CATIA V5 Part Design: Solid Modeling Fundamentals — From Pad & Shaft to Fillet, Draft, and Beyond

CATIA V5 · Part Design · Solid Modeling

3D solid modeling in CATIA is fundamentally about taking a 2D sketch and turning it into a physical 3D shape. You push a cross-section upward, spin it around an axis, or cut material away — and through a combination of those three ideas, you can build virtually any part.

“Push it (Pad), spin it (Shaft), cut it (Pocket/Groove), and clean up the edges (Fillet/Chamfer). That’s the whole game.”

In this post, I’ll walk through the essential Part Design features you’ll reach for every day: the commands that add material, the ones that remove it, and the finishing touches that make a model production-ready.

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1. Pad — Extruding a Sketch into a Solid

Pad takes a 2D sketch and pushes it perpendicular to the sketch plane to create a 3D solid. If you’ve used AutoCAD’s EXTRUDE command, the concept is identical.

1. Finish your sketch and click Exit Workbench to return to Part Design.
2. With the sketch selected in the spec tree, click the Pad icon.
3. In the Pad Definition dialog, enter your extrusion Length.
4. Preview the result and click OK.

Pad Type Options

Type	What It Does	When to Use
Dimension	Extrude to a specific numeric distance	The default — use this most of the time
Up to Next	Extrude until the next face is hit	Adding a feature on top of existing geometry
Up to Last	Extrude all the way through the last face	Creating a through-boss that spans the entire body
Up to Plane	Extrude until a specified reference plane	When the end face must align to a specific datum
Up to Surface	Extrude until a curved surface	When the feature needs to conform to a curved face

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2. Pocket — Cutting Material Away

Pocket is the inverse of Pad. Instead of adding material, it removes it — cutting the sketch shape into an existing solid. Use it for pockets, slots, blind holes, and recesses of all kinds.

1. Draw a sketch on the face where you want to remove material. (Circle for a round hole, rectangle for a slot, etc.)
2. Exit Workbench.
3. Click the Pocket icon.
4. Set your cut Depth in the Pocket Definition dialog.
5. Preview and click OK.

• The Type options (Up to Next, Up to Last, etc.) work identically to Pad. Up to Next stops at the next face; Up to Last cuts completely through.
• For standard round holes — especially threaded ones — the dedicated Hole command is more convenient. It handles diameter, depth, thread type, and countersink all in one dialog.

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3. Shaft — Revolving a Sketch into a Solid

Shaft takes a 2D profile and revolves it around an axis to create a rotationally symmetric solid. Cylinders, cones, discs, pipes, and anything else that’s round in cross-section — this is how you make them.

1. In your sketch, draw the cross-section profile and a separate axis line to revolve around.
2. Exit Workbench.
3. Click the Shaft icon.
4. In the Shaft Definition dialog, confirm that the correct profile and axis are selected.
5. Set First Angle / Second Angle. For a full revolution, enter 360° on one side.
6. Click OK.

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4. Groove — Revolving a Cut into Existing Geometry

Groove is Shaft’s cutting counterpart. Instead of adding material by revolving a profile, it removes material along that same rotational path. Perfect for O-ring grooves, lathe-turned recesses, and any circular channel cut.

• The workflow is identical to Shaft: sketch a profile and axis, then click the Groove icon.
• The cleanest way to remember all four: Pad adds / Pocket cuts (linear) and Shaft adds / Groove cuts (rotational).

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5. Fillet — Rounding Sharp Edges

Fillet (specifically Edge Fillet) rounds off a sharp edge on a 3D solid to a specified radius. You’ll find it in the Dress-Up Features toolbar.

1. Click the Edge Fillet icon.
2. Select one or more edges to round. (Multi-select is supported.)
3. Enter the desired Radius value.
4. Click OK.

• Propagation mode — Tangency: CATIA automatically extends the fillet to all edges that flow tangentially from your selection. You click one edge and the entire tangent chain gets filleted. Very handy on organic shapes.

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6. Chamfer — Cutting a Beveled Edge

Chamfer does the same job as Fillet — cleaning up a sharp edge — but instead of rounding it, it cuts a flat angled bevel (typically 45°).

1. Click the Chamfer icon.
2. Select the edge(s) to chamfer.
3. Choose a mode:
   • Length-Angle: Define the cut length and the angle — the most common option
   • Length-Length: Define the setback distance on each adjacent face independently
4. Click OK.

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7. Draft — Adding Taper to Faces

Draft tilts a vertical face by a specified angle to create draft angles — the slight taper that injection-molded plastic parts need so they can be ejected cleanly from the mold.

1. Click the Draft icon.
2. Faces to Draft: Select the walls you want to tilt.
3. Neutral Element: Pick the parting face or reference plane that stays fixed. Everything measured from here gets tilted.
4. Angle: Enter the draft angle (typically 1–3° for injection-molded parts).

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8. Fillet and Chamfer Order — Why Save Them for Last?

One of the most common beginner mistakes in Part Design is adding fillets and chamfers as soon as the edge exists.

• If you fillet an edge and then later cut a Pocket through it, the geometry can become tangled — CATIA’s kernel struggles to calculate where the filleted face ends and the pocket begins, and you end up with unpredictable errors.
• If you need to go back and edit a sketch later, a Fillet sitting in the middle of the spec tree can block the update or throw cascading errors on everything below it.

The recommended modeling order that keeps your tree clean and modification-friendly:

1. Build the base geometry — Pad, Pocket, Shaft to establish the main body
2. Add secondary features — holes, slots, patterns
3. Apply Draft — only if it’s a molded part
4. Fillets and Chamfers last — always at the bottom of the tree

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9. Editing Sketches and Managing the Spec Tree

9-1. How to Edit an Existing Sketch — Double-Click Twice

Need to change the size of a solid you’ve already created? You have to reach back into the original sketch that defined it.

1. Double-click the feature (e.g., Pad.1) in the spec tree → the Pad Definition dialog opens.
2. Inside the dialog, double-click the sketch name (e.g., Sketch.1) → you drop straight into the Sketcher.
3. Edit your dimensions, click Exit Workbench, and every dependent feature below updates automatically.

9-2. Spec Tree Management — Habits That Pay Off Later

CATIA is a history-based modeler: it evaluates the spec tree top-to-bottom every time you make a change. A messy tree today becomes a nightmare to debug six months later.

• Rename features immediately: Click a feature, press F2, and give it a meaningful name — “Base_Plate”, “M8_Hole”, “Mounting_Boss”. Once you’re past 20–30 features, default names like Pad.7 are useless.
• Deactivate instead of delete: Right-click → Deactivate temporarily switches a feature off without removing it. Great for checking what the part looks like without a particular hole or slot — just reactivate when done.
• Reorder by dragging: You can drag features up and down the tree to change the evaluation order. Be careful with dependencies — moving a Fillet above the Pocket it’s applied to will cause an error.

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Wrapping Up

The individual commands aren’t complicated — what separates an experienced CATIA designer from a beginner is knowing when to use each one and in what order. Here’s the short version:

• Pad / Shaft to build, Pocket / Groove to cut — everything else is a variation on those four
• Fillets and Chamfers go at the very bottom of the spec tree — always, without exception
• When something breaks or the geometry looks wrong, Define In Work Object is your first stop — trace back through the timeline until you find where it went sideways

Get these fundamentals solid and CATIA’s more advanced surfacing and assembly tools will make a lot more sense when you get there.