An assembly records which parts belong together and how they fit

A part defines a component's shape. An assembly places instances of parts and subassemblies and records relationships between them. Two instances of one part can occupy different positions while using the same part definition.

In a file-based SOLIDWORKS assembly, the .SLDASM normally references external .SLDPRT and other assembly files. An assembly drawing references the assembly. Sending only the assembly file can leave the recipient without its components. Virtual components are an exception: their definitions can be stored inside the assembly.

Onshape organizes Part Studios, Assemblies, and Drawings as tabs in documents. Inserted instances reference their source definitions; a tab name is not a Windows filename. Share the document with the appropriate access and identify the intended version when a fixed design state matters.

Supporting detail: Addendum 1 — Definitions, instances, and design changes.

Ground a base, then count the motion you intend to keep

A free rigid component in three-dimensional space has six degrees of freedom (DOF): translation along three axes and rotation about three axes. A degree of freedom is an independent motion, not a count of arrows or mates.

Choose a base or housing as the reference. Fix it, or fully locate it to the assembly origin and planes. In SOLIDWORKS, insertion options include fixing only the first component, fixing inserted components, or leaving them floating. Check the actual state; do not assume that the first component is always fixed. Fixing a base away from the origin holds it there; it does not move it to the origin.

A lever should still rotate about its pivot. A cover should stay put. Fully locating every moving part would turn a mechanism into a rigid model.

Supporting detail: Addendum 3 — Check the insertion setting.

Use geometric mates to describe the intended contact

Select the actual locating faces, axes, or reference planes. The same mate name can accept different geometry, so its effect depends on what you select. The diagrams below are schematic before/after comparisons, not complete constraints for whole assemblies.

Coincident

For two planar faces, put their supporting planes together. The faces can still slide in that plane and rotate about its normal. Coincident planes do not guarantee that finite faces overlap.

Concentric

Put two cylindrical axes on the same line. Without a rotation lock or other mates, a shaft can still slide along and rotate about that line.

Supporting detail: Addendum 4 — Why subtracting one DOF per mate gives the wrong answer.

Parallel and perpendicular mates set orientation

Parallel keeps selected planes parallel without setting their separation. Perpendicular keeps selected planes at a right angle. Neither condition alone fully locates the part. These diagrams show the planes edge-on.

Distance, angle, and tangent mates control gaps and contact

Distance sets a separation between selected entities. For parallel planar faces, use the normal gap, not a slanted edge length. Angle sets the angle between selected entities; check alignment and direction so the model uses the intended side of the angle.

Tangent keeps compatible curved and planar or curved surfaces touching tangentially. Tangency alone does not enforce rolling without slipping.

Choose a joint or mechanical relationship when motion is the point

For a simple lever on a grounded pin, align the pivot axes and locate the lever axially. Leave rotation free. A hinge mate expresses this single rotational freedom directly. In Onshape, a Revolute mate serves that joint purpose; Cylindrical allows axial slide and spin, Slider allows one translation, and Fastened allows no relative motion. Mate connectors establish the joint frames.

A slot mate locates a pin or similar feature relative to a slot. Select free travel or a prescribed position to match the design; other motions depend on the selections and remaining mates. Onshape's Pin Slot mate allows rotation about the connector's Z axis and translation along its X axis. Set appropriate travel limits; it is not an identical set of SOLIDWORKS slot options.

A gear mate or gear relation couples rotations by a ratio. Locate the shafts first. The relation does not create teeth or prove they mesh without interference. Use Gear Ratios for the ratio calculation and Torque for the separate question of turning effort.

Supporting detail: Addendum 5 — Compare vendor joint vocabulary.

Build reusable parts and subassemblies with deliberate dependencies

Bottom-up design starts with existing parts and brings them into an assembly. Top-down design starts with an overall layout or shared design references and develops parts around them. A mixed approach is common: use a shared layout for custom plates and insert purchased hardware.

A subassembly groups parts into a reusable unit. Give it a useful function, such as a pivot cartridge, rather than hiding unrelated parts in it. Check whether its internal joints are allowed to move at the parent level; a rigid subassembly can make a working joint appear locked.

Top-down references can keep mating holes aligned when the layout changes, but they also create dependencies. Keep the direction of those dependencies understandable and check them when copying or sharing the design.

Supporting detail: Addendum 6 — What makes a feature top-down?.

Use SOLIDWORKS Toolbox or Onshape Standard Content, where available, for standard hardware. Choose the standard, size, thread pitch, length, and material or grade deliberately. A visually similar bolt or an automatic size suggestion is not a completed fastener selection.

Supporting detail: Addendum 7 — Library hardware still needs checking.

For sketching and part-modeling topics, browse Engineering Graphics and CAD. Continue with Checking CAD Assemblies and Exploded Views and Bills of Materials.

Practice shaft freedom Choose locating mates

Judge remaining motion against the design intent

A successful rebuild means the CAD system can solve the model. It does not mean the model describes the mechanism you intended. Try moving each component and name the motion that should remain.

Under-mated means freedom remains. That is a defect for a loose cover, but rotation at a lever pivot can be intentional. Over-mated or conflicting constraints ask for relationships that the solver cannot satisfy together. A redundant constraint repeats an existing condition; it adds no useful location and can complicate diagnosis.

For a shaft with concentric axes and seated shoulder faces, one rotation remains. Adding another mate that merely keeps those axes parallel is redundant. Adding an angle mate to lock that remaining rotation may be correct for a stationary shaft and wrong for a rotating lever. Review Assembly Files and Mates for the geometry.

Check interference and clearance as different questions

Interference is shared volume: two solid parts occupy the same space. Clearance is the gap between parts. A model with no overlap may still lack enough room for movement, manufacturing variation, or tool access.

Run interference detection on the relevant components in the intended configuration and position. Inspect each result. An intentional press fit or simplified thread representation can produce overlap, but an unwanted bolt tip inside a moving path needs attention. Record the reason for any accepted interference.

Supporting detail: Addendum 8 — Selection scope can hide an interference.

An exploded view separates parts to explain their relationship

An assembled view shows the working arrangement. An exploded view spaces components apart so the reader can identify them and follow how they fit. The separation is for communication; it is not an operating clearance or a change to the part geometry.

Separate components along understandable directions, keep related parts aligned, and use explode lines where the connection would otherwise be unclear. Preserve the working assembly and create a saved exploded view rather than deleting mates to pull the model apart.

Supporting detail: Addendum 10 — Use the saved view in a drawing.

A balloon finds a BOM row; a part number identifies the component

A bill of materials (BOM) lists the components required for the stated assembly. A drawing balloon points to a component and usually shows its BOM item number. The item number is a row identifier in that drawing's list. The part number identifies the part for reuse, manufacture, or purchase.

Balloon 4 identifies HW-410, not four washers. Its quantity is two per assembly. This list has five distinct rows and six component instances. Repeated instances of the same specified part share an item number; different sizes or variants need distinguishable identities.

Supporting detail: Addendum 11 — Linked tables reduce manual mismatches.

Decide whether the BOM lists units or their internal parts

A top-level list can show a purchased subassembly as one unit. A structured list can show the assembly hierarchy, while a flattened list collects the underlying components without that hierarchy. State the scope before interpreting a quantity. Do not order a complete unit and all its contents accidentally.

Verify part numbers, descriptions, quantities, and relevant configuration or revision information. A library model's filename is not automatically a useful purchasing description. The teaching identifiers above are examples, not an orderable hardware specification.

Supporting detail: Addendum 12 — Subassembly display changes what the table means.