SolidWorks 2011 Assemblies Bible - Matt Lombard [90]
FIGURE 10.12
Indicators that you are editing a part in-context
Probably the most common mistake you can make with in-context editing has to do with editing the part versus editing the assembly when you add a sketch. If you intend to add a sketched feature to a part in the context of an assembly, but you fail to switch to Edit Part mode before creating the sketch, then the sketch ends up in the assembly rather than the part. You can only do limited things with a sketch in an assembly. Likewise, if you intend to make an assembly layout sketch, but you do not switch out of Edit Part mode, you end up with a sketch in a part that cannot do what you want it to do.
Fortunately, SolidWorks has added a remedy for the first situation. When you make a sketch in the assembly but need to make a feature in the part, you can choose the Propagate feature to parts option in the Feature Scope area of the PropertyManager for the feature, as shown in Figure 10.13.
Notice in the image on the right that the last sketch in the part appears as derived. This means that the sketch and the feature are still driven from the assembly, but they have been propagated to the part enough to allow the feature to be edited in the part. You may not want to go this route just because you made a mistake and it's simpler to do this than to move the sketch to the part, but it is an option that is valid in some situations. Interestingly, this feature cannot be deleted from the part; you must delete it from the assembly.
External reference symbol
The external reference symbol appears as a dash followed by a greater-than sign (->). External references indicate more than just in-context features. You can also create external references by using the Split Part command as well as the Insert Part (base or derived part) or the mirrored part functions. Figure 10.6 shows the expanded FeatureManager for a part with an in-context reference in a sketch.
FIGURE 10.13
Propagating an assembly feature to the part
External references can have four states, as shown in Figure 10.14. These are In-context (->), Out-of-context (->?), Locked reference (->*), and Broken reference (->x).
FIGURE 10.14
The in-context “->” symbol on Extrude1 and Sketch1
• In-context (->). The in-context symbol signifies that the relation created between two parts within the current assembly is fully resolved. It can find both parts involved in the relationship and the assembly where the relationship that was created is active.
• Out-of-context (->?). Out-of-context means that the document — usually but not necessarily an assembly — where the reference was created is not open at the time. It is indicated by an in-context symbol followed by a question mark. You can open the document where the reference was created by clicking the right mouse button (RMB) and selecting the Edit In Context option from the menu. Edit In Context opens either the parent part of an inserted part or the assembly where the reference was created for an in-context reference. When you open the referencing document, the out-of-context symbol changes to the in-context symbol.
• Locked reference (->*). You can lock external references so that the model does not change, even if the parent document changes. The symbol for this is ->*. Other features of the part may be changed, but any external reference within the part remains the way it is until the reference is either unlocked or removed. In the top and base example mentioned earlier, this means that if the Bottom part is changed, and the external reference on the Top is locked, then the Top will no longer fit the Bottom.
One of the best things about locked references is that you can unlock them. They are also flexible and give you control over when updates take place to parts with locked references.
• Broken reference (->x). The broken reference is another source of controversy. Some users believe that if you make in-context references,