Sketch Fully Constrained but Dimension Cannot Be Added
A colleague hands you a sketch of a linkage arm that reports fully constrained. You need to add a 15 mm dimension between two hole centers to match a revised drawing. When you place the dimension, Inventor accepts it as a driven (reference) dimension and will not let you edit the value. The sketch has two holes, an arc slot, and several construction lines. The colleague says the sketch was copied from another part and pasted, then re-constrained. The revised design requires the hole spacing to be exactly 15 mm, and other geometry must adapt.
1. Explain why the new dimension becomes driven and how to identify what is controlling the spacing.
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A new dimension becomes driven when the sketch already has no remaining degrees of freedom, meaning the distance is already determined by existing constraints or dimensions. Because the sketch was pasted from another part, it may carry coincident, equal, symmetry, or projected geometry constraints that fully fix the hole centers. The 15 mm distance is therefore a computed result, not a free parameter, so Inventor reports it as reference.
To find the controlling geometry, display all constraints and dimensions, then drag one hole center; if it will not move, the sketch is rigid. Temporarily suppress dimensions one at a time or convert suspect dimensions to reference and watch which entity gains freedom. Look especially for symmetry constraints about a construction centerline, equal-radius constraints on the two holes, and any projected edges from the source part that were pasted along with the sketch. The controlling item is the one whose removal allows the hole to move.
2. How do you make the 15 mm spacing driving while keeping the rest of the sketch adaptive?
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Remove or relax the constraint that fixes the spacing, then add the 15 mm dimension as a driving dimension. Practically: identify the controlling constraint (often symmetry or a pasted projected edge), delete or suppress it, and immediately place the 15 mm dimension between the hole centers. Confirm it is driving by editing the value and watching the geometry update. If the sketch then becomes over-constrained elsewhere, convert one existing dimension to reference or replace a redundant constraint with the new dimension.
To keep the rest adaptive, ensure the holes are constrained to the arm by dimensions that reference the new spacing, and avoid locking both holes to absolute origin coordinates. Use construction geometry to define the centerline and let the arc slot follow via tangency. Test by changing the 15 mm value to 16 mm and back, verifying that the slot and arm update without error, then restore 15 mm and save.