More specifically to what Matt wrote - don't delete these dimensions from the drawing, use Erase.
The dimensions were created in the drawing but with the Configuration setting so that the created dimensions are stored in the model. Ordinarily this isn't noticed because people who Create dimensions would not Show the draft dimensions on other drawings. Because this is a Save-As of the drawing alone, the same model is used in both drawings and the same dimensions (carried in the model) are Shown in the drawings. Deleting a Created dimension stored in the model that is Shown in the drawing deletes the dimension from the Model.
The best approach is to Show dimensions from the Model and never Create drawing dimensions, but PTC hasn't covered the failure mode in Shown dimensions that makes Created Drawing dimensions prized - if a feature is redefined or deleted and replaced, the drawing will not echo the deleted Shown Model dimension, prompting the drafter to fix/account for the change. At least with Created Drawing dimensions the dimension and leaders will remain and change color to show their broken status.
The setting Matt mentions is also useful when the Part/Assembly is Released/Checked-out by someone else/otherwise Locked (That was a nice feature in PTC Intralink that didn't make it to WC Intralink) to prevent the part being changed by the Drawing Mode Created Dimensions being stored in the related Part/Assembly.
One clue to this is that there could have been a prompt that the model was being modified by deleting the dimension, just like there should have been a prompt that the model was being modified when the dimension was Created.
