How to Show Dimensions in a SOLIDWORKS Part
Contents
To show dimensions in a SOLIDWORKS part, first identify which dimensions you need. Sketch dimensions are visible while editing a sketch and can also be displayed when the sketch is not active. Feature dimensions belong to operations such as extrudes, cuts, fillets, and holes. Annotation or MBD dimensions use a separate visibility control. Drawing dimensions are shown in a drawing document, not permanently over the part graphics area.
If dimensions are missing, the cause is usually a disabled visibility control, a hidden sketch or annotation, an unselected feature, or geometry covering the dimension text. The steps below separate those cases so you can restore the dimensions without creating duplicates.
Show dimensions while editing a sketch
- Expand the part’s feature tree and right-click the sketch.
- Select Edit Sketch.
- Open View > Hide/Show and make sure Sketch Dimensions is enabled.
- You can also use the Hide/Show Items eye icon on the Heads-Up View toolbar.
A fully defined sketch does not require every dimension to remain visible at all times, but you need enough dimensions and relations to control the intended shape. Use Smart Dimension to create missing driving dimensions. Do not add a second dimension merely because an existing one is hidden; show the existing dimension first and check whether the sketch is already defined.
Preview a sketch dimension without showing everything
Current SOLIDWORKS versions can preview sketch dimensions when you select sketch geometry. Go to Tools > Options > System Options > Sketch and enable Preview sketch dimension when selected. When you select a supported sketch entity, its dimension can appear temporarily and can be selected for editing. The preview disappears when you click elsewhere.
This is useful in a crowded sketch because you can inspect one entity without displaying every dimension. A preview is not a new driving dimension, and it should not be confused with a hidden dimension that remains part of the sketch.
Show sketch dimensions when the sketch is not active
You can inspect dimensions without entering Edit Sketch mode:
- Expand the feature that contains the sketch.
- Click or right-click the sketch in the FeatureManager design tree.
- Show the sketch if it is hidden.
- Use the sketch-dimension visibility control or select the sketch to expose its dimensions.
If the sketch dimensions still do not appear, edit the sketch and verify they exist. Imported bodies and direct-edit geometry may not have the original parametric sketch dimensions. For imported models, the guide to files SOLIDWORKS can open explains why neutral geometry may arrive without its design history.
Show feature dimensions in a part
Feature dimensions control values such as extrusion depth, cut depth, fillet radius, shell thickness, pattern spacing, and feature position. To display them:
- Select the feature in the FeatureManager design tree.
- Look for its dimensions in the graphics area.
- If necessary, right-click the Annotations folder and use the feature-dimension display command available in your version.
- Right-click an individually hidden dimension and choose Show.
Selecting the feature is often the fastest method because SOLIDWORKS displays the dimensions associated with that feature only. Double-clicking a displayed driving dimension lets you edit its value; rebuild the model afterward and check downstream features.
Do not change a feature dimension only to make it easier to read. Its value controls geometry. If you only need a measurement, use the Measure tool or create a reference dimension rather than altering a driving dimension.
A dimension can be enabled but still appear missing because the part blocks the text or extension lines. Rotate the model, zoom out, or drag the dimension into a clear area after selecting the relevant sketch or feature.
If many dimensions overlap, show only the sketch or feature you are working on. Displaying every dimension across a complex part makes selection harder and increases the chance of editing the wrong value.
Show annotations and MBD dimensions
Annotations, DimXpert dimensions, and model-based definition information are not controlled by the sketch-dimension toggle. Use View > Hide/Show > Annotations to control annotation visibility in parts and assemblies. Also check the Annotations folder and any annotation views that organize 3D product manufacturing information.
If the part contains MBD data but nothing appears, verify the correct annotation view is active and that the individual annotation has not been hidden. These dimensions communicate product definition and should be reviewed differently from dimensions that drive a feature sketch.
Model dimensions versus drawing dimensions
Dimensions visible in a part are not automatically a finished manufacturing drawing. In a SOLIDWORKS drawing, you can insert model dimensions into appropriate views with Model Items, or create reference dimensions that document the drawing without changing model geometry.
Inserted model dimensions remain associated with the part. Editing an inserted driving dimension can change the model. Reference dimensions are normally shown as driven values and should be used when the dimension is needed for information rather than feature control.
For drawing documentation, see SOLIDWORKS detailing and drawing techniques and how to create a SOLIDWORKS title block.
Common reasons dimensions do not show
Sketch Dimensions is turned off
Enable it from View > Hide/Show or the Hide/Show Items eye icon, then reopen or select the sketch.
Right-click the sketch in the FeatureManager design tree and select Show, then verify sketch-dimension visibility.
The feature is not selected
Click the feature that owns the dimension. SOLIDWORKS often shows feature dimensions contextually rather than keeping every one visible.
The part has no editable feature history
An imported STEP, IGES, or parasolid body may contain geometry without the source sketches and dimensions. You may need FeatureWorks, direct editing, or manual remodeling. The Convert Entities guide covers one way to reuse existing geometry in a new sketch.
Dimensions are behind the model
Rotate the view, zoom out, switch to a standard orientation, or move the displayed dimension into clear space.
Annotations are turned off
Use View > Hide/Show > Annotations for MBD and annotation dimensions; the sketch-dimension control does not manage them.
A dimension was deleted
If the sketch becomes under-defined after deletion, recreate the required controlling dimension with Smart Dimension. If the sketch remains fully defined, inspect its relations before adding another constraint.
Dimension types you may encounter
- Driving dimensions: control sketch or feature geometry.
- Driven or reference dimensions: report a value without controlling it.
- Sketch dimensions: define lines, arcs, circles, positions, and angles inside sketches.
- Feature dimensions: control feature parameters such as depth, radius, or spacing.
- DimXpert and MBD dimensions: communicate 3D manufacturing definition.
- Drawing dimensions: document drawing views and may be inserted model dimensions or drawing references.
Linear, angular, radial, diameter, ordinate, chamfer, and hole-callout formats describe how a value is presented. The more important distinction during troubleshooting is whether the dimension drives the model, reports a value, belongs to an annotation, or exists only in a drawing.
Bottom line
To show dimensions in a SOLIDWORKS part, enable Sketch Dimensions for sketches, select the owning feature for feature dimensions, and use annotation visibility for MBD information. If a dimension still appears missing, check whether the sketch is hidden, the model obscures the text, or the imported part has no parametric history. Create a new dimension only after confirming the original one does not already exist.
Official references: Previewing Sketch Dimensions, Dimensions, Hiding and Showing Annotations, and Inserting Dimensions into Drawings.
