Building Solid Geometry in CATIA V5
CATIA V5 Part Design is the core module for creating 3D solid geometry. Unlike some CAD systems where you stumble toward a result, CATIA V5 is built around a logical sequence of sketch-based and surface-based operations. Master the ten operations in this guide and you can model the vast majority of machined and cast mechanical components.
Each operation maps to a manufacturing process or a logical design intent. Understanding that connection makes you a better modeler and catches design-for-manufacture issues early.
1. Pad (Boss)
Pad extrudes a 2D sketch profile into a 3D solid. Select a sketch, choose the extrusion length, and confirm. The result is a prism whose cross-section is the sketch profile.
Key options:
- Mirrored extent: extrudes equally in both directions from the sketch plane. Use for symmetric geometry to keep the design intent clear.
- Up to face/surface: extrudes until it contacts a specified face. This creates features that automatically adapt to neighboring geometry — preferred over fixed-length pads in assemblies where mating parts can change.
- Thick sketch: creates a shell-like result from an open sketch profile. Rarely used in standard practice.
Practical note: name every Pad feature. “Pad.1” tells you nothing. “BasePlate_Pad” is clear in the tree and in change management.
2. Pocket
Pocket removes material by cutting a sketch profile into an existing solid. The logical inverse of Pad. Use it for recesses, slots, and counterbores.
The “Up to last” option is powerful for through-pockets in complex geometry — it cuts through everything in the path rather than requiring a fixed depth. For blind pockets, set an explicit depth and verify the floor face is exactly where manufacturing requires it.
3. Shaft (Revolution)
Shaft revolves a 2D profile around an axis to create a solid of revolution. This is the primary tool for turned parts: shafts, discs, flanges, and bearing seats.
The sketch for a shaft operation is typically a cross-section of the part above the rotation axis (a half-profile). The axis is either a sketch line or a reference axis. CATIA creates the full 360° solid (or partial, for sectors).
Critical requirement: the sketch profile must be entirely on one side of the rotation axis. If any part of the profile crosses the axis, the feature fails. Common mistake when modeling stepped shafts — ensure each shoulder of the sketch stays clear of the axis line.
4. Groove
Groove removes material by revolving a sketch profile around an axis — the subtractive counterpart to Shaft. Use it for turning operations: undercuts, groove reliefs for bearing seats, sealing grooves for O-rings.
For an O-ring groove on a shaft, sketch the groove cross-section (typically rectangular with rounded corners per AS 568 or ISO 3601 standards), place the profile at the correct axial position, and revolve 360°. The resulting groove is accurate to the standard dimensions and directly communicates the design intent.
5. Fillet
Fillet rounds sharp edges to remove stress concentrations, meet safety standards (no sharp edges), or represent a manufacturing process (a milled corner has a natural radius equal to the tool radius).
CATIA V5 offers variable-radius fillets and stylistic fillets for complex transitions. For standard engineering use, constant-radius edge fillet is sufficient in most cases.
Design-for-manufacture guidance: on CNC milled pockets, the internal corner radius equals the radius of the end mill used. Specify fillet radii in whole millimeters that correspond to standard tool sizes: 1, 2, 3, 4, 5, 6, 8, 10, 12, 16 mm. A 3.7 mm radius requires a non-standard tool or additional operations.
6. Chamfer
Chamfer adds an angled cut at edges. Standard applications: deburring edges (0.5×45° or 1×45°), creating lead-ins on shafts for easy assembly, and chamfering thread runouts.
Specify chamfer by angle and distance (e.g., 1 mm at 45°) or by two distances. The 45° chamfer is the machinist default. If you need a specific angle for a functional reason, note it explicitly on the drawing — otherwise machinists will apply 45° regardless of what the model shows.
7. Draft
Draft applies a taper angle to faces to enable part ejection from molds. Without draft, plastic injection molded and die cast parts cannot be removed from the tool — they lock mechanically.
Minimum draft angle depends on material and surface finish: typically 0.5° to 1° for polished surfaces, 1° to 3° for textured or grained surfaces. Deep ribs and bosses need more draft than shallow features.
Apply Draft early in the Part Design tree — before fillets. If you fillet first and draft second, the draft operation can distort the fillet geometry unpredictably. The correct sequence: Shaft/Pad → Draft → Fillet → Pocket.
8. Shell
Shell hollows a solid part to a uniform wall thickness, optionally removing specified faces to create openings. This is the standard modeling approach for plastic enclosures, thin-walled housings, and formed sheet metal shapes.
Specify which faces to remove (these become openings) and the desired wall thickness. CATIA offsets all remaining faces inward by the wall thickness.
Shell fails when the offset distance creates self-intersecting geometry — typically at sharp concave corners or small features. If Shell fails, add fillets to the problematic edges first, or increase the wall thickness until the geometry is self-consistent.
9. Pattern (Rectangular and Circular)
Pattern copies features at regular intervals. Rectangular Pattern creates a 2D grid of copies; Circular Pattern distributes copies around an axis.
Always pattern the feature, not the sketch. If you pattern at the sketch level (creating multiple circles in one sketch), you lose the ability to modify individual instances later. At the feature level, you can suppress, modify, or delete individual pattern members.
For hole patterns on a bolt circle, Circular Pattern driven by a Hole feature gives the cleanest result. Set the rotation axis, number of instances, and total angle (360° for a full circle). Verify that the angular spacing matches your thread callout and torque specification.
10. Boolean Operations
CATIA V5 Part Design supports multiple bodies within one part. Boolean operations combine or subtract these bodies:
- Assemble: combines two bodies into one (similar to Union). Used to merge separately modeled sections of a complex part.
- Add: explicitly adds material from one body to another.
- Remove: subtracts one body from another. Useful for modeling cavities defined by complex tool paths or mating geometry.
- Intersect: keeps only the material common to both bodies.
Multi-body design is powerful for complex parts where different sections have different design history. A housing with a main body, a separate boss structure, and a mounting flange can each be modeled as independent bodies, then assembled with Boolean operations. Changes to one section do not disturb the others.
Body Management in Multi-Body Parts
When working with multiple bodies, always name each body in the specification tree. Use Insert > Body to create new bodies. Assign features to the correct body using the Define in Work Object function (right-click the body name).
A common mistake is accidentally adding features to the wrong body, which creates unexpected geometry or failures. Check the active body (shown in bold in the tree) before creating any new feature.
Key Takeaways
- Pad/Pocket and Shaft/Groove are the primary volume-creating and volume-removing operations — master these first before exploring advanced operations.
- Apply Draft before Fillet in the feature tree for cast and molded parts. Reversing this order causes geometry problems.
- Name every feature. An unnamed tree is a maintenance nightmare in team environments.
- Pattern features, not sketches — feature-level patterns allow individual instance modification.
- Boolean operations with multiple bodies allow complex parts to be modeled in logically separate sections that can be individually modified.
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