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View Locking in NX 11.0.1


Maintaining data integrity is absolutely critical to the design process. If one item shows different information than another, serious issues can occur, such as manufacturing errors, building incorrect parts, or even warranty and safety problems.


Lock View.png


Drawings can be especially vulnerable to this kind of problem. If a drawing is changed without updating the model, it’s highly possible, even likely, that the change will not propagate to all downstream parties.

NX 11.0.1 helps to prevent these issues by ensuring a drawing view’s content cannot change with Lock View option that prevents any changes to the view content, including view updates. Annotation and location of a view remain enabled.


Use the new Lock Method view setting to lock Exact or Smart Lightweight views and prevent them from updating. You can lock views to prevent model changes or user edits from applying to a view.

There are three levels of locking to a view as:

None - Allows view updates and edits to view content

Snapshot - Disallow view updates but allows edits to view content

Complete - Disallows view updates and edits to view content


Default lock method can be set in the drafting preferences. 

Lock View.PNGNX 11.0.1: 'Lock Method' location in the Drafting Preferences dialog


After locking a view, respective symbol will appear for that view in the ‘Up to Date’ column.

Lock View1.PNGNX 11.0.1: 'Lock View' icon display in the column Up to Date (Part Navigator)

After model update, drawing and unlocked views will be marked as out-of-date in the part navigator. Locked views status will remain unchanged and updating the drawing/views will have no effect on status of locked views. 

Lock View2.PNGNX 11.0.1: Views update status in the Part Navigator after model update


Tooltips are available in the Part Navigator and the graphics window help you identify the locked status of a view. The status line also lists a view's locked status.

Hovering the cursor on icon in the Up to Date column of part navigator will display the tooltip that shows the method used to lock. Tooltip will not be displayed for the views which are not locked.

Also in UI if cursor is hovered over view boundary, it will show the tooltip for all the views irrespective of their lock status.Lock View4.PNGNX 11.0.1: Tooltip information for the view in the Part Navigator


Lock View3.PNGNX 11.0.1: Tooltip information for the view in drawing UI and status bar information

Lock View5.PNGNX 11.0.1: Tooltip information for normal view in drawing UI

Upon changing lock status of views to ‘None’, it will updates on the drawing automatically.