Why did an Altium impedance-profile change leave the old routing limits?

Check the actual stackup values first: copper thickness, dielectric thickness and the material parameters agreed with the fabricator. Then refresh the relevant constraint data and inspect minimum, preferred and maximum widths together. A new preferred value outside the existing limits is an inconsistent rule. Save the constraint changes so the router can use them; a visible edit is not necessarily an applied edit.

Inspect the specific net or differential pair as well as its class. A more specific assignment can explain why one connection behaves differently from its neighbors. Also confirm the active routing layer and associated impedance profile. Keep a short test track on a copy of the board and inspect the applicable rule, rather than inferring rule selection only from the width shown in a toolbar.

Send the revised stack and nominal geometry back to fabrication for confirmation, including the required tolerance. A field-solver estimate depends on its material and geometry assumptions. Review already routed tracks separately; changing a rule does not mean every existing segment has been corrected. Run DRC, inspect affected nets and regenerate the release documentation after the stack and rules are settled.