CATIA V5 · Part Design Intermediate · Patterns & Multi-Body
Once you’re comfortable with the fundamentals — Pad, Pocket, Shaft — it’s time to work smarter. Modeling complex parts efficiently means knowing how to stop drawing the same feature over and over, and how to organize a part’s geometry in a way that actually scales. That’s where Patterns and Multi-Body design come in.
“The gap between a beginner and an experienced CATIA designer isn’t the commands they know — it’s how effectively they use patterns and manage bodies.”
In this post, I’ll cover Rectangular and Circular Patterns with their key parameter options, the Multi-Body design philosophy used in real production environments, and when (and when not) to use Boolean Operations.
1. Rectangular Pattern
Rectangular Pattern copies a selected feature and arranges the copies in a grid along two linear directions. Cooling fin arrays on a heat sink, evenly spaced bolt holes on a cover plate — instead of drawing each one individually, you draw one, define the pattern, and CATIA handles the rest.
- Create the base feature you want to repeat (a Hole, Pocket, or any other feature).
- Select it in the spec tree, then click the Rectangular Pattern icon.
- First Direction: Under Reference element, select an edge or straight line to define the pattern direction. Use Reverse to flip it if needed.
- Second Direction (optional): Switch to the Second Direction tab to add a perpendicular repeat — turning a linear array into a full 2D grid.
- Set your Parameters and click OK.
Pattern Parameter Options — Comparison
| Parameter Option | What You Define | How It Works |
|---|---|---|
| Instance(s) & Length | Count + total span | CATIA divides the total length evenly across the given number of instances |
| Instance(s) & Spacing | Count + pitch distance | The most commonly used option in practice — “N copies, X mm apart” |
| Spacing & Length | Pitch distance + total span | CATIA calculates how many copies fit within the span at the given pitch |
| Instance(s) & Unequal Spacing | Count + individual gaps | Lets you set a different spacing between each pair of instances independently |
2. Circular Pattern
Circular Pattern arranges copies of a feature around a rotation axis — the circular equivalent of Rectangular Pattern. Gear teeth, bolt holes on a pipe flange, fan blades: all of these are a single feature repeated around a center.
- Create and finalize the base feature you want to repeat.
- Select it and click the Circular Pattern icon. (It’s nested under the Rectangular Pattern icon — click the dropdown arrow.)
- Reference element: Select a cylindrical face or the center axis of the body to define the rotation center.
- Set your Parameters and click OK.
Set the Parameters option to Complete Crown and you don’t have to calculate angles at all. Just enter the number of instances and CATIA automatically distributes them evenly around 360°. This is how experienced designers almost always set up circular patterns — it’s faster and eliminates rounding errors.
3. Multi-Body Design — “One Body, One Material”
Beginners tend to dump everything — dozens of Pads, Pockets, Fillets — into the single default PartBody. For simple shapes it works fine, but as complexity grows, that single-body approach becomes a maintenance trap. Editing anything cascades errors everywhere.
Experienced designers use Multi-Body design instead: creating multiple separate Bodies inside a single Part file, each representing a distinct piece of raw material or manufactured component. In fixture and jig design shops especially, you’ll find this guiding principle:
- 1 Part = 1 independent component: The base plate is one Part file. The locating pin is another. The clamp is another.
- 1 Body = 1 piece of raw stock: If the base is a welded weldment made from several steel plates, each plate gets its own Body inside the single Part file.
- Done right, your 3D model’s structure mirrors your Bill of Materials (BOM) — which makes drawing creation and fabrication data extraction dramatically more straightforward.
- Cleaner drafting: When you create 2D drawings later, you can generate a separate view for each Body and dimension each piece of raw stock individually — no need to untangle a single monolithic geometry.
- Laser / plasma cut data in seconds: Since each plate is its own Body, exporting individual DXF flat patterns for laser cutting is trivial. No manual extraction, no geometry hunting.
- Safe, isolated edits: Changing the thickness or profile of one Body doesn’t cascade errors into the others. Each piece of stock is self-contained.
4. Boolean Operations — Merging and Subtracting Bodies
In automotive, tooling, and injection mold design, flows that use Multi-Body modeling eventually consolidate everything into a single main body at the end. That’s where Boolean Operations come in.
| Operation | What It Does | Typical Use Case |
|---|---|---|
| Add | Merges the volumes of two bodies into one | Welding a handle body onto a main body to form a single solid |
| Remove | Subtracts one body’s volume from another | Creating a machining pocket as a separate body, then stamping it out of the main casting |
| Intersect | Keeps only the overlapping volume between two bodies | Extracting the exact intersection zone between two complex curved solids |
Boolean Add makes sense for injection-molded parts that need to be “one piece” in the end. But for jigs, fixtures, and welded weldments — parts made from multiple individual pieces of stock bolted or welded together — merging Bodies via Add destroys the very structure that makes Multi-Body useful. Once merged, you lose the ability to dimension each plate individually in 2D and you can no longer export per-piece laser cutting files. In fixture and weldment design, keep each Body as its own discrete piece — and leave them that way.
Wrapping Up
How efficiently you model in CATIA comes down to two habits: using patterns to eliminate repetitive work, and managing Bodies to keep geometry organized and modifiable. The short version:
- Any time you’re about to draw the same feature a second time, stop — reach for Rectangular or Circular Pattern instead
- Follow the 1 Body = 1 piece of stock principle and your drawing and fabrication workflows become dramatically faster
- In jig and weldment design, resist the urge to Boolean-merge everything — individual Bodies are an asset, not a problem to be solved