How to Renew NX Sketches using ‘Renew Feature’ in your latest NX update

When the new sketch is enabled, modifying previous legacy sketches are possible but a renew action may be required. If only dimensional expression value changes are required, a renewing action is not necessary. However, if sketches require any type of reattach, curve manipulation, or what is now known as relation changes, the sketch must be renewed. Basically, almost any modification other than dimensional value changes require a renew. Once a sketch is renewed, the sketch can utilize the new solver and upgraded functionality.

A Renew shortcut is available when attempting to modify a legacy sketch using a double-click action. A message appears with the ability to Renew and Edit as an option. If utilized, the sketch is renewed and then activated to make changes right away.

When several sketches are to be renewed, or an edit is not currently necessary, Menu > Edit > Feature > Renew Feature can be used. The Renew Feature function is not new as it was introduced back in NX11 to renew several feature types. Previously renewing sketches was not supported but now is supported because of the new sketch. The Renew Feature only allows one feature to be selected at a time, but overall it is still faster when several sketches are to be renewed.

After a sketch is renewed, some legacy may remain which can be addressed manually if desired. Expressions, unnecessary persistent relations (formerly known as geometric constraints), and colors are areas that may require additional actions as follows:


Start by opening the part file and double click the first sketch. The Edit Legacy Sketch message appears with two edit options to proceed.

Start by opening the part file and double click the first sketch. The Edit Legacy Sketch message appears with two edit options to proceed.


If you are ready to convert the sketch simply select Renew and Edit. The sketch takes a few moments to renew and to fully activate. The floating scene bar at the top contains relation symbols allowing you to easily recognize and apply them if necessary.


Some legacy remains after the renew process and you will notice dimensions appear with p#’s. New sketches no longer automatically create expressions per dimension. Expression with a p# indicate an expression exists. To remove the expressions, group select all dimensions, right-click and select Add/Remove Expression.

Dimensions remain but no longer are the expressions present.


Another legacy condition that remains are the original geometric constraints which are considered persistent relations. Toggle on Display Persistent Relations.

The symbols appear like the old legacy sketch.


Many common persistent relations are no longer required as the solver will automatically find common relations. Therefore, to make the former legacy sketch more modern, several of the persistent relations can be removed. Select Menu > Tools > Persistent Relations Browser. Activate Relations and use Shift and Ctrl to multi-select several relations.

Choose all CoincidentEqual RadiusHorizontalPerpendicularTangent, and Vertical Relation listings. (Do not select dimension listings.) Right-click > Delete when all are selected.

Close the dialog when complete. Notice the sketch status remains fully defined even with the relations removed.


The last remaining legacy aspect is about appearance. The colors used by the sketch remain the previous settings. Colors do not update with a renew. To update the colors, select Task > Preferences gallery > Sketch PreferencesOK the message if it appears.

(The message is identical to the previous sketch. If settings within the Sketch Settings tab are to be changed, they will not change for the current active sketch. In our case, colors will be changed within the Part Settings tab and therefore is not an issue.) Upon selecting Part Setting tab, the legacy colors are shown. Select Inherit from Customer Defaults to update the colors. The curves color should be black when complete.

(If your company has modified customer default colors, the colors in fig. may not match.)


Ok the Sketch Preferences dialog and the sketch colors update.

No actual sketch edits will be performed. Select Finish to complete the sketch.


As the sketch is renewed and finished. The Part Navigator shows the sketch just completed as the current feature. The Renew functionality made the sketch current and does not return the last feature as current. For now, leave as is.

In this case, the part file contains two more sketches to be renewed. This time select Menu > Edit > Feature > Renew Feature. The Renew Feature dialog lists all renewable features and what feature version they derived from.


Set the Sort type to Feature Type and expand Sketch. Both remaining sketches are listed and must be renewed. Only one feature can be renewed at a time.  Select one sketch and then ApplyOK the message.

Repeat for the other sketch. When complete the list no longer lists sketches. (If a feature is not listed, the feature is already renewed.)


Cancel the Renew Feature dialog to exit. Once again, the Renew feature keeps the last renewed feature current. Select the cell in the Current Feature column for the last feature to make it current.

The actions to remove expressions, persistent relations, and color changes are not required and will not be performed again on the last two sketches.

The activity is now complete.

For more tech tips and in-depth eLearning for NX Sketchers, including new courses on other design solutions, please visit to explore more information. There are subscription plans to get access and started on your upskilling journey! If you should have any questions, please reach out to for help.

Leave a Reply