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Engineering Graphics and CAD · Lesson 21 of 35

Solid features: extrude, revolve, cut, hole, fillet, chamfer

Turn constrained sketches into solids with the core feature set and understand each feature's parameters.

Readiness check

Learning objectives

By the end of this lesson you can:

Create extrude and revolve features with correct end conditions.
Remove material with cut and the hole tool.
Apply fillets and chamfers appropriately.
Choose add versus remove and the right end condition for robustness.
Order fillets and chamfers late in the feature tree.

Check your starting point

Five to ten minutes.

To make a shaft (a round part), would you extrude a circle or revolve a profile? Why might revolve be better?
If you extrude a boss "blind" to a set depth, and later make the base thicker, does the boss still reach the top?
Should you round the edges early or late when modelling?

Interpretation.

Q1: Either can work, but revolving a profile about the axis captures the round shape in one feature and makes diameters easy to edit. Skill 21.1 explains.
Q2: Not necessarily; a blind depth is fixed, so it may no longer reach. An "up-to-face" end condition would. Skill 21.1 covers end conditions.
Q3: Late. Fillets and chamfers are finishing features; adding them late keeps earlier references clean. Skill 21.3.

You need L20 (fully constrained sketches to build from).

0 or 1 weak itemsContinue with this lesson.

2 weak itemsReview Lesson 20, then return.

3 or more weak itemsWork through the prerequisite examples before continuing.

The core idea

What it is. Solid features turn sketches into 3D geometry and modify it. The core set is extrude and revolve (to add or remove material), the hole tool (to make standard holes), and fillet and chamfer (to finish edges). Each has parameters, including end conditions that control how far a feature goes.

Why an engineer needs it. These few features build most mechanical parts. Choosing the right feature and end condition makes a model both correct and robust: an "up-to-face" cut still reaches when the part changes size, while a fixed-depth cut may not.

What problem it solves. It converts 2D profiles into editable 3D solids with control over how features relate to the rest of the part.

What goes wrong when it is ignored. Wrong end conditions make features that break when the part is resized; fillets added too early complicate later references; using a plain cut instead of the hole tool loses the standard callout.

A simple mechanical example. The L-bracket is an extrude (the L profile), a hole (the mounting hole), and a fillet (a rounded inner corner). The flanged shaft is a revolve (the stepped round profile) with a chamfer on its lead end and a fillet at its shoulder.

The feature set:

Extrude: push a profile straight to make or cut a solid. End conditions: blind (a set depth), through-all (all the way), up-to-face (to a chosen face), symmetric (equal both ways).
Revolve: spin a profile about an axis to make round parts; an angle less than 360 makes a partial revolve.
Cut (extrude-cut): the same as extrude, but removing material.
Hole tool: makes standard holes (simple, counterbore, countersink, tapped) with the callouts from L16.
Fillet (rounds an edge) and chamfer (bevels an edge): finishing (dress-up) features, placed late.

End conditions matter for robustness. Prefer an end condition that follows the part (up-to-face, through-all) over a fixed blind depth when the feature should track another face, so edits do not break it.

Order fillets and chamfers late. These modify existing edges, so adding them after the main shape keeps early features simple and their edges available as clean references.

Neutral terminology: extrude, revolve, fillet, and chamfer are named the same across Onshape, SolidWorks, Fusion, NX, Creo, and CATIA; the hole tool is the "Hole" feature in most.

Part 4: Parametric CAD foundations.

Check: explain the decision in your own words before using a CAD command.

The lesson map. Solid features: extrude, revolve, cut, hole, fillet, chamfer becomes manageable when you move through the four checks in order and verify each result before continuing.

The skills, taught in order

Skill 21.1 - Extrude and revolve with the right end condition

Concept. Add or remove material by extruding a profile or revolving it, choosing an end condition that suits the intent. Terminology. Extrude, revolve, end condition (blind, through-all, up-to-face, symmetric), revolve angle. Procedure. Extrude linear profiles, revolve round ones. Choose blind for a fixed size, through-all or up-to-face when the feature should follow the part, symmetric to build both ways from the plane. Reasoning. End conditions determine whether a feature survives resizing. Failure mode. Using blind depth where up-to-face is meant, so the feature no longer reaches after an edit. Check. State which end condition keeps a cut passing fully through a wall of changing thickness (through-all).

Skill 21.2 - Remove material with cut and the hole tool

Concept. Cut removes material; the hole tool makes standard holes with callouts. Terminology. Cut/extrude-cut, hole tool, counterbore, countersink, tapped. Procedure. Use a cut for general removal; use the hole tool for round holes so the standard callout (from L16) is carried. Reasoning. The hole tool encodes the standard feature and its documentation, not just a round cut. