Best practices – Pro/ENGINEER

Check your models before migration Before you migrate parts with features from Pro/ENGINEER to NX, check that the model can be properly regenerated in Pro/ENGINEER. To check the models, use the Pro/ENGINEER command Analysis→ModelCHECK→ModelCHECK Regenerate. If features can not be regenerated properly in Pro/ENGINEER, they will not be migrated successfully to NX. Parts As you migrate from Pro/ENGINEER to NX, most of your high-level practices for creating parts, assemblies, and drawings will also be good practices in NX because many of the general concepts of associativity, datums, features, parameters, sketches, and sketch constraints are similar. On the other hand, the danger of mapping all of your practices to similar practices in NX is that you may miss the opportunity to use new functionality in NX. Check that the migrated model uses the most efficient modeling techniques. Datum features Pro/ENGINEER datum planes are migrated to the equivalent NX datum planes. The size of these datum planes may not be initially sized properly in NX. To resize datum planes, right-click a datum plane feature in the Part Navigator and select Resize Datum Plane. The Datum CSYS feature is not the same in Pro/ENGINEER and NX. If possible, consider creating a new Datum CSYS feature in NX. Reorder this feature to the beginning of the history. As you make changes, position features and sketches relative to this Datum CSYS. Chapter 10: Migrating Pro/ENGINEER data

Migrating Pro/ENGINEER data Sketches When you edit a migrated sketch, carefully consider the design intent reflected in the dimensional and geometric constraints. It is possible that even though the sketches have migrated properly, constraints that were inferred in Pro/ENGINEER are not inferred the same way in NX. Since NX does not use strong and weak constraints, some Pro/ENGINEER constraints may be migrated as conflicting constraints, overconstraining the sketch. Delete redundant dimensional constraints. Minimize the number of dimension constraints by using NX geometric constraints instead; such as equal length, equal radius, collinear, coincident, and midpoints constraints. Reference curves from Pro/ENGINEER are mapped to NX reference curves, which are not identical. These curves may appear as very long NX reference curves with points at the ends. Replace constraints to these long reference curves in sketches with other constraints directly to datums or other part geometry. Then delete these long reference curves. Delete the unconstrained points at both ends of the migrated reference curves. Each unconstrained point will introduce two unconstrained degrees of freedom in the sketch. Features When a migrated model is edited, this is the time to review the modeling methods. Make sure that the model captures your design intent when parameters are modified. Even when model geometry and features have migrated correctly, the model might not accurately capture your design intent such as symmetry. Other options may be available in NX, such as the Offset option on Extrude features. Do not confuse hide with suppress. Hide only removes objects from the display. Suppress makes them inactive in the history. Suppress features by clearing the green check mark in the Part Navigator. Migrating Pro/ENGINEER data

Migrating Pro/ENGINEER data Assemblies Use the Assembly Navigator to investigate the assembly structure. To work on a specific part in an assembly, make it the work part in the assembly, or make it the displayed part. Use the Part Navigator to investigate the features in the assembly work part. View assembly constraints in the Constraint Navigator. Drawings After migrating drawings, use the NX Drawing Comparison Tool in the Drawing Migration toolbar to compare the original drawing to the migrated drawing. Family tables By default, family table generics are migrated with features; any instance of a family table that is referenced by an assembly is migrated as a B-Rep part. All instances will have the correct location in their respective assemblies. For parametric migration of family tables, the generics need to be migrated first and then NX instance equivalents need to be created along with a mapping file. When a Pro/ENGINEER family table instance is found in an assembly, the new NX part is swapped for the instance B-Rep, giving the user a parametric NX part family member. Chapter 10: Migrating Pro/ENGINEER data