CATIA V5 · Sketcher · Fundamentals
Before you can create any 3D solid in CATIA, you have to go through one essential first step: the Sketch. Whether you’re using Pad, Pocket, or Shaft, every 3D feature starts from a 2D Profile drawn inside the Sketcher workbench.
“Sketching in CATIA isn’t really about drawing — it’s about constraining. Keep going until everything turns green.”
In this post, I’ll walk through how to enter and exit the Sketcher, the essential drawing commands, the different types of constraints, and how to diagnose and fix over-constrained sketches — everything you need to build clean, reliable sketches from day one.
1. What Is a Sketch?
A sketch is the 2D foundation of any 3D model. You draw shapes — lines, circles, rectangles — on a plane, define their size and position using dimensions and constraints, and then use a 3D command (Pad, Pocket, Shaft, etc.) to give it depth or volume.
- Every 3D feature in CATIA follows the same flow: Sketch → 3D Feature.
- The quality of your sketch directly determines the quality of your 3D model. A sloppy sketch makes downstream edits painful.
- The goal at the end of every sketch session is to reach a Fully Constrained state — no ambiguity, no loose geometry.
2. Entering and Exiting the Sketcher
2-1. How to Enter the Sketcher
- Click the Sketch icon in the toolbar, or go to Insert → Sketcher.
- Select a plane to sketch on.
- The view switches to 2D and you’re now inside the Sketcher workbench.
2-2. Choosing Your Sketch Plane
Choosing the right plane is the first decision you make in any sketch. There are three main options:
| Plane Type | Description | When to Use |
|---|---|---|
| Default Planes (XY, YZ, ZX) | The three reference planes built into every part file | Your very first sketch when starting a new part |
| Existing Face | Any flat face on an already-created 3D solid | Adding a pocket or boss on top of existing geometry |
| Reference Plane | A custom plane created by the user | When you need a sketch at an offset or angled position |
2-3. How to Exit the Sketcher
- Click the Exit Workbench icon on the right side of the Sketcher toolbar.
- Alternatively, double-click the part name above the sketch in the specification tree to return to the 3D environment.
If you see “Sketch is not fully constrained” when exiting, CATIA is telling you the sketch still has unconstrained degrees of freedom. You can still create a 3D feature from it — but if you ever edit a dimension or constraint later, the geometry may shift in unexpected ways. Get in the habit of exiting only when the sketch is fully green.
3. Essential Sketcher Commands
Once you’re inside the Sketcher, a set of drawing tools appears in the toolbar. Here are the ones you’ll reach for most often in practice:
| Command | Location | What It Does |
|---|---|---|
| Profile | Profile toolbar | Draws connected lines and arcs in a single continuous stroke. The most-used command in the Sketcher. It seamlessly transitions between straight segments and arcs, letting you draw a complete closed shape in one go. |
| Line | Profile toolbar | Click two points to draw a straight line. Unlike Profile, it stays in line mode only — no arc transitions. |
| Circle | Profile toolbar | Click to set a center point, then drag to define the radius. Used constantly for bolt holes, shaft cross-sections, and similar round features. |
| Rectangle | Profile toolbar (Predefined Profile) | Click two diagonal corners to draw a rectangle. Horizontal and vertical constraints are applied automatically. |
| Spline | Profile toolbar | Click multiple points to create a smooth freeform curve. Used for organic or aerodynamic shapes. |
| Corner (Fillet) | Operation toolbar | Rounds the corner where two lines meet with a specified radius. |
| Chamfer | Operation toolbar | Applies an angled cut at the intersection of two lines. |
| Trim (Quick Trim) | Operation toolbar | Click the unwanted segment between intersections to remove it. Similar to the TR command in AutoCAD. |
In real-world use, most designers don’t switch between Line and Circle separately — they draw almost everything with Profile. While drawing a straight segment, nudge the third point slightly off-axis and Profile automatically switches to arc mode. A complete closed shape, drawn without lifting a finger. It’s a huge time saver once you get the feel for it.
4. Constraints — The Heart of the Sketcher
Drawing a shape is just the beginning. Without constraints, nothing is locked down — drag any element and it moves freely. Constraints are what pin the geometry in place, defining exactly where things are, how big they are, and how they relate to each other.
There are two types: Geometrical Constraints (relationship-based) and Dimensional Constraints (number-based).
