In top-down assembly design, one or more features of a part are defined by something in an assembly, such as a layout sketch or the geometry of another part. The design intent (sizes of features, placement of components in the assembly, proximity to other parts, etc.) comes from the top (the assembly) and moves down (into the parts), hence the phrase "top-down."
For example, when creating a locating pin on a plastic part using the Extrude command, you might choose the Up to Surface option and select the bottom of a circuit board (a different part). This selection would make the locating pin exactly long enough to touch the board, even if the board were moved in a future design change. Thus the length of the pin is defined in the assembly, not by a static dimension in the part.
You can use some or all of these top-down methods:
Individual features can be designed top-down by referencing other parts in the assembly, as in the case of the locating pin described above. In bottom-up design, a part is built in a separate window where only that part is visible. However, SolidWorks also allows you to edit parts while working in the assembly window. This makes all of the other components' geometry available to reference (for example, copy or dimension to). This method is helpful for those parts that are mostly static but have certain features that interface with other assembly components.
- Complete parts can be built with top-down methods by creating new components within the context of the assembly. The component you build is actually attached (mated) to another existing component in the assembly. The geometry for the component you build is based upon the existing component. This method is useful for parts like brackets and fixtures, which are mostly or completely dependent on other parts to define their shape and size.
An entire assembly can be designed from the top down as well, by first building a layout sketch that defines component locations, key dimensions, etc. Then build 3D parts using one of the methods above, so the 3D parts follow the sketch for their size and location. The speed and flexibility of the sketch allows you to quickly try several versions of the design before building any 3D geometry. Even after you build the 3D geometry, the sketch allows you to make a large number of changes in one central location.
- Whenever you create a part or feature using top-down techniques, external references are created to the geometry you referenced.
- In some cases, assemblies with large numbers of in-context features (which form the basis of top-down design) can take longer to rebuild than the same assembly without them.
SolidWorks is optimized to rebuild only parts that have changed.
- When creating in-context features, it is important to not create mating conflicts because they can cause long rebuild times and unexpected geometry behavior. You can generally avoid these conflicts by not creating mates to geometry created by in-context features.