Assemblies · Lesson 1
SOLIDWORKS assembly basics
An assembly is a file (.sldasm) that places parts relative to each other. It does not copy the parts — it links to the part files and stores their positions and the mates between them. The first part you insert is usually fixed at the origin; every other part floats with six degrees of freedom until mates take them away.

Where to find it
File → New → Assembly; Assembly tab → Insert Components
Tree symbols
| Symbol | Meaning |
|---|---|
(f) |
Fixed — cannot move |
(-) |
Under defined — can still move |
(+) |
Over defined — conflicting mates |
| (none) | Fully defined by mates |
Moving components
| Action | How |
|---|---|
| Move | Left-drag a face (moves in the plane of the view) |
| Rotate | Right-drag |
| Exact move | Move Component: along XYZ, along an entity, by delta, to a position |
| Exact rotation | Rotate Component: about an entity or by delta |
| Free a fixed part | Right-click → Float |
Move Component also has collision detection (stops at contact) and dynamic clearance. Positions set by dragging are not stored as rules — mates are. Next: standard mates.
Step by step
-
1
Model the parts
Make two parts and save them: a plate 100 × 60 × 10 mm with two Ø10 through holes, and a pin Ø10 × 30 mm.
-
2
Start the assembly with the plate
File → New → Assembly. In Begin Assembly pick the plate and click the green tick — the plate is placed at the assembly origin and fixed. It shows (f) in the tree.

The green tick places the first component at the origin and fixes it. -
3
Insert the pins
Assembly tab → Insert Components, pick the pin and click in the graphics area to drop it — do not use the green tick, or it is also fixed. Insert it a second time. The pins show (-): they can still move.
-
4
Move and rotate them
Left-drag a pin to move it; right-drag to rotate it. For exact moves use Move Component (along XYZ, by delta, to a position).
-
5
Save and package
Save the assembly in the same folder as the parts. To send it to someone, use File → Pack and Go, which collects the assembly and all its part files.
Common mistakes
- Clicking the green tick for every component — each one is then fixed at the origin and cannot be mated.
- Fixing a component that already has mates, which causes mate errors. Float it, or delete the conflicting mates.
- Sending only the .sldasm file. Without the part files the assembly opens empty — use Pack and Go.
- Renaming part files in Windows Explorer, which breaks the links. Use the SOLIDWORKS rename tools.
Lesson 1 of 16 in the assemblies course.
Practice
Insert the plate (fixed) and two pins (floating). Check: Evaluate → Mass Properties on the assembly gives 63,141.59 mm³ (plate with two holes 58,429.20 + two pins 2 × 2,356.19), whatever the pin positions — mass properties do not care about overlaps. Mate the pins in the next lesson.
Sources
- Hawk Ridge — Assembly user interface overview (Mar 2022)
- GoEngineer — Introduction to SOLIDWORKS mates (Feb 2022)
- GoEngineer — Fixed vs floating components (Apr 2024)
- Javelin — How to use Move Component (Mar 2026)
- GoEngineer — Pack and Go: what it is and how to use it (Feb 2026)
- Javelin — Why is SOLIDWORKS unable to locate my components?
- SolidProfessor — SOLIDWORKS 2015 assemblies
Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.
Frequently asked questions
How do I start an assembly in SOLIDWORKS?
+
File → New → Assembly. The Begin Assembly PropertyManager opens; pick a part and click the green tick to place it fixed at the origin.
What does (f) mean in an assembly?
+
The component is fixed: locked in all six degrees of freedom. (-) means it can still move, and (+) means it is over defined.
How do I unfix a component?
+
Right-click it in the FeatureManager tree and choose Float. Then add mates to position it.
Does an assembly file contain the parts?
+
No. It references the part files and stores positions and mates, so the part files must travel with it — Pack and Go collects them.
Related
- SOLIDWORKS standard matesHow to use SOLIDWORKS standard mates: coincident, parallel, perpendicular, tangent, concentric, lock, distance and angle, Quick Mates and lock rotation.
- What is an SLDASM file?An SLDASM file is a SOLIDWORKS assembly that references its part files. Why it opens with missing parts, how to send it with Pack and Go, and how to convert it.
- SOLIDWORKS missing references — unable to locate fileSOLIDWORKS "unable to locate file" when opening an assembly or drawing? How the search order works, how to repair references, and how to rename files safely.
- SOLIDWORKS subassembliesHow to create subassemblies in SOLIDWORKS from selected components, save virtual ones, make them flexible or dissolve them, and why they speed things up.