4-1. Geometrical Constraints
These define the relationship between geometric elements — no numbers involved, just rules like “these two lines must be parallel.”
| Constraint | What It Does | Typical Use |
|---|---|---|
| Coincidence | Merges a point with another point or a line | Snapping a line endpoint to a circle center |
| Horizontal | Forces a line to lie along the H axis | Keeping a bottom edge perfectly level |
| Vertical | Forces a line to lie along the V axis | Keeping a side edge perfectly upright |
| Perpendicular | Makes two lines meet at exactly 90° | Ensuring a clean right angle on an L-shaped profile |
| Parallel | Keeps two lines running in the same direction | Maintaining equal slope between top and bottom edges |
| Tangent | Joins a line and an arc with a smooth transition | Blending a straight section into a curve |
| Concentric | Aligns the centers of two circles or arcs | Inner and outer diameters sharing the same center |
| Symmetry | Mirrors two elements about an axis | Designing a left-right symmetric profile |
| Fix | Locks a point or element in absolute space | Anchoring the sketch to the origin |
4-2. Dimensional Constraints
These lock down size and position with numbers. Click the Constraint icon in the Constraint toolbar, select an element, and CATIA automatically offers the appropriate dimension type.
- Line length: Select a line to constrain its length.
- Circle radius / diameter: Select a circle or arc to constrain its size.
- Distance between two elements: Select two lines or points in sequence to constrain the gap between them.
- Angle: Select two lines to constrain the angle between them.
- Position from origin: Select a point to lock its H or V distance from the origin.
The recommended order: apply geometrical constraints first (horizontal, vertical, coincident, tangent, etc.) to establish all the relationships between elements, then add dimensional constraints to pin down the sizes. This approach minimizes the number of dimensions you actually need — and significantly reduces the risk of accidentally over-constraining your sketch.
5. Reading Constraint Status by Color
One of the most intuitive things about the CATIA Sketcher is that you can tell the constraint status of any element just by looking at its color.
| Color | Status | What It Means |
|---|---|---|
| ⬜ White | Under-constrained | The element still has unconstrained degrees of freedom. Drag it and it moves. Something about its size, position, or orientation is still undefined. |
| 🟩 Green | Fully Constrained | Every degree of freedom is locked down. This is the target state — nothing moves, everything is exactly where it should be. |
| 🟪 Purple / Pink | Over-constrained | Too many constraints are applied, or two constraints are contradicting each other. You need to find and delete the conflicting or redundant one. |
5-1. Common Causes of Over-Constraint
- Applying duplicate constraints that mean the same thing: If you apply a Horizontal constraint to a line and then also give it a 0° angle dimension — that’s over-constrained. Both say “make it horizontal.” One of them has to go.
- Adding H/V constraints to a Rectangle: The Rectangle command automatically applies horizontal and vertical constraints. Adding them again manually creates exact duplicates.
- Dimensioning something already determined by geometry: If two lines have Parallel + Equal Length constraints, giving each its own length dimension creates a conflict — one of those lengths is already implied by the other.
5-2. How to Fix Over-Constraints
- Identify the purple/pink elements in your sketch.
- Click on an affected element — CATIA will highlight the associated constraint icons.
- Right-click the redundant or conflicting constraint and select Delete.
- Once the purple turns green, you’re done.
Over-constraints are immediately visible — the sketch turns purple and you know something’s wrong. But leaving an under-constrained sketch (white elements) as-is is a subtler and often more damaging mistake. It might look fine today, but the moment you modify a dimension or feature downstream, your sketch can drift in directions you never intended. “Why did my shape suddenly change?” — nine times out of ten, that’s an under-constrained sketch coming back to haunt you.
6. Recommended Sketch Workflow
Here’s the step-by-step process that experienced CATIA designers tend to follow:
- Select a plane and enter the Sketcher.
- Use Profile to rough out the shape. Don’t worry about exact dimensions at this stage — just get the general form down.
- Apply geometrical constraints (horizontal, vertical, coincident, tangent, symmetry, etc.) to lock in the relationships between elements.
- Add dimensional constraints to define sizes and positions with numbers.
- Confirm that every element is green (Fully Constrained).
- Click Exit Workbench to return to the 3D environment.
Quick Reference: Key Sketcher Commands
| Command | Location | Description |
|---|---|---|
| Sketch | Insert → Sketcher | Enter the Sketcher workbench (plane selection required) |
| Exit Workbench | Right side of Sketcher toolbar | Return to the 3D Part Design environment |
| Profile | Profile toolbar | Draw connected lines and arcs — most used command |
| Constraint | Constraint toolbar | Apply dimensional constraints (length, angle, distance, etc.) |
| Coincidence | Constraint toolbar | Merge a point with another point or edge |
| Fix | Constraint toolbar | Lock an element’s absolute position in space |
| Quick Trim | Operation toolbar | Remove the segment between two intersections with a click |
| Corner (Fillet) | Operation toolbar | Apply a rounded fillet to a sharp corner |
Wrapping Up
The Sketcher isn’t really about drawing — it’s about constraining. Getting a rough shape onto the screen takes seconds. What takes real attention is locking that shape down so it can’t move. Here’s the short version:
- White = under-constrained, green = fully constrained, purple = over-constrained — the color tells you exactly where you stand
- Workflow: Profile to rough the shape → geometrical constraints → dimensional constraints → confirm all green → Exit
- Never leave white elements behind — an under-constrained sketch will eventually cause geometry to shift in ways that are very hard to trace back