If your SOLIDWORKS sketch is still under defined after adding dimensions, check which geometry can still move. A diameter fixes a circle’s size, but its centre also needs a position relation or locating dimensions. Follow the example below to find the missing constraint, then test that the intended dimension changes without moving the centre.
Use a new practice part. Keep a note of your SOLIDWORKS version and unit system so the exercise is repeatable.
Jump to: the three-state illustration, the symptom checklist, finding the remaining free geometry, or the final check.
Why a diameter does not locate a circle
The circle has a horizontal centre coordinate, a vertical centre coordinate and a diameter. A diameter dimension fixes size, leaving two position variables. Making the centre coincident with the fixed origin removes those two freedoms. This explains why adding a size dimension alone can leave a sketch under defined.
1. Create a deliberately simple sketch
Start a sketch on the Front plane and draw one circle away from the origin. Do not place the centre on another point or line. Automatic relations can still be added while drawing, so inspect the relations that actually exist before proceeding.
Use the status bar and the geometry’s state to inspect the sketch. In the default colour convention, under-defined entities appear blue and fully defined entities black. Colour settings and selection highlighting can differ; the displayed status and relation list are the stronger checks.
The official Sketch Geometry Status guide includes real interface examples of the different states. Use it as the visual reference for your installed version.
2. Separate size from position
For this isolated circle, ask three questions: where is the centre horizontally, where is it vertically, and what is the diameter? A diameter dimension answers only the third question.
- Add a diameter dimension of 20 mm. This is an invented teaching value.
- Try moving the circle’s centre in the practice sketch. If no position relation was added, it should still be free to move.
- Choose the intended design: a circle centred on the origin, or a circle offset from it. Those are different constraint choices.
If the circle does not behave as expected, inspect existing relations first. An automatic coincident relation or a Fix relation may already constrain it.
3. Add the intended position constraint
For the origin-centred version, select the circle centre and the sketch origin and add a coincident relation. Together with the diameter, that should define this simple circle. For an offset version, use horizontal and vertical dimensions from the origin instead, with explicit teaching values such as 30 mm and 15 mm.
Record which design you chose. Making the centre coincident and also demanding nonzero offsets describes conflicting intentions. Similarly, a Fix relation can stop motion without making the intended origin or dimensional relationship clear to the next engineer.
Open Display/Delete Relations to inspect the relation attached to the centre. Confirm that you constrained the centre point you intended, rather than an unrelated piece of geometry.
4. Verify the result with a controlled change
Change the diameter from 20 mm to 24 mm. The centre should remain at its intended location while the size changes. Restore 20 mm and verify the sketch status again. Save your practice file with a name that identifies the chosen case.
A sketch can be fully defined and still describe the wrong design. The useful result is both a solved sketch and predictable behaviour under the changes the design is supposed to allow.
5. Diagnose a sketch that remains under defined
| Observation in the practice file | Check next |
|---|---|
| Circle size stays fixed but its centre moves | Inspect the centre’s position relations or horizontal/vertical locating dimensions. |
| A shown dimension changes when you drag | Check whether it is a driven measurement rather than a driving dimension. |
| The main profile looks defined, but sketch status is not | Inspect construction geometry, loose endpoints and imported or duplicated entities. |
| Adding one relation creates an over-defined state | Read the existing relations and dimensions for a conflict or redundancy before removing anything. |
A line or point can look coincident with another without having the intended relation. Check the relation record and the sketch status; screen position or colour alone is insufficient. See the official sketch status conventions.
Fully Define Sketch can calculate additional dimensions and relations for selected entities or the entire sketch. Review its proposed datums and relationships against your intention before accepting them. Automatic completion is most useful when you understand what the result should mean.
How do I find what is still under defined?
Read the whole sketch’s status in the status bar, then inspect individual entities. A solved outline does not establish the state of every construction line or point in the sketch.
- In the practice copy, select a suspect endpoint, centre or construction entity and gently try dragging it. Observe whether position, length, angle or size changes; undo the move afterward.
- Open Display/Delete Relations. Inspect the selected entity’s relationships and referenced geometry. Its filters can isolate dangling or conflicting relations, but they are not an automatic list of every missing constraint.
- Add the relationship that expresses the intended design, then repeat the controlled-change check. If a new relation produces a conflict, inspect the existing constraints before deleting one.
Why did Fully Define Sketch leave something unresolved?
Check whether you chose selected entities or all entities. Also review which relations were permitted: the Fully Define Sketch PropertyManager can be unable to complete a sketch when needed relation types are excluded. Review the proposed horizontal and vertical datums before accepting calculated dimensions. A Fix relation can conceal the missing design relationship, so use it only when fixing that geometry is your actual intent.
Final check: which change should still be possible?
For the origin-centred circle, try to drag the centre, then edit the driving diameter from 20 mm to 24 mm. Write the expected result before performing the two actions.
Show the expected result
Dragging should not relocate the centre. Editing the diameter should change the circle’s size while keeping the centre at the origin. Fully defined means the current dimensions and relations determine the geometry; it does not mean you can never edit a driving dimension. If your result differs, inspect automatic relations and the selected entities before continuing.
Continue and consult the official illustrations
Continue with assembly mate troubleshooting to apply the same reasoning to components. Use the configuration and BOM tutorial when different design variants must retain clear identities.
When you reach an assembly BOM review, try BOM Check to flag missing values, repeated parts and conflicting fields in a CSV. It checks the supplied BOM data; sketch constraints still need to be inspected in SOLIDWORKS.
- Sketch Geometry Status, including illustrated states.
- Fully Define Sketch PropertyManager and illustrated dimension schemes.
- Fully Defined Sketches overview.
Frequently asked questions
Why is my SOLIDWORKS sketch still under defined after adding dimensions?
Some geometry can still move. A diameter fixes a circle's size, but its centre also needs a relation to the origin or locating dimensions. Drag the blue entities to see which freedom remains.
How do I find what is under defined in a SOLIDWORKS sketch?
Look for blue entities and the status bar message, then drag each blue point or line. Display/Delete Relations lists the relations that exist, which helps you see what is missing.
What do blue, black and red sketch colours mean?
In the default scheme, blue is under defined, black is fully defined, and red or yellow indicates over-defined or conflicting geometry. Colour settings can vary, so trust the status bar and relation list.
Does a sketch have to be fully defined?
SOLIDWORKS can build features from under-defined sketches, but fully defined sketches change predictably when you edit dimensions. Many teams require fully defined sketches in released parts.
How do I fix an over-defined sketch?
Open Display/Delete Relations or SketchXpert, find the redundant or conflicting relation or dimension, and remove one at a time until the sketch solves without errors.
Reviewed against official documentation on 5 October 2026. This exercise was not executed in a SOLIDWORKS session for this publication; use the stated observations to verify it in your installed release.
MST Engineering Intelligence. “SOLIDWORKS Sketch Under Defined? Find the Missing Constraint.” MST Engineering Intelligence. Updated 2026-11-02. https://mst-us.ai/solidworks-under-defined-sketch-tutorial/
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