Use a driven sketch dimension. Inventor stores it as a reference parameter that measures existing geometry, updates when the geometry changes, and does not resize that geometry. This is the right approach for a read-only calculated result; use a normal dimension or a user parameter when the value must drive design intent.
Driven dimension, normal dimension, or user parameter?
| Type | Controls geometry? | Updates from geometry? | Directly editable? | Best use |
|---|---|---|---|---|
| Normal (driving) dimension | Yes | Not applicable | Yes | Design requirement or input |
| Driven (reference) dimension | No | Yes | No | Measured result or report value |
| User parameter | Only when referenced by an equation | Not inherently | Yes | Named, reusable design input |
A driven dimension appears in parentheses in the sketch. It is still represented in Inventor’s parameter system, but it is non-driving: changing it cannot directly alter the sketch. See Autodesk’s explanation of driven dimensions and reference parameters at Autodesk Inventor Help.
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Method 1: Add a driven dimension directly
Inventor 2026 documentation places the command on the Sketch tab; older releases can arrange ribbon panels differently.
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- Edit the part sketch, or create a new 2D sketch.
- On Sketch > Format, activate Driven Dimension.
- Choose Sketch > Constrain > Dimension.
- Select the geometry and place the dimension. Select a line for length, two points or elements for distance, a circle for diameter or radius, or suitable line pairs for angular measurements.
- Turn off Driven Dimension when you need to return to ordinary driving dimensions.
The corresponding control is available on the 3D Sketch tab for 3D sketches. Dimension types depend on the selected entities and command context; Autodesk lists linear, aligned, angular, radial, and diameter dimensions at Sketch dimension types.
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Method 2: Measure a fully constrained sketch
This is often the fastest way to capture an existing result.
- Edit the fully constrained sketch.
- Start Dimension and select the entities to measure.
- When Inventor warns that the dimension would over-constrain the sketch, choose Accept, not Cancel.
- Inventor saves the new dimension as a reference (driven) parameter. Its value follows later changes to the underlying geometry.
The warning is expected here: you are deliberately adding information without adding another constraint that controls the shape.
Find and name the captured parameter
- Exit the sketch if necessary.
- Open Manage > Parameters > Parameters.
- Expand Model Parameters and locate the reference parameter, often initially named
d0,d1, and so on. - Rename it to a durable identifier such as
MeasuredSlotLength,OverallWidth,HoleSpacing, orClearanceValue; add a comment when its purpose is not obvious.
Sketch dimensions and other model measurements are automatically listed in the Parameters dialog. A driven measurement normally remains a model/reference parameter, not a manually created User Parameter. Autodesk documents the browser and naming workflow at Parameters dialog.
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For a normal editable dimension, an expression such as OverallWidth = 125 mm can name the parameter while editing. For driven dimensions, create the measurement first and rename it in the Parameters dialog for the most consistent result across releases.
Use the measurement in equations and iLogic
A named reference parameter can feed downstream calculations. For example:
Clearance = MeasuredSlotLength - NominalInsertLengthNumeric parameters support expressions in dimension fields, feature dialogs, and the Parameters dialog; text and true/false parameters do not. See Inventor parameter expressions.
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Reference parameters are also exposed through Inventor’s parameter system for iLogic and other automation. Use a named measurement as an input to a rule that reports values, selects configurations, or updates metadata, but verify syntax for the target Inventor release and rule context. Autodesk’s parameter-type guidance is at Reference parameters and parameter types.
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NominalWidth = 100 mm
MeasuredWidth = actual resulting width
Clearance = MeasuredWidth - RequiredWidthExport the value to properties, BOMs, or parts lists
- Open Manage > Parameters.
- Enable Export Parameter for the named measurement.
- Click Done.
- Open iProperties > Custom and verify the generated property.
The custom property can then be selected in BOMs and parts lists. Inventor also supports XML parameter import and export; the documented workflow is in the Parameters help.
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Show the name, expression, or precise value
While editing a sketch, use the dimension display options Value, Name, Expression, Tolerance, or Precise Value. Name is useful when reviewing a parameterized sketch; Precise Value prevents display rounding from being mistaken for a calculation failure. Set the document-wide default at Tools > Document Settings > Units > Modeling Dimension Display. Details are in Autodesk’s dimension display settings.
Put the result on a drawing
A model parameter does not automatically become a manufacturing annotation in every drawing view. In a drawing, select the appropriate part or feature and use Retrieve Dimensions; view-plane and selection limitations apply, so some parameters may not be suitable for every view. See Retrieve Dimensions.
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The dimension is not editable
That is normal for a driven/reference dimension. Turn off Driven Dimension or convert the selected dimension to driving. If that over-constrains the sketch, remove a conflicting constraint or convert another driving dimension to driven first.
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The sketch becomes distorted
Stabilize the shape with geometric constraints before adding dimensions, and dimension larger elements before smaller ones. Poor constraint order can let under-constrained geometry move unexpectedly.
The value appears not to update
- Confirm that the referenced geometry actually changed.
- Check that the intended entities were selected.
- Update the model with the Update command when required by the operation.
- Check model states, derived parts, or feature configurations that may suppress or replace the source geometry.
- Switch to Precise Value to rule out display rounding.
You cannot find the parameter
Look under model/reference parameters rather than only User Parameters, and search for its automatic name if it has not been renamed. A transient result from the ordinary Measure command is not necessarily a durable associative parameter; placing a driven sketch dimension is the reliable parametric workflow.
The drawing does not show it
Retrieve the model dimension into a suitable view, or create a separate drawing dimension when the value is documentation rather than a model constraint.
When a user parameter is the better choice
Create a user parameter with Parameters > Add Numeric when the value is an intentional requirement, is reused across features, or should remain clearly separate from automatically generated model parameters. For example, keep RequiredClearance = 2 mm as an input and compare it with a measured result. User parameters can also support equations, iLogic, templates, and spreadsheet-linked design tables. Spreadsheet links are useful for families of parts but add external file-management considerations; Autodesk documents the link workflow at spreadsheet-linked parameters.
The core workflow needs no add-on: driven dimensions, model parameters, equations, iLogic, and property export are Inventor capabilities. Excel, Vault, or consulting services are optional choices for larger configuration or document-control systems, not prerequisites for capturing one measurement.
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