Hidden dangling dimensions make a changed drawing look clean
· 7 min read · Written with an AI assistant
When a design change deletes or rebuilds a feature, drawing dimensions that pointed to it lose their reference. SOLIDWORKS can hide them. Before release, switch that off and look.
A design change deletes a cut and rebuilds it from a new sketch. The model rebuilds without errors, the drawing opens without complaint, and the depth dimension that the inspector checks on every part is simply no longer on the sheet.
That is a dangling dimension that has been hidden. It is one of the quieter ways a drawing and its model drift apart, and it tends to surface at the worst moment: after release, when a supplier asks why a toleranced feature has no tolerance.
Why a dimension dangles, and why nothing fails loudly
A drawing dimension in SOLIDWORKS is not a number typed onto a sheet. It is a reference to model geometry: a face, an edge, a vertex, or a component in an assembly view. The value comes from that geometry. When the geometry goes, the reference has nothing to point to.
The common causes during a change are familiar:
- Deleting a feature and replacing it with a different one, such as swapping a slot for two holes.
- Rebuilding a feature from a new sketch. The new cut may look identical, but its faces and edges are new entities, not the old ones.
- Replacing a component in an assembly, so the edges a drawing view dimensioned belong to a part that is no longer there.
None of these is an error in the model. The part rebuilds cleanly because the part does not know or care what the drawing referenced. The drawing is a downstream consumer, and a lost reference there is treated as a detailing problem rather than a rebuild failure. That is the right design for a CAD system, but it means the burden of noticing falls on whoever checks the drawing.
The setting that hides them
SOLIDWORKS has a document setting that automatically hides dimensions left dangling when the features or components they referred to no longer exist, according to DriveWorks knowledge base article KB13022001. The same article gives its location: Tools > Options > Document Properties > Detailing > “Hide dangling dimensions and annotations”, and notes that because it is a document property, it has to be set in each affected drawing rather than once for the whole system (DriveWorks KB13022001).
The context of that article matters. It is third-party documentation from DriveWorks, not Dassault Systèmes, and it is written for drawings that DriveWorks generates automatically (DriveWorks KB13022001). In a configurator, that makes sense. One master drawing serves many variants. A variant without a particular hole should not carry a stray dimension for that hole. Hiding dangling items is how the template stays tidy across every option.
A manually maintained production drawing is a different object. Each dimension on it was put there by someone for a reason: a fit, an inspection point, a supplier’s process limit. If one of those dimensions loses its reference during a change, hiding it removes the evidence that something needs a decision. The drawing looks finished because the one signal that it is not has been suppressed.
Because the setting lives in each document, it also travels with templates. A drawing created from a template that had it switched on will hide dangling items from day one, and nobody on the current project may know it is set.
A worked example: the pocket that lost its depth
Take a machined aluminium mounting plate. The drawing calls out a rectangular pocket: width, length, corner radius, and a depth of 6.0 ±0.05, because a sensor sits in that pocket and its height above the plate face matters.
An engineering change request asks for the pocket to be lengthened and for its corners to suit a larger cutter. The designer finds the original sketch awkward to edit, deletes the cut-extrude and draws a new one. The new pocket is correct. The model rebuilds.
On the drawing:
- The length and corner radius dimensions referenced edges of the old pocket. They now dangle.
- The depth dimension referenced the old pocket floor. It dangles too.
- A note with a leader,
BREAK ALL SHARP EDGES 0.2 MAX, was attached to an edge of the old pocket. It has lost its attachment. - The width happened to be driven from the plate’s outer edges in this example, so it still resolves.
If the drawing has hiding switched on, the designer sees a section view with a width dimension and nothing else on the pocket. They add a new length and radius because those obviously changed. The depth, which did not change in intent, does not prompt anyone. It goes to release without a depth callout.
With hiding switched off, all four dangling items are in front of the checker. Each one becomes a question with an answer.
A routine before check-in
The aim is simple: no dangling item reaches PDM release by accident. A routine that works on any manually maintained drawing:
- Open the drawing after the model change is complete, not part-way through it.
- Switch hiding off in Tools > Options > Document Properties > Detailing, if it is on (DriveWorks KB13022001). Note that you changed it.
- Rebuild and walk every sheet and every view. Detail and section views are where references most often break, because they focus on the features most likely to change.
- For each dangling dimension or annotation, make one of two decisions:
- Reattach it to the new geometry, then confirm the value and tolerance still express the design intent.
- Delete it deliberately, because the feature it described no longer exists or is now dimensioned differently.
- Write down what you did with each item (see the last section).
- Decide whether hiding should stay off. For a drawing that people will inspect against, the safer default is off, so the next change surfaces its broken references as well.
If a change touches many drawings, the per-document nature of the setting is worth knowing. Checking one drawing tells you nothing about the others, and a script or PDM task that reports the setting across a set of files is a reasonable thing to build.
What tooling should check, and what it should not decide
This is a clean example of where automation helps and where it must stop.
A broken reference is a fact about the file. Software can find every one, list it by sheet and view, and refuse to let a drawing pass a release check while any remain unresolved. That is tedious work for a person and trivial for a machine, and it is the sort of check that should run on every drawing touched by a change, whether or not anyone remembers to look.
What a machine cannot know is why the dimension was there. In the plate example, the depth matters because of a sensor’s mounting height. Nothing in the geometry says so. Reattaching the depth to the new pocket floor is probably right. Reattaching the old length to the new pocket’s edges would silently carry an obsolete value if the dimension were driven rather than reference. Deleting the edge-break note might be fine if a general note covers it, or wrong if it does not.
So the split we think is right for CAD and engineering tooling is:
- Detect automatically: every dangling dimension and annotation, and drawings where hiding is switched on.
- Propose, not apply: a likely new reference, with the reason it was chosen.
- Leave to the engineer: whether the dimension is still needed, what it should point to, and whether its tolerance still holds.
That principle shapes how we are building AI-CAD. Its target workflow includes drawing and verification stages, and an engineer approves every decision. A bounded check like this is where an assistant should be either confident or asking, never guessing quietly.
Record it where the change is recorded
The last step is the one most often skipped. Every reattached or deleted dimension is part of the change, so it belongs in the drawing’s revision description and should match what the change notice says. If the notice says “pocket lengthened” and the drawing also lost and regained its depth callout, a reader comparing revisions deserves to know the depth was reviewed rather than left untouched by luck.
What exactly your revision record must contain depends on the drawing standard and procedure your organisation follows. We have not covered those requirements here; check them against your own procedure before you rely on a particular format.
The broader point holds either way. A dangling dimension is not a cosmetic problem. It is a place where the model changed and the drawing did not keep up. Hiding it is convenient for generated variants and risky for anything released. Turn hiding off, look, decide, and write down what you decided.
If you check drawings differently, or have found references that break in ways we have not described, get in touch. We will keep writing about where drawings and models part company in this journal.