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"External" and "defined-in-context" references are SolidWorks features that allow designers to reuse existing geometry to insure parts fit together during the entire product life cycle.
An "external" reference is created when a sketch entity is related to something external to the sketch. Dimensioning to existing geometry or offsetting an edge within the active file will create an external reference.
A "defined-in-context" reference refers to the creation of an external reference in the context of an assembly. This is done by using the Edit Part function while in the assembly.
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Design challenge: create a rubber gasket that fits on top of the existing engine case assembly
The sketch geometry for the washer references the case holes and needs to have .5 mm clearance to the main boss.
The designer working on the part thinks there may be a change, but he does not know when it will occur in the design process.
If the feature dimensions change, the gasket must move with the new design. When the designer releases the tool, the references should no longer automatically update.
This is a good case for creating in context references. The gasket geometry will reference the holes in the case and update when the case geometry changes. The update requirement can be handled using the Lock Reference function.
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| Final design |
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| Existing design |
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A good place to start this design would be to create a simplified configuration of the existing assembly.
This is done for the following reasons:
- Minimize visual clutter – when more parts are shown within the assembly, it becomes more difficult to locate what you need
- Performance – with less geometry to update, the assembly will perform better
- Minimize unwanted references – when creating external references, you want to ensure the correct geometry is referenced. If the wrong geometry is selected for the referenced, this may cause obstacles later in the design
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| Simplified configuration |
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Editing the part within the context of the assembly means opening a part using the Edit Part function from inside the assembly.
The part will display with a unique color as shown in the diagram. The rest of the assembly is shown in gray.
References can be made in relation to any assembly component. Once the references are complete, the part can be opened and edited without the assembly open. SolidWorks also has the option to edit the external reference in the context of the assembly. This option will open the assembly and the part in edit part mode.
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| Edit part |
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Parts that have external references are denoted within the FeatureManager with the "->" symbol.
The feature that was created with the reference and the overall part icon will both display the symbol. The part may also have multiple features with external references.
To view or modify the reference, select the feature, press the right mouse button and select List External References.
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| Feature manager |
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The external reference dialog box allows the user to see and modify the external references within the part. This dialog box also offers additional information on the features used for the reference and the ability to lock or break the relationship(s).
"Lock" and "break" references are functions that can be used to control the reference geometry. Break allows the reference to be permanently removed from the model. No further reference is made to the original geometry.
Lock allows the reference to be frozen. If the original geometry changes, the in context geometry will not update. The advantage of lock is two-fold - the new geometry does not update unless a user unlocks the reference and the references can be restored (unlock).
The practice of locking all external relations on a part ready for release means the geometry will never update without unlocking the relationships first. If the relationship is no longer meaningful, then the Break All function can be used to remove the relationship permanently.
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Beware of in-context references in which the same subassembly appears but with different values (see example to right).
To overcome this challenge:
- Use different components. Break the sub-assembly into two different parts.
- Do not use in-context references for this condition.
- Use the ability to suppress sketch relations (SolidWorks 2001Plus) and specify specific configurations when creating the geometry. Have two construction circles in the hex part and use sketch relations to drive the in-context feature.
See the SolidWorks Knowledge Base Log ID: 92280 for a more complete description of this limitation.
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| subassembly configuration |
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| Two subassembly configurations used in the same assembly |
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The power of external references and in-context features offers the designer the ability to shorten design cycles and improve the quality of the work. The key is to understand why and where they were created and control the state - locked, automatic update - of the relationship.
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