Understanding Parent/Child Relationships

One challenge that many users face is how to create parts that are intelligent in nature. An intelligent part is one that can be modified allowing you to change or remove features without causing other non-related features to fail. One reason a part will fail is when a feature is removed or changed and a seemingly non-related feature fails. This could have been caused by an unwanted parent-child relationship.

A parent-child relationship is created when:

• Selecting a sketch plane or face
• Re-using model geometry with a sketch (Convert or Offset)
• Dimensioning to existing model geometry
• Establishing relationships to existing geometry

There are a number of techniques that can be used to avoid creating unwanted references. The first is creating a part with the most important feature created early within the design (i.e., near the top of the FeatureManager). The reason this creates a more robust part is that the more important features are less likely to be change or removed. The features of lesser importance can be removed more readily if they are closer to the end of the design (i.e., near the bottom of the FeatureManager).

If a feature of lesser importance is created early within the design process, there is a higher probability that the feature could be referenced, intentionally or not, by another feature. If the feature is created later in the part design, there is less chance the feature could be referenced inadvertently.

When creating references it is always preferable to reference simple entity types. Axes, points, and planes are the simplest type of entity and are more robust in name than any other type of entities due to the simplicity of the object.

Another method that can be used to make your design more readable and robust is group features by function. For example, if a mounting boss is made up of several design features; it makes sense to create those features together. This makes modification easier because you do not need to hunt for the features used to create that function (i.e., mount boss) with the FeatureManager Tree.

It is debatable whether the non-design element features (i.e., fillets, draft, chamfers) should be included within the functional group. The advantage of using a plane or axis is that the feature can be named and reused by a number of other features. For example, if a bicycle frame references the sprocket axis, an axis can be inserted and all features within the other components could reference the axis.

A common practice when creating a new feature within a design is to select the sketch plane and start the sketch. A better practice is to review the function of the feature and determine where it should be created within the FeatureManager Tree. This is determined by the location of related features, and the overall importance of the feature being created.

Use the rollback bar to select the desired placement of the new feature prior to creating the feature. This will do two things; the feature is in a functionally grouped location within the FeatureManager Tree and the number of features shown within the graphics display is minimized. This means the part is rebuilt faster and there is less chance of selecting unwanted geometric reference when sketching the new feature. After the feature has been inserted, the rollback bar is dragged back down to the bottom of the FeatureManager Tree and the entire model is re-displayed. Rollback can be used to determine design intent and how the part was built.

The following are sketch tips to help minimize unwanted relationships:

• Exercise your sketches: change your sketch to review whether the changes made were as intended. Before adding dimensions, drag the sketch entities to insure they are constrained in the desired manner. Create sketch geometry with the correct general shape but not the size. Then when dimensions are placed on the geometry, the final dimensions change the size of the sketch. The manner in which the changes took place can also give clues to how the geometry was constrained.
• Rotate the part to insure the selection of the intended model reference.
• Review the relationships created within the sketch.

By using the following techniques, the amount of unwanted parent-child relationships can be minimized, and the part design is easier to understand and modify:

• Feature order based on importance
• Functionally grouping like features
• Reference simple entity type when possible
• Use rollback to minimize model complexity and functionally group like features

Category: Modeling

Written to: SolidWorks 2005