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Find the under-defined sketches before you change a dimension

· 6 min read · Written with an AI assistant

A dimension edit is only as predictable as the sketch it lives in. Here is how to audit a SOLIDWORKS part for under-defined sketches before a change, stop new ones, and use Fully Define Sketch without locking in accidents.

A dimension change is only as predictable as the sketch it sits in. If that sketch is under-defined, editing one value can move geometry nobody asked to move, and the feature tree will rebuild without complaint.

This is a common way for a routine engineering change to go quietly wrong. The part rebuilds, the drawing updates, the reviewer checks the dimension that changed, and nobody checks the hole that drifted. This article covers how to find loose sketches in a SOLIDWORKS part before you edit it, how to stop new ones appearing, and how to use the Fully Define Sketch tool without turning a modelling accident into a documented requirement.

A note on sourcing: the SOLIDWORKS behaviour described here comes from a Hawk Ridge Systems article, first published in 2014 and updated in September 2026. Menu names and paths can shift between releases, so confirm them against Dassault’s help for your version, such as the Fully Define Sketch PropertyManager page.

Why a loose sketch is a change risk

A fully defined sketch has one solution. Every entity’s size and position follows from dimensions and relations. An under-defined sketch has many solutions, and the solver picks one. Usually it picks the one closest to where the geometry already is, which is why loose sketches look fine for years.

The trouble starts when something else in the sketch changes. Free entities are positioned by whatever happened to be true when they were drawn, not by any rule. Change a neighbouring dimension and the free geometry either stays put when it should have moved, or moves when it should have stayed. Either way, the model no longer says what the designer meant.

There is a second, quieter cost. A loose sketch does not tell the next engineer what matters. If a hole has a vertical dimension but no horizontal one, is its horizontal position critical or arbitrary? The model cannot answer, and the engineer approving a change has to guess.

A worked example: the hole that stopped being centred

Take a mounting plate. The base sketch is a 120 mm by 80 mm rectangle with its lower-left corner on the origin. A clearance hole sits in the middle of the plate. The designer added a 40 mm vertical dimension to the hole centre, then moved on. The horizontal position was never constrained. The hole was dragged to roughly the middle, at 59.7 mm from the left edge.

A change request arrives: widen the plate to 160 mm to suit a new enclosure. The engineer edits the 120 to 160 and rebuilds. No errors, no warnings. The hole stays at 59.7 mm. It is now well off-centre on a plate where every mating part assumes it is centred.

Nothing in the rebuild flags this. The only clue was in the feature tree before the edit: the sketch name carried a minus sign.

Auditing a part before you edit it

SOLIDWORKS puts a minus sign, (-), in front of the name of an under-defined sketch in the feature tree, according to Hawk Ridge Systems. In a long tree, those flags are easy to miss when sketches are folded under features.

The Search Filter at the top of the feature tree searches the whole tree by name, so typing sketch lists every sketch and makes the (-) entries easy to spot, as the same article describes. This only works cleanly if sketches keep a name containing “sketch”. If your team renames sketches to describe their purpose, which is good practice for readability, you will need a naming convention the filter can still catch.

For a change review, you do not have to fix every loose sketch in the part. You need to know which loose sketches sit upstream of, or inside, the geometry you are about to change. Those are the ones that can move.

Preventing new ones

Under System Options > Sketch there is a setting called Use fully defined sketches. With it on, you cannot leave a sketch until it is fully defined, and a warning appears if you click Exit Sketch too early, per Hawk Ridge Systems.

Its limit matters for change work. Turning the option on does not flag sketches that were already under-defined; those still have to be found and fixed one at a time, the article notes. So the setting protects new work but tells you nothing about a legacy part pulled out of PDM for a revision. The audit above still has to happen.

In our view the option is worth turning on as a team standard. It costs a few seconds per sketch and removes the class of problem in the worked example. The friction is the point.

Fully Define Sketch: useful, but it dimensions what is there

The Fully Define Sketch tool only appears while you are editing an under-defined sketch, according to Hawk Ridge Systems. It asks for three inputs:

You click Calculate, check the preview, then click OK, and you can move the dimensions afterwards, as the same source explains. The article suggests the tool for large, messy, copied or converted sketches, or for sketches that do not matter much.

That recommendation is sensible, and it hints at the catch. What follows is our reasoning, not the source’s. The tool resolves the degrees of freedom that are left. It cannot know why they were left. Run it on the mounting plate before the change, with a Baseline scheme from the origin, and it will happily add a 59.7 mm dimension to the hole. The sketch is now fully defined, the (-) disappears, and the accident has become a dimension that looks deliberate. The right fix was a midpoint relation, or a dimension that expresses centring.

So treat the tool’s output as a draft:

  1. Choose the datum deliberately. Measure from the feature that controls fit or function, not just the origin.
  2. Choose the scheme to match how the part will be inspected. Baseline and ordinate dimensions from a datum often read more like the drawing than chained dimensions do.
  3. Read every added dimension. Odd values such as 59.7 usually mark geometry placed by eye. Replace them with relations or round values that carry intent.

What this means for CAD and engineering tooling

Sketch status is cheap to read and expensive to ignore, which makes it a good candidate for an automatic check. Any tool that edits a model on an engineer’s behalf, whether a macro or an AI agent, should check the definition state of the sketches it touches before it changes a value, and report the loose ones rather than silently running Fully Define Sketch over them. Auto-completing constraints is exactly where intent gets lost.

This is the kind of verification we want in AI-CAD, the engineering copilot we are building for SOLIDWORKS. It is a prototype, and the principle is that the agent proposes and the engineer approves: flag the (-) sketches upstream of a change, suggest relations, and let a person decide what the design intent was.

A pre-change checklist you can run by hand today:

1. Filter the feature tree for "sketch"; list every (-) entry.
2. Mark which loose sketches drive the geometry being changed.
3. For each, decide the intent of every free entity.
4. Add relations or dimensions that state that intent.
5. Use Fully Define Sketch only for copied/converted geometry,
   then review every dimension it added.
6. Make the change, rebuild, and re-check positions that matter.
7. Note what was locked down in the change record.

Closing

A rebuild with no errors is not evidence that a change did what was intended. It only shows the solver found an answer. Finding the under-defined sketches first, and pinning them to real design intent rather than to wherever the geometry happened to sit, is a few minutes of work that makes the change predictable and leaves the model readable for whoever edits it next. If you have a team standard for sketch definition that works, we would like to hear about it; follow the journal for more on keeping parametric models editable.

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