (Theoretically Exact, the basic dimension used with GD&T). Insert Symbol adds symbols to the dimension text. The Inspection section adds a Round or Angular frame with a Label and Rate.

Precision is set under Primary Units (units cm, mm, m, in or ft; Decimal, Fractional, Engineering or Architectural format for inches and feet; Linear Precision; leading and trailing zeros; unit abbreviation), with an optional Alternate Units block. Precision should match the tolerance: a 0.05 tolerance needs two decimals. Edits in the dialog override Document Settings, and later Document Settings changes do not alter overridden dimensions.

General tolerances#

Place general tolerances in the title block or in a note: for example, "Unless otherwise specified: dimensions in mm, linear +/-0.1, angular +/-0.5 degrees" or "ISO 2768-m". Fusion does not enforce these; they are text you add.

Options reference#

Associativity#

Dimensions are associated with the drawing view: moving the view moves them, and editing the design updates them. If a dimension loses its geometry, an Annotation Monitor badge appears; click it and choose Reassociate, then pick new edges or points. Dimensions in exported DWG files become static objects (see export page).

Dimensioning practice#

1. Put overall dimensions on the outside, feature dimensions closer.
2. Dimension each feature in the view where its shape is shown (profile view).
3. Do not dimension to hidden lines if a section can show the feature instead.
4. Avoid duplicating dimensions; use reference dimensions sparingly.
5. Do not close a chain; if overall size is given, omit one of the chain dimensions.
6. Use consistent units and precision.
7. Align parallel dimensions and keep spacing even.
8. Use TYP and nX for repeated features rather than repeating dimensions.
9. Avoid dimensioning outside what the manufacturing process can hold.
10. Give manufacturers datums that match how the part will be fixtured (see GD&T page).

Tips and pitfalls#

Tip: Add centerlines and center marks first (Geometry panel). Many dimensions to hole centers snap to them, and the drawing looks more professional.

Tip: Use Hole and Thread Note for holes and threads: it fills in the note from the model's hole or thread definition and avoids typing errors.

Tip: Set up default precision in the template so you rarely edit it dimension by dimension.

Warning: Because dimensions measure the model, a "wrong" dimension means the model is wrong. Do not override a dimension's displayed text to make it say something else, except in rare cases flagged with a reference or "NOT TO SCALE" note.

Warning: Chain dimensions with +/- tolerances stack up. Use baseline or ordinate to avoid tolerance accumulation.

ISO fits with real numbers#

The Fit tolerance type generates these limits for you, but it is worth knowing the numbers to check them. General ISO 286 values for a nominal size of 25 mm (the 18 to 30 mm band) are as follows (general standards data, not Autodesk data).

Combine them for the fit: H7/g6 gives a clearance of 0.007 to 0.041 mm (a sliding fit); H7/h6 gives 0 to 0.034 mm (a locational clearance fit); H7/k6 gives -0.015 (interference) to +0.019 (clearance), a transition fit; H7/p6 gives 0.001 to 0.035 mm of interference, a press fit. The practical value of the exercise is the stack-up: for a hole with limits 25.000 to 25.021 mm and a shaft of 24.980 to 24.993 mm, the smallest clearance is 25.000 - 24.993 = 0.007 mm, and the largest is 25.021 - 24.980 = 0.041 mm. Use Show Tolerance "Tolerance class with limits" so the drawing carries both the class symbol and the limits for the shop to check.

Precision and rounding#

Precision must be consistent with the tolerance: +/-0.05 needs two decimals, ISO fits need three. A displayed value of 25.0 with a tolerance of +/-0.05 is inconsistent, because the reader cannot tell the tolerance zone from the trailing zero. For inch drawings, ASME practice shows trailing zeros to the tolerance digit: 1.250 +/-.005. In a template, set one default precision (two decimals in mm) and override only for fits.

Worked example: a plate with a hole pattern#

A plate 100 x 60 mm has four holes at 10 mm in from each corner. Dimensioning with a chain from the left edge gives hole positions 10, 80 and 10, so chain tolerances of +/-0.1 per link stack up: the right-hand hole (reached through two links) could be 0.2 mm off. The same data as ordinate dimensions from the lower left corner reads 10 and 90 in X, 10 and 50 in Y, and each hole position is only affected by its own +/-0.1. If the 90 mm hole spacing is functionally critical, add a position frame, and make the 10 and 90 values basic dimensions. This is the reason ordinate and baseline sets are preferred where tolerance accumulation matters.

Failure modes and fixes#

Workflow advice#

Dimension in a sequence: overall size, then main features, then secondary features, then tolerances. Before you start, decide the datums: a part located on its bottom face and one edge should be dimensioned from those. Aim for no dimension duplicated across views and no feature that has to be calculated by the shop. As a test, cover each dimension in turn and see whether the feature can still be built; if so, the dimension was redundant (and should have been a reference), and if not, it was needed. Finish with a read-through at 100 percent zoom looking for crossing extension lines and small gaps.

Practice exercise#

1. On the Bracket drawing add center marks and centerlines, then overall length and width on the Front view.
2. Dimension two holes and the slot with an ordinate set from the lower left corner. Write down each hole position.
3. Dimension the same features with a chain from the left edge and compute the worst-case position error of the last feature with a +/-0.1 tolerance on each link.
4. Set the hole diameter to the Limit type 6.000 / 6.012, then try the Fit type with a Hole-based H7 preferred fit and compare the limits (an H7 hole at 6 mm is 6.000 to 6.012).
5. Add a note "FIT: 6 H7 / g6, CLEARANCE 0.004 TO 0.020" and verify the numbers: g6 for 6 mm is -0.004 to -0.012, so the shaft is 5.988 to 5.996, giving 6.000 - 5.996 = 0.004 minimum and 6.012 - 5.988 = 0.024 maximum. Correct the note to 0.004 TO 0.024.
6. Place a general tolerance note ISO 2768-m.
7. Expected result: a Front view with no duplicate dimensions, a chain error figure of 0.2 mm versus 0.1 mm for the ordinate set, a limits dimension on the hole, and a fit note whose arithmetic you checked.

Related#

• GD&T and symbols
• Annotations, text, and notes
• Base and projected views