Assembly reference geometry in soliswoks

Planes and axes are frequently created within assemblies to drive symmetry or placement of parts. You can use assembly layout sketches to create the reference geometry entities. When you create reference geometry within the assembly in this way, be aware that the normal history-based parent/ child relationships are still followed. The familiar icons for reference geometry entities are also used in the assembly tree.

History-based and non-history-based portions of the assembly tree

Because features such as sketches and reference geometry are history based and found in the assembly tree, at least a portion of the assembly FeatureManager is history based. However, not all of it is. For example, the list of parts and subassemblies is not history based.

Sketches and reference geometry may appear before or after the list of parts, subassemblies, and mates. All the remaining entity types that can be found in the assembly FeatureManager are also history-based features, and you can reorder them in the tree. However, several situations can disrupt the process. Under normal circumstances, sketches and reference geometry at the top of the assembly FeatureManager are solved, then the parts are rebuilt if required, and then the mates. This ensures that the sketches and reference geometry are in the correct locations so that if parts are mated to them, all the components end up being the correct size and in the right position.

Assembly-level reference geometry can be created that references component geometry instead of layout sketches. This creates a dependency that changes the usual order. For example, the planes are usually solved before the part locations, but when the plane is dependent on the part location, the plane has to be solved after the part. If a part is then mated to the plane, you are beginning to create a dependency loop, such that the plane is solved, followed by the part, then the plane again because the part has moved; and then the mate that goes to the plane has to resolve the part.

Best Practice

If you are a bit confused by all of this, don’t worry. You can simply follow this rule: Do not mate to anything that comes after the mates in the assembly FeatureManager tree. This includes assembly planes or sketches that are dependent on part geometry, assembly features such as cuts, in-context features, component pattern instances, Series Holes, or Smart Fasteners.

This is probably a lot of information if you are a new user, but if you remember this rule, you can avoid creating models with circular references, where A is dependent on B, which is dependent on A — a neverending loop that causes major problems for large assembly rebuild times.

Parts and subassemblies

Parts and subassemblies are shown with their familiar icons in the design tree. You can reorder and group them in folders, which is covered in the next section.

Parts are sometimes shown with a feather, which indicates a lightweight part, and assemblies can have an icon that indicates a flexible subassembly.

Special icons also exist for hidden and suppressed components.


You can create folders to organize and group both parts and mates. I discuss this technique in detail later in this chapter.


The Mates area remains a constant, single folder, but you can organize it by reordering the mates and grouping them into folders. Each mate is shown with a symbol corresponding to the type of mate it is, but the mate folder is shown as a pair of paperclips.

Assembly features

In manufacturing, once parts are assembled, secondary machining operations are sometimes applied to them to ensure that holes line up properly, or for other purposes. For example, assembly features can be cut extrudes, cut revolves, or hole features. These features appear only in the assembly, not in the individual parts.

You should not confuse assembly features with in-context features. In-context features are created when you are editing a part in the assembly with a reference between parts, but the sketch and feature definition are in the part itself.

Component patterns and mirror components

Component patterns can pattern either parts or assemblies by creating either a pattern defined in the assembly, or a pattern that follows a pattern feature created in a part. The pattern is listed as a feature in the assembly FeatureManager, and all the instance parts appear indented from the pattern feature in the design tree.You can hide or suppress each instance, change its configuration, and in most ways control it as if it were a regular part in the design tree.

Because the options for locally defined patterns are comparatively limited, users generally like to use part feature patterns to drive the component patterns when possible.

Component patterns are listed at the bottom of the assembly FeatureManager with a set of components under a LocalPattern icon. The component instances under the LocalPattern can be controlled in several ways, including assigned configurations, colors, and display states. The pattern can even be dissolved, leaving the components, but dissolving the intelligent pattern that places them.

Mirror components are revamped in 2010 and are also listed under a special MirrorComponent icon after the mates.


To improve performance, it is best to pattern subassemblies if possible. If it is not possible, then patterning a group of parts is the next best option. Making multiple patterns, one for each part, is an inefficient way to accomplish the same thing.


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