CATIA V5 Assembly: The Basics and Beyond
CATIA V5’s Assembly Design workbench (Product Structure and Constraints) is designed for large, complex assemblies — the kind that automotive OEMs and aerospace primes build routinely. The constraint system is robust, the clash detection tools are powerful, and the performance on large assemblies is better than many competitors when managed correctly.
This guide covers constraint types, degrees of freedom management, clash detection workflow, and the practices that keep large assemblies from becoming unusable.
Constraint Types and When to Use Each
Coincidence (Coïncidence)
Forces two geometric elements to coincide: point-to-point, line-to-line, axis-to-axis, or plane-to-plane. This is the most fundamental constraint. For cylindrical assemblies, a coincidence between two axes aligns a shaft inside a bore — it removes two translational and two rotational degrees of freedom, leaving one rotation (the shaft spinning in the bore) and one translation (axial position).
Axis coincidence is how you align bolts in holes, pins in bores, and shafts in bearings. If you get one constraint type right, make it this one.
Surface Contact (Contact de surface)
Forces two faces to be coplanar and in contact — touching, not interpenetrating. Use this for mating flat surfaces: the bottom of a flange onto a base plate, a bearing face against a shoulder, a gasket between two flanges.
Surface contact removes one translational degree of freedom (the direction normal to the faces) and two rotational degrees of freedom (the faces can no longer tilt). This leaves two translations (sliding in the plane) and one rotation (spinning around the normal).
Offset (Décalage)
Creates a specified gap between two elements — a parallelism constraint with a distance. Use it for clearance fits, stand-offs, and any situation where two faces must be a precise distance apart but not touching.
Offset value can be positive (gap) or zero (equivalent to Surface Contact but using the Offset dialog). When the design intent is “these faces touch,” use Surface Contact — it communicates intent more clearly than an Offset of 0.
Angle (Angle)
Forces a specific angle between two elements (planes, lines, or axes). Use for angled brackets, bevel gear axes, and any geometry that cannot be expressed as 0° (coincident) or 90° (perpendicular). Parallelism and Perpendicularity are special cases of the Angle constraint set to 0° and 90° respectively — CATIA provides them as separate dialog options for clarity.
Fix (Ancrage)
Locks a component completely in space, removing all 6 degrees of freedom. The first component in every assembly should be fixed. Everything else is constrained relative to this anchor. CATIA will prompt you to fix the first component automatically — accept it.
Fix in Space vs. Fix: “Fix in Space” locks the component at its current absolute position in the CATProduct space. “Fix” locks it relative to the assembly origin. In most cases they behave identically, but the distinction matters when you move assembly origins or work with published elements.
Managing Degrees of Freedom
A free body in 3D space has 6 degrees of freedom: 3 translations (X, Y, Z) and 3 rotations (around X, Y, Z). Each constraint removes one or more DOF. A fully constrained component has 0 DOF remaining.
CATIA tracks DOF for each component. Right-click a component and select Component > Analyze. The DOF count tells you how many freedoms remain. If a component has 2 DOF remaining after you have applied what should be all necessary constraints, you have a gap in the constraint logic.
Common under-constrained cases:
- Shaft in bore: Axis coincidence removes 4 DOF. You still have axial translation and rotation around the axis — add a Surface Contact or Offset to fix axial position if required.
- Flat plate on surface: Surface contact removes 3 DOF. The plate can still slide in two directions and rotate around the normal — add a coincidence constraint to a hole or edge to remove remaining DOF.
Clash Detection
CATIA V5’s clash detection tools are in the DMU Space Analysis workbench (or accessible from the assembly workbench via Analyze > Clash). Three modes:
- Contact + Clash: finds actual geometric intersection between bodies — they overlap. This is a hard interference — the parts cannot physically exist in this configuration.
- Clearance: finds pairs of components that are closer than a specified minimum distance. Use this to verify assembly clearances: “no two parts closer than 3 mm during operation.”
- Authorized Penetration: for designed-in fits like press fits and O-ring grooves where nominal interference is intentional.
Run a full clash analysis before releasing any assembly for manufacturing. Filter by “Contact + Clash” first — resolve all hard interferences. Then run clearance analysis for moving assemblies.
Export the clash report as HTML or XML for traceability. If clashes are authorized (press fits, designed contacts), document them in the report with an explanation — future engineers will question them during design reviews.
Flexible and Rigid Sub-Assemblies
By default, sub-assemblies in a CATIA product are rigid — their internal constraints are honored but the entire sub-assembly moves as a single unit. This is correct for most situations.
Flexible sub-assemblies allow internal degrees of freedom to be active at the parent assembly level. A hinge mechanism modeled as a sub-assembly can be set to flexible so the assembly can show different hinge angles in different positions. A spring can be set to flexible to show compressed and extended states.
To set a sub-assembly as flexible: right-click the sub-product in the tree and select Properties > Flexible/Rigid sub-assembly > Flexible.
Warning: flexible sub-assemblies significantly increase rebuild time. Use them only for components that genuinely need to move at the assembly level. For clearance analysis of mechanisms, use DMU Kinematics instead of flexible sub-assemblies — it is more efficient for that purpose.
Publication-Based Assembly
Publications are named geometric elements (faces, axes, planes) exposed from a part or sub-assembly for use in the parent assembly. Instead of constraining directly to part geometry (which breaks if the geometry is renamed or restructured), you constrain to published elements.
Example: a shaft part publishes its main axis as “ShaftAxis.” The assembly constrains a bearing bore to “ShaftAxis.” If the shaft geometry is redesigned internally, as long as “ShaftAxis” still exists and refers to the correct axis, the assembly constraint remains valid.
In large-team and long-lifecycle projects (automotive, aerospace), publication-based assembly is the standard approach. Direct geometric references are acceptable for smaller projects where parts are unlikely to be restructured.
Performance Tips for Large Assemblies
Use Visualization Mode (cgr files)
Load assemblies in Visualization Mode (each component shown as a lightweight cgr representation) rather than Design Mode when you only need to view geometry. Switching to Design Mode for a specific component loads it for editing without loading the entire assembly at full resolution.
Use the Cache System
CATIA’s cache system stores cgr files locally. Enable it in Tools > Options > Infrastructure > Product Structure > Cache Management. With cache enabled, large assemblies load dramatically faster on second open.
Suppress unused constraints
Suppressed constraints are not solved during rebuild. For assembly positions that are not needed in the current analysis (e.g., an open position that is not the design-intent closed position), suppress those constraints to reduce solver overhead.
Avoid massive flat assemblies
An assembly with 500 components at the top level is harder to manage than a hierarchy with 5 sub-assemblies of 100 components each. Organize parts into logical sub-assemblies. This also enables parallel team work on sub-assemblies without conflicts at the top level.
Key Takeaways
- Understand how many DOF each constraint type removes. Build constraints logically until 0 DOF remain — neither over-constrained nor under-constrained.
- Run Contact + Clash analysis before every design release. Hard interferences must be resolved; clearance violations must be documented and justified.
- Use flexible sub-assemblies sparingly — they are powerful but expensive in terms of performance.
- In team environments, use publication-based constraints to decouple assembly constraints from internal part geometry changes.
- Enable the CATIA cache system for large assemblies. It is the single highest-impact performance setting for day-to-day work.
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