NX Repairing Parts and Assemblies in NX - Part 5 Conclusion

Errors in Parts and Assemblies, Part  Features out of Date, Poor Performance, etc.

Recommend doing the following, for all parts and assemblies, if there are any error messages, performance issues (slow to open or update), problems working on a part or assembly.

Recommend following this procedure prior to releasing single parts and assemblies to ensure all components and inter-part relationships between components are both up to date and have no errors in them.

1. Single parts;

1.1 Remove all unused features within Part Navigator.

1.2 Run Feature Replay to ensure all features properly update without it stopping prematurely before reaching the end of the last feature within each single part file. (See attached document or online article)

1.3 Run Part Cleanup on the single part file. (See attached document or online article)

1.4 Run Examine Geometry to ensure the body or surfaces within the part file are valid. If not valid manually change them so they are valid. (See attached document or online article)

1.5 For parts with interactive feature changes using Suppression by Expression, Product Template Studio, Part Family, etc. make sure that the smallest and least number of features and also the most or all features and largest body also are tested with steps 1.1 through 1.4.

1.6 Save the Single part file which is now ready for production and assembly use.

2. Assemblies:

2.1 When using Wave links and IPE (Inter-Part Expression) use the Inter-part Link Browser to ensure there are no unexpected broken wave links or IPE's within the assembly as these will not automatically update when both the parent and children are fully loaded.

NOTE: Set File Open Load Options to Partially Load and Load Inter-part Data to All Levels. To automatically update wave links and IPE's it is mandatory to do this or wave links and IPE's will not update.

2.2 Follow the procedure within the attached Repairing Parts and Assemblies in NX11 and later releases.pdf called Update Entire Assembly in Modeling. This may generate a list of feature failures in components which need to be corrected. (See attached document or online article)

2.3 Run Examine Geometry to ensure all bodies and surfaces within the assembly component file are valid. If not valid manually change them so they are valid. (See attached document or online article)

2.4 Save the Assembly which is now ready for production use.

3. Teamcenter PDM users:

NX has a tool called Check-Mate that can be customized to ensure part files meet company requirements for standards, which out of the box include 300 plus functions including all Examine Geometry checks. Only within the Teamcenter PDM a company can set a process to prevent a single part file from being releases for use until it passes all of a company's Check-Mate tests.

Regardless if working within Teamcenter, native Windows or even another PDM, this will not only ensure released parts are now compliant, but help self-direct users to build good quality models which are both valid for manufacturing, but also may reduce actual hard drive size, will improve single and assembly performance when opening, editing, etc.

See articles Parts 1-4

PL8733434

PL8733451

PL8734734

PL8737728