How to Resolve Under-Defined Sketches in SOLIDWORKS

In SOLIDWORKS, it is considered best practice to fully define your sketches. A fully defined sketch is predictable, stable, and far less likely to break downstream features when you edit dimensions or update design intent. In contrast, under-defined sketches still have degrees of freedom (DOF) – entities can shift, resize, or rotate unexpectedly, which can cause assemblies or features to rebuild in ways you didn’t intend.

To help with this, SOLIDWORKS provides the Fully Define Sketch tool. This tool automatically adds the dimensions and sketch relations needed to fully define selected entities or an entire sketch. You can let SOLIDWORKS do most of the work, then fine-tune the dimensions and relations as needed.

You may have noticed that even if you enable Add Dimensions when using Sketch Pattern, some pattern instances remain under-defined. This is especially common when instances are still free to rotate. In this article, you’ll learn why this happens and how to systematically find and resolve under-defined sketches in SOLIDWORKS using the Search Filter, the Use fully defined sketches option, and the Fully Define Sketch tool.

What Is an Under-Defined Sketch in SOLIDWORKS?

Every sketch in SOLIDWORKS has a status:

• Under-defined – some geometry can still move or change size (missing dimensions or relations).
• Fully defined – all geometry is locked in size and position.
• Over-defined – conflicting or redundant dimensions/relations exist.

By default, SOLIDWORKS gives you clear visual feedback:

• Blue sketch entities are under-defined.
• Black sketch entities are fully defined.
• Red entities indicate over-definition or conflicts.

In the FeatureManager design tree, SOLIDWORKS also uses prefixes on sketch names:

• (–) before the sketch name – the sketch is under-defined.
• (+) – the sketch is over-defined.
• (?) – the sketch cannot be solved.
• No prefix – the sketch is fully defined.

When you see a minus sign (–) next to a sketch and blue sketch entities, SOLIDWORKS is telling you that something is still free to move. That “something” might be as simple as a missing length dimension or as subtle as a rotational degree of freedom in a sketch pattern.

Why Sketch Patterns Are Often Under-Defined

A very common source of under-defined sketches is sketch patterns (especially older models or legacy templates). Even if you add spacing dimensions, pattern instances can remain under-defined because they’re still allowed to rotate.

Before SOLIDWORKS 2017, instances in a Linear Sketch Pattern could rotate unless you manually locked them with extra relations. Adding a Horizontal or Vertical relation to one of the construction lines tied to the instances was a common workaround to fully define the pattern.

From SOLIDWORKS 2017 onward, linear sketch patterns were enhanced so that the instances can be locked automatically based on Direction 1. When you enable options such as:

• Dimension X spacing
• Fix X-axis direction
• Dimension Y spacing
• Dimension angle between axes

the software can fully define a linear pattern of a fully defined seed entity, including the rotation of each instance.

However, Circular Sketch Patterns can still remain under-defined if the construction geometry or angles are not fully constrained. In such cases, you may need to add:

• Horizontal or vertical relations to construction lines.
• Angular dimensions that lock the rotation of the pattern.
• Additional relations such as concentric, coincident, or equal, depending on the geometry.

Understanding these pattern behaviors will help you diagnose why a sketch that looks “dimensioned” is still under-defined.

How to Find and Resolve Under-Defined Sketches in SOLIDWORKS

On large parts and assemblies, manually hunting for under-defined sketches can be tedious. SOLIDWORKS provides a couple of tools that make this much easier:

• The Search Filter at the top of the FeatureManager design tree.
• The Use fully defined sketches system option.

Below, we’ll walk through a practical workflow that uses both.

Step 1: Identify Under-Defined Sketches in the Feature Tree

At the very top of your FeatureManager design tree is a Search Filter box. Type “sketch” (or any part of a sketch name) to quickly filter the tree and show only the sketches and related features.

Step 1: Look for sketches with a (–) in front of the name. These are the sketches that are under-defined and candidates for cleanup.

Step 2: Enable “Use fully defined sketches”

To prevent new under-defined sketches from slipping into your models, enable a system option that forces sketches to be fully defined before you can exit them.

Step 2: Go to Tools > Options > System Options > Sketch and enable Use fully defined sketches.

With this option turned on, SOLIDWORKS will warn you when you try to exit a sketch that is still under-defined. This encourages good practice and helps prevent new under-defined sketches from being created as you work.

Note that this option does not retroactively fix or “flag” sketches that were already under-defined before you enabled it. Those existing sketches will still need to be found (using the minus sign in the FeatureManager tree) and manually edited.

Step 3: Edit Under-Defined Sketches and Respond to Warnings

Step 3: Double-click one of the under-defined sketches (with the (–) prefix) to edit it. As you try to exit the sketch while it is still under-defined, SOLIDWORKS will display a warning dialog indicating that the sketch is not fully defined.

This dialog gives you the choice to exit anyway or stay in the sketch to finish adding dimensions and relations. If your goal is a robust model, you should generally stay in the sketch and fully define it before exiting.

Step 4: Exit Once the Sketch Is Fully Defined

Step 4: Continue adding dimensions and relations until all entities are black and the status bar reads Fully Defined. When you then click Exit Sketch, SOLIDWORKS will allow you to leave the sketch without any warning.

Once you repeat this process for all sketches with a (–) prefix, your FeatureManager design tree will no longer display under-defined sketches — no more minus signs cluttering the tree, and far fewer surprises when you edit your model later.

Using the Fully Define Sketch Tool

Manually adding every dimension and relation is sometimes overkill, especially for imported, copied, or “utility” sketches. In these cases, the Fully Define Sketch tool can automatically add the constraints needed to lock things down.

This tool is particularly helpful when:

• You have large, messy sketches created by converting or importing geometry.
• You’ve copied sketch entities from another feature or part.
• You simply want SOLIDWORKS to finish constraining a sketch and then make small adjustments afterward.

Consider the example of a simple LEGO®-style head profile. The goal is to quickly fully define the sketch and remove the remaining degrees of freedom.

Step 1: Edit the Sketch and Access Fully Define Sketch

Step 1: Edit the under-defined sketch you want to complete. While the sketch is active, access the Fully Define Sketch tool from one of the following:

• Dimensions/Relations toolbar – click Fully Define Sketch.
• Tools > Dimensions > Fully Define Sketch.
• The Sketch tab on the CommandManager under Display/Delete Relations.

If the command is grayed out, you’re not currently editing a sketch. Once you’re in an active sketch, the Fully Define Sketch PropertyManager will appear.

Step 2: Set Entities, Relations, and Dimension Schemes

The Fully Define Sketch PropertyManager controls how SOLIDWORKS will automatically constrain your geometry. It’s organized into three key areas:

1. Entities to Fully Define
   Choose whether to define the entire sketch or only specific selected entities. This is useful if you want to control certain critical geometry manually but let SOLIDWORKS handle the rest.
2. Relations
   Specify which sketch relations SOLIDWORKS is allowed to apply automatically (for example: horizontal, vertical, coincident, concentric, collinear, perpendicular, parallel, equal). These relations help constrain geometry without adding unnecessary dimensions.
3. Dimensions
   Control how dimensions are placed. You can set:
   • The scheme (such as chain, baseline, or ordinate dimensions for linear geometry).
   • The origin or reference point for dimensions.
   • The general placement of dimensions (how far and in what direction they are pulled from the entities).

   These settings affect how the dimensions are displayed, not their numeric values.

Step 3: Calculate and Review the Result

Step 3: Click Calculate in the PropertyManager to let SOLIDWORKS propose the dimensions and relations needed to fully define the selected entities. You’ll see a preview of the added constraints and dimensions.

If the result looks reasonable, click OK (the green check). After exiting the PropertyManager, you can drag dimension callouts to clean up the sketch and improve readability. If you don’t like the result, you can undo and adjust the options before trying again.

Step 4: Exit the Sketch

Step 4: Once the sketch is fully defined (all geometry black, no (–) prefix in the FeatureManager tree), click Exit Sketch. With the Use fully defined sketches option enabled, you should no longer see warnings for this sketch.

Sometimes, leaving a sketch slightly under-defined is acceptable — for example, during a quick demo, a concept study, or when intentionally allowing certain geometry to slide or scale. However, for production models and collaborative projects, enforcing fully defined sketches generally results in far more robust designs.

How to Quickly Fully Define Your SOLIDWORKS Sketch

Most SOLIDWORKS part models begin as one or more 2D sketches. Investing a bit of time to define those sketches properly greatly reduces rebuild issues later. Below are a couple of simple but effective habits that help you fully define sketches quickly.

1. Copy and Paste Sketch Geometry Efficiently

You can reuse sketch geometry by using standard keyboard shortcuts: Ctrl + C to copy and Ctrl + V to paste, or by holding Ctrl and dragging entities in the graphics area.

For example, suppose you have a circle on the left side of a sketch that you’d like to repeat on the right. Instead of sketching a new circle from scratch, you can window-select the original circle, copy it, and paste or drag-copy it. This keeps the shape consistent and often reduces the number of dimensions you need to add.

After copying, if you want those circles to always remain the same size, you can apply an Equal relation between them so that changing one automatically updates the other. This is a simple way to enforce design intent while still sketching quickly.

2. Use Fully Define Sketch to Lock Things Down

Once you’ve roughed in your geometry and added any critical dimensions manually, use the Fully Define Sketch PropertyManager to finish the job:

• Click Tools > Dimensions > Fully Define Sketch, or choose Fully Define Sketch from the Dimensions/Relations toolbar.
• Select All entities in sketch if you want SOLIDWORKS to constrain everything at once.
• Customize which relations and dimension schemes are applied, then click Calculate and OK.

This is especially powerful on large or imported sketches where manually chasing every missing dimension would be tedious. The tool can rapidly add all remaining dimensions and relations, after which you can fine-tune names, placements, and values to match your design standards.

Finally, for multi-contour sketches, you can use the Selected Contours option of features like Extruded Boss/Base to turn different regions of a single, fully defined sketch into multiple features. This allows you to drive more of your part from one robust sketch while still maintaining control.

Conclusion

Under-defined sketches are a major source of instability in SOLIDWORKS models. A sketch that’s allowed to move or rotate can cause features or assemblies to update in unexpected ways when changes are made later in the design process.

By learning how to:

• Recognize under-defined sketches using colors and the (–) prefix in the FeatureManager tree,
• Use the Search Filter and enable Use fully defined sketches in System Options, and
• Apply the Fully Define Sketch tool to automatically add dimensions and relations,

you can systematically resolve under-defined sketches and greatly improve the robustness of your models.

In day-to-day work, you may occasionally accept under-defined sketches for quick experiments or demonstrations. But for production designs and long-term projects, fully defined sketches are one of the simplest, most effective ways to keep your SOLIDWORKS parts and assemblies predictable, stable, and easy to modify.