Before you draw a single line in CATIA, you need to answer one question: where exactly am I going to sketch? The answer is always a sketch plane — and that’s where CATIA’s Plane feature comes in.
“The three default planes — XY, YZ, and ZX — will only take you so far. Once your models get more complex, the Plane command becomes indispensable.”
This post covers the Plane command in CATIA Part Design, focusing on the 5 creation options most commonly used in real engineering work — with practical tips on when and why to use each one. We also cover uses that go well beyond sketching.
The Default Sketch Planes — XY, YZ, ZX
Every time you create a new Part in CATIA, three reference planes are generated automatically.
- XY Plane: The most frequently used default. Corresponds to the Top View — looking straight down at the part.
- YZ Plane: The left/right lateral reference. Corresponds to the Front View.
- ZX Plane: The front/rear cross-section reference. Corresponds to the Right Side View.
To start sketching, click the Sketch icon or go to Insert → Sketcher → Sketch, then click one of the three planes to enter the sketcher. Once inside, the yellow arrow marker at the intersection point is the sketch origin. Always apply at least one constraint relative to this origin before you start drawing.
If your sketch floats freely — not anchored to the origin — editing dimensions later or assembling the part can cause the geometry to move in unpredictable ways. It’s a small habit that prevents major headaches down the line. Always lock at least one relationship to the origin.
What Is the Plane Command?
The three default planes aren’t always enough. You might need to sketch on an angled surface, add geometry at a specific offset distance, or define a cross-section perpendicular to a curved path.
That’s what the Plane command is for. A Plane is a virtual reference plane stored in the model tree — it acts as a sketch base or a geometric reference. It’s not a physical surface that gets machined or printed; it’s a positioning tool.
How to launch it: Insert → Reference Elements → Plane, or click the Plane icon in the toolbar.
The Plane Definition dialog box opens immediately. Use the dropdown at the top to select the creation method that suits your situation.
The 5 Most Useful Plane Creation Options
① Offset from Plane — Parallel at a Set Distance
The most frequently used option by far. Creates a new plane parallel to a reference plane, offset by a specified distance.
- Required inputs: A reference plane and an offset distance (mm)
- Pro Tip: Need to sketch 50mm above the XY plane? Create an offset plane at Z+50 and sketch directly on it. Use the Reverse Direction button to flip the offset to the opposite side.
② Parallel Through Point — Parallel but Pinned to a Vertex
Creates a plane parallel to a reference plane, but forced to pass through a specific point.
- Required inputs: A reference plane and a point
- Pro Tip: When you can’t easily type in an exact offset distance, selecting an existing vertex or point lets you anchor the plane precisely without guessing numbers.
③ Angle / Normal to Plane — Rotated at a Specific Angle
Creates a plane rotated by a specified angle around a selected axis, relative to a reference plane.
- Required inputs: A reference plane, a rotation axis (line, edge, or cylinder axis), and an angle value
- Pro Tip: Essential for angled brackets, drafted faces, and tapered geometry. Set the angle to 90° and it behaves exactly like a “Normal to Plane” — perpendicular to the reference.
④ Tangent to Surface — Flush Against a Curved Face
Creates a plane tangent to a curved surface at a specified point on that surface.
- Required inputs: A reference surface and a point on that surface
- Pro Tip: Use this when you need to sketch markings or add features on the outer face of a cylindrical part. Also comes up frequently in GSD (Generative Shape Design) work where surface tangency defines direction.
⑤ Normal to Curve — Perpendicular to a Path
Creates a plane perpendicular to a curve at a specific point along it.
- Required inputs: A reference curve and a point (defaults to the curve midpoint if none is specified)
- Pro Tip: This is the go-to option for defining cross-section profiles for Pipe or Sweep features. Define the sweep path first, then use Normal to Curve to place a section plane exactly where you need the profile.
Quick Reference — 5 Practical Plane Options
| Option | Required Inputs | Best Used For |
|---|---|---|
| Offset from Plane | Reference plane + distance (mm) | Sketching at a precise offset distance |
| Parallel Through Point | Reference plane + point | Anchoring a plane to an existing vertex |
| Angle / Normal to Plane | Reference plane + axis + angle | Angled brackets, tapered features |
| Tangent to Surface | Surface + point on surface | Sketching on cylindrical or curved faces |
| Normal to Curve | Curve + point | Cross-section profiles for Pipe / Sweep |
Planes are powerful, but adding too many bloats the model tree and makes future edits much harder to manage.
- Whenever possible, select an existing face directly as your sketch plane — this keeps the tree lean and readable.
- Reserve the Plane command for situations where no suitable face exists, or when you need an angled or curve-based reference.
- Rename your planes to something meaningful (Plane_Top_50, etc.) — future you and your teammates will thank you.
Beyond Sketching — Other Practical Uses of the Plane Feature
Most engineers first encounter Planes as sketch bases — but that’s only one of their jobs. A reference plane in CATIA can serve as a geometric anchor across the entire modeling and assembly workflow.
① Mirror Reference Plane
The Mirror command in Part Design lets you symmetrically copy existing features — Pad, Pocket, and more. The mirror symmetry axis is defined by a plane, and that’s where a custom reference plane earns its keep.
- Finish modeling the left half of a bracket, create a center plane using Offset from Plane, and Mirror — the right side is done in seconds.
- At the assembly level, the Symmetry command works the same way: define a reference plane and CATIA mirrors the selected components across it. This is essential when generating a Right-Hand (passenger-side) jig from a Left-Hand (driver-side) model.
② Assembly Constraint Reference
When positioning components in an assembly, part faces aren’t always a practical constraint target — especially when you’re working with curved or irregular geometry. A common real-world example: mounting a sensor or bracket perpendicular to a curved surface.
- Create a plane using Tangent to Surface or Normal to Curve in advance, then use that plane as the reference for a Coincidence or Offset constraint in the assembly.
- When a component’s mating face is a freeform surface, a pre-positioned reference plane massively simplifies the constraint workflow and eliminates guesswork.
③ Section Analysis Reference
The Sectioning command in the Space Analysis workbench cuts through an assembly dynamically, letting you inspect internal geometry. The cutting plane is defined by a reference plane, so placing it precisely is essential.
- Use this to verify part-to-part clearances during an interference check at a specific cross-section location.
- In Generative Drafting, the same applies: defining a Section View requires a cutting plane, and a pre-created reference plane gives you full control over its position.
④ Distance & Angle Measurement Reference
The Measure Between command accepts a reference plane as one of its measurement targets. You can measure exactly how far a part face sits from your reference plane, or at what angle it’s tilted.
- Useful for verifying that geometry aligns with a carline coordinate plane or meets a tolerance requirement defined in Carline space.
- Sketch base — Define where to draw your 2D profile (the most fundamental use)
- Mirror reference — Symmetrically copy features or assembly components across a center plane
- Assembly constraint anchor — Constrain parts with curved or freeform mating faces precisely
- Section & measurement reference — Interference checks, drawing section views, distance / angle verification
Wrapping Up
The CATIA Plane feature is far more than a sketch helper. It’s a core reference element used throughout the entire modeling and assembly process — for mirroring, constraining, sectioning, and measuring, not just drawing.
- Most-used option — Offset from Plane (parallel at a set distance)
- Angled geometry & mirror base — Angle / Normal to Plane
- Sweep / Pipe cross-sections & curve-normal constraints — Normal to Curve
- Curved surface constraints & sensor mounting — Tangent to Surface