Sketcher and Part Design - Practical Guide

CATIA · Part Design

Overview

Part modeling starts in the Sketcher and finishes in Part Design. This page walks through sketch entry, sketch-based features (Pad, Pocket, Shaft, Rib), Dress-Up operations (fillet, chamfer, draft, shell), Boolean, Reference Elements, and Body / Feature tree management — all in one coherent flow.

These are the fundamentals that let automotive-part, tooling, and structural engineers model quickly while preserving Design Intent.

1. Entering Sketcher and Core Concepts

A Sketch can only be drawn on a Plane or a planar face. Select the plane and click the Sketcher icon, or simply double-click the plane.

Sketch vs. Positioned Sketch — a standard Sketch fixes the origin automatically, whereas a Positioned Sketch lets you choose the H / V axes and origin. For reusability and Design Intent, defaulting to Positioned Sketch is the safer habit.
H-axis (Horizontal) — horizontal axis, red arrow.
V-axis (Vertical) — vertical axis, green arrow.
Origin — intersection of H and V. The reference point for the first Constraint.

Tip Snap and spacing can be tuned at Tools → Options → Mechanical Design → Sketcher → Grid. In practice, however, it is better for maintainability to turn the grid off and drive geometry with Constraints.

2. Sketcher Toolbar Overview

2.1 Profile and Shape Tools

Profile — the workhorse for chaining lines, arcs, and splines
Rectangle, Oriented Rectangle, Parallelogram
Elongated Hole, Keyhole, Cylindrical Elongated Hole
Circle, Three Point Circle, Tri-tangent Circle, Arc
Spline, Conic — GSD-style curves
Line (Bi-tangent, Angle/Normal, Bisecting)
Axis — rotational axis. Mandatory for Shaft / Groove.
Point (Coordinates, Equidistant, Intersection, Projection)
Ellipse, Parabola by Focus, Hyperbola by Focus
Connect — joins two elements with a curve

2.2 Operation Tools

Corner / Chamfer — fillet and chamfer
Trim / Break / Quick Trim — trimming
Close Arc / Complement Arc — close or complete arcs
Mirror, Symmetry
Translate, Rotate, Scale, Offset — move / rotate / scale / offset (with a duplicate option)
Project 3D Elements — project a 3D edge onto the sketch plane (yellow)
Intersect 3D Elements — intersection of a 3D element with the sketch plane (yellow)
Project 3D Silhouette Edges — silhouette projection (for sphere / cylinder boundaries)

Tip Yellow elements created by Project / Intersect are linked back to their 3D source and update automatically. To break the link, right-click → Isolate.

Note Overusing Project clutters the Tree and sharply increases Update time. Use it only where truly needed, and prefer Reference Elements as a workaround when possible.

3. Constraint Strategy

The field rule is simple: geometric constraints first, dimensional constraints last. If you lead with dimensions, the geometry warps in unintended ways when a dimension changes.

Order of application:

Horizontal / Vertical
Parallel / Perpendicular / Coincident / Tangent / Concentric
Symmetry / Equal Radius / Equal Length
Dimensional (Length, Radius, Angle, Distance)

3.1 Color Codes

White — Under-constrained (can still be dragged)
Green — Iso-constrained (fully constrained, ideal)
Purple — Over-constrained (must be cleaned up)
Red — Inconsistent (contradictory)
Yellow — External Reference
Brown — Not changed (not yet updated)

Tip Aim for green (Iso-constrained) in everyday work, but when driving a model with a Design Table it is sometimes intentional to leave a little Under-constraint so dimensions can drive freely.

Note When an Over-constraint warning appears and is acceptable from an engineering standpoint, you can press "Deactivate" in the dialog to silence just one constraint as a temporary fix.

3.2 Common Constraint Combinations

Goal	Constraint combination
Symmetric profile	Symmetry (about a centerline)
Two concentric circles	Concentric
Two matched gears	Equal Radius
Both ends of a slot	Tangent + Concentric
Parallel bars	Parallel + Distance
Rounded corners	Tangent + Equal Radius

4. Sketch Analysis and Practical Sketch Tips

Tools → Sketch Analysis (inside Sketcher) has three tabs.

Geometry — open profiles, self-intersection, closure
Use-Edges — status of external references (broken links)
Diagnostic — over-/under-/inconsistent-constraint diagnosis

Tip Running Sketch Analysis before Pad/Pocket to verify "Closed Profile" is the fastest way to stay clear of the "The profile is not closed" error.

A handful of habits that have stuck from real work:

1 Sketch = 1 Design Intent — do not stuff every detail into one sketch. Split the work across Pad → Pocket → Chamfer.
Use Construction Geometry — auxiliary lines such as the one aligning two circle centers should live as Construction lines (toggle the icon).
Anchor near the origin — coincident-couple one point of the profile to Origin to prevent dangling geometry.
Leverage sub-elements — draw a rectangle, then drag a single edge to tweak only that part.
Animate Constraint — right-click a dimension → Animate Constraint to sweep a range slider and preview the mechanism's motion.
Change Sketch Support — move a sketch onto a different plane to reuse the sketch itself.

5. Part Design — Sketch-Based Features

The shared menu path is Insert → Sketch-Based Features → {feature}.

Pad (extrude) — Type: Dimension / Up to Next / Up to Last / Up to Plane / Up to Surface. Thick (thin wall), Mirrored Extent (symmetric), Second Limit under More.
Pocket — Pad subtracted.
Shaft (revolve) — Sketch + axis of revolution (an Axis inside the Sketch or an external Line). Angle 0 – 360°.
Groove — Shaft subtracted.
Rib — sweep a Profile along a Center Curve. Profile Control options: Keep Angle / Pulling Direction / Reference Surface. A Spine can be specified.
Slot — Rib subtracted.
Stiffener — creates a rib from a single line.
Multi-Sections Solid (Loft) — multiple Sections + Guide Curves + Spine.
Removed Multi-Sections Solid — Loft subtracted.
Solid Combine — intersection of the extruded volumes of two profiles. Handy for cam and gear shapes.

6. Dress-Up Features

Edge Fillet — Constant / Variable Radius, Chordal mode, Conic Parameter
Variable Radius Fillet — different R at each point
Face-Face Fillet — round between two faces even without an edge
Tritangent Fillet — round tangent to three faces
Chamfer — Length/Length or Length/Angle
Draft Angle — draft. Neutral Element is required. Essential for mold design.
Draft Reflect Line — draft based on the silhouette (reflect line)
Shell — hollow out a solid. Outer Face + Inner / Outer Thickness.
Thickness — change face thickness.
Thread / Tap — virtual threads (no geometry is created; only annotation data is attached).
Remove Face / Replace Face — delete or replace faces.

7. Boolean Operations

Operations that combine multiple Bodies within a Part.

Assemble — preserves plus / minus signs
Add — union
Remove — subtraction
Intersect — intersection
Union Trim — merge, then cut away a portion
Remove Lump — strip off an unwanted chunk

Tip Building several Bodies and combining them with Boolean yields a cleaner Tree and fewer edit conflicts than a long Pad → Pocket chain. Strongly recommended for automotive parts.

Note Boolean operations are order-sensitive. Reordering Assemble operations can change the final geometry.

8. Reference Elements

The skeleton of a Part design — a collection of "Point / Line / Plane" elements.

Point — Coordinates, On Curve, On Plane, On Surface, Circle Center, Tangent on Curve, Between
Line — Point-Point, Point-Direction, Angle/Normal, Tangent to Curve, Normal to Surface, Bisecting
Plane — Offset, Parallel through Point, Angle/Normal, Through 3 Points, Through 2 Lines, Through Point and Line, Through Planar Curve, Normal to Curve, Tangent to Surface, Equation, Mean through Points

Tip Collect Reference Elements at the top of the Tree so that every downstream feature references them. That is the Skeleton approach, and it minimizes the ripple of design changes.

→ See also: /cad-tips/catia/assembly-dmu.md for skeleton-based Top-down design.

9. Transformation Features

Move or pattern the Body / Feature itself.

Translation / Rotation / Symmetry — translate / rotate / mirror the entire Body
AxisToAxis — coordinate-system move
Mirror — mirror-copy a Body or Feature
Rectangular Pattern — rectangular array. Instance(s) & Length / Instance(s) & Spacing
Circular Pattern — circular array. Specify the reference axis.
User Pattern — based on sketch points (irregular array)
Scaling / Affinity — scaling

Tip Turning on Pattern's "Keep specifications" lets each instance's length track dynamically (e.g., "Up to Next"). Turn it off to replicate at a fixed length.

10. Using the Hole Feature Properly

Path: Insert → Sketch-Based Features → Hole. One of the most frequently used tools on the shop floor.

Type — Simple / Tapered / Counterbored / Countersunk / Counterdrilled
Thread — Metric, UNC, UNF, Gas, or No Thread
Extension — Blind / Up To Next / Up To Last / Up To Plane / Up To Surface
Positioning Sketch — the center-dimension sketch of the Hole
Bottom Type — Flat / V-bottom (118° / 120°)

Tip When you create a Hole, a Positioning Sketch is generated alongside it automatically. You must double-click that sketch and dimension it to pin down the Hole location. Without constraints, the hole snaps to the origin.

11. Body / Feature Tree Management

PartBody — the default main Body (cannot be deleted)
Body.2, Body.3 … — additional Bodies, created via Insert → Body
Define in Work Object — activates a specific Body (green underline). Features are added only to the active Body.
Change Body — moves a given Feature into a different Body.

Tip For symmetric parts, model one half in Body.2, then Mirror + Assemble into PartBody. Editing one side automatically updates the other, cutting design-change cost in half.

11.1 Naming Conventions

Rename to something meaningful: Pad.1 → Pad_BaseHousing
Split Bodies by function: Main / Mounts / Cutouts
Gather Reference Elements at the top of the Tree and prefix them (e.g., Ref_)
Prefer Ordered Geometrical Set (guarantees build order)

Field Checklist

Start every sketch as a Positioned Sketch
Honor the geometric-first, dimensional-last order
Verify Closed Profile with Sketch Analysis before Pad / Pocket
Rename features meaningfully (e.g., Pad.1 → Pad_Housing)
Split Bodies by function and combine with Boolean
Keep Reference Elements at the top of the Tree (Skeleton approach)
Set Pattern's Keep specifications option to match the intent
Always dimension the Positioning Sketch of a Hole
For symmetric parts, maintain one side via Mirror + Assemble