Chapter 16: Modeling in Context
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 I 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-con-
text references, the best way to respond to them is to break them immediately. However, I would
argue that using the Break References function is never a good thing to do. I believe that you
should remove the reference by editing the feature or the sketch or change it to make it useful.The problem with a broken reference is that it has absolutely no advantage over a locked reference.
For example, while locked references can at least be unlocked, broken references cannot be
repaired. The only thing that you can do with a broken reference is to use Display/Delete Relations
or to manually edit features to completely remove the external reference. Perhaps it would be bet-
ter for SolidWorks to replace Break References with a function called Remove References. Would
anyone like to make an enhancement request?Best Practice
Best practice is to not put yourself in a situation where you are using broken references. Parametric relations
should not change if the driving geometry does not change.
You cannot selectively lock or break external relations. For example, all the external relations in the part can
be locked, all the external relations can be broken, or none of them can be locked or broken. If you need to
selectively disable relations, then you should consider suppressing features, sketch relations, end conditions, or
sketch planes. n