Suggested Technique for Managing Parent-Child Relationships in Pro/ENGINEER Wildfire 3.0

When working in Pro/ENGINEER you may find you need to manage parent-child relationships in order to control features in a model. The ability to remove and create different parent-child relationships in Pro/ENGINEER models is an invaluable tool to the novice and expert alike. Determining the type of relationship and how to break it is important for reordering, redefining and rerouting features, as well as maintaining desired associations between components and parent assemblies.

1. To manage parent-child relationships, you must first decide what needs to be changed. Figure 1 shows a rectangular cut in a block which is supposed to be placed on face B instead of A. Instead of deleting this feature, which may have many children, the cut's references will be re-established.
   
   
2. Once the desired change has been isolated, the second step is determining the type of relationships and the resulting technique(s) available to control them. To see the references (from the parent features) of a feature in a model, click Info > Parent/Child and select the feature to find its references. Figure 2 shows a sample of the REFERENCE INFORMATION WINDOW dialog box displaying the references for the cut in the block.
   
   
3. As each reference is selected in the dialog box, the screen will highlight the entity used to create the reference. In the case of the cut, the protrusion reference highlights face A, which is the chosen sketching plane for the feature. The remaining references are for orienting and locating the section to the existing geometry. Most are from Sketcher during section creation and are therefore either dimensioning or alignment references.
   
   
4. After determining what references exist, how the references are going to be managed must be determined.
   
   
5. For the cut feature, the sketching plane controls the direction of the feature so this reference must be modified. The below table lists the most common methods for creating parent-child relationships. Most parent-child relationships can be managed through Edit > References or Edit > Definition.
   
   
6. Edit > References breaks the parent-child relationship by letting you change feature references. Pro/ENGINEER checks the reference of features to determine if the new reference and the old reference are compatible. If the references are not compatible, Pro/ENGINEER issues a warning message and continues processing.
   
   
7. Edit > Definition allows you to change how a feature is created. The types of changes you can make depend on the selected feature. For example, if a feature was created using a section, you can redefine the section, feature references, and so on.
   
   

   Creating Parent/Child Relationships in Part Mode	Creating Parent/Child Relationships in Assembly Mode
   Selecting the sketching plane	Selecting component placement references
   Selecting the orientation plane	Creating a component using Insert > Component > Create... > Mirror
   Creating a dimension in Sketcher	Creating cutout and merge features Edit > Component Operations > Merge
   Aligning an entity in Sketcher	Creating data sharing features Insert > Shared Data
   Using Sketch > Edge > Use... or Sketch > Edge > Offset... in Sketcher	Creating part features in Assembly mode
   Creating concentric circles/arcs
   Selecting a depth reference
   Creating data sharing features Insert > Shared Data

   
   
   
8. As seen above, the sketching plane can be modified by selecting the cut feature, then clicking Edit > References or Edit > Definition.
   
   
9. Select the cut feature, then click Edit > References. The REROUTE REFS menu appears. Click Reroute Feat > Done/Return. The option to roll back the model appears. The model can roll back to when the feature being rerouted was created. All features after the rerouted feature are no longer available for referencing. Choose "No" to rolling back the model. Each feature reference is then highlighted on the screen. The option to select an alternate reference or keep the existing reference is available for each. For the cut, the first reference is the sketching plane. Click Alternate when face A is highlighted and select face B as the new reference.
   
   
10. It is important to be aware of all the feature references during rerouting. For example, if face B is now chosen as the sketching plane then the orientation plane must also be appropriate. Since the top of the block would be a valid orientation plane for both face A and B, that reference does not need to be changed when the sketching plane is changed. When the top surface is highlighted, click Same Ref. If face B had been chosen as a Left orientation plane when the feature had been placed originally, then the orienting plane would need to be rerouted along with the sketching plane (the sketching and orienting planes cannot be the same).
    
    
11. Additionally, dimensioning and alignment references created in Sketcher must be rerouted to new references that correspond to the new sketching plane. In this example, the cut was dimensioned laterally from surface B to locate it, but if surface B is the new sketching plane then the surface opposite A would be the new dimensioning reference to be rerouted.
    
    
12. When face B is highlighted as the dimension reference, click Alternate and select the surface opposite A. Click Okay for the direction to complete the rerouting of the feature.
    
    
13. Figure 3 shows the resulting rerouted feature. Note that these relationships are established any time an entity is selected from geometry on the screen. For example, suppose a protrusion was created in a part while in Assembly mode. The Sketch > Edge > Use... functionality was used to define a closed loop while in Sketcher. At the time of feature creation, a dimension was not needed to define the section and it was driven by existing geometry in the assembly. This external reference (external because the reference resides in the assembly and not the part in which the feature resides) creates a parent-child relationship between the assembly and the part. If the assembly is not in memory, that protrusion will not change its geometry and will be 'frozen' in its last regenerated state.
    
    
14. Supposing the design intent changes and the protrusion now must have its own dimensioning scheme. Edit > Definition should be used to remove the references to the assembly and to create the new dimensions.