How to remove the IP (Intellectual Property) from the database in Allegro PCB, APD or SiP?

I have a design that I wish to share with someone outside of our company and need to remove our IP before sending the design out. Modifying the netlist manually to have generic names and importing it into the design does not work cleanly.  Is there an easy way to remove design IP?

Starting SPB17.2 the Strip Design option can be found in File > Export >Strip Design. 

In SPB16.6 an environment variable unsupported_strip_design can be set to enable the Strip IP design capability in the File > Export menu. Use the User Preferences Editor (Setup — User Preferences) to set the variable located under the Unsupported folder.

Note that this may not clear a design of ITAR restrictions. You should still consult your ITAR compliance manager.

The PCB Editor menu selection, File > Export > Strip Design (strip_design command) invokes the following UI which allows you to define the item(s) which are modified or deleted.

Note :-  For the Packaging tools (APD/SiP), the option is presently not available under File > Export. Users need to type the command strip_design at the Command line.

          Command > strip_design

In the General tab the following items are either modified or deleted.

• Net, bus, diffpair, xnet, match group and net class names renamed. The renaming methodology replaces names with CDN_<number> where <number> is a unique number. Use the Prefix to New Name field to set a prefix to something other than the default CDN
• Part names, devices, packages, component (instance and definition) and module renamed.
• Delete text that is part of symbols as long as it is NOT refdes or pin numbers.
• All user defined properties including their definitions deleted.
• Logical path (LOGICAL_PATH) and Physical path (PHYSICAL_PATH) property instances deleted.
• LIBRARY_PATH property instances deleted.
• Constraint manager based view attachments deleted.
• Produce a was-is file for objects that are renamed.

Selecting the Save Configuration button will store the selected options in a configuration file that can be stored at a central site location.

The Optional Delete tab has the following items (removing these items may impede Cadence's ability to debug the issue.):

• All user defined subclasses with associated data deleted.
• Delete text associated with design root (eliminates all notes etc.)
• All format symbols deleted.
• All constraint data deleted.
  • Electrical
  • All other (including DFA)
• Attached signal models (if present).
• Delete SI multi-design configuration data (if present).
• Reset cross-section parameters to defaults.
• Delete constraint manager advanced constraint attachment (if present)
• Delete items on layers not currently visible.
  • If any part of a symbol is visible the entire symbol is kept
  • Selecting this item disables delete by net option
• Net selection UI to delete all items except for selected nets.
  • Symbols are kept only if they have pins associated with the selected nets.
  • Selecting this item disables delete except for visible option.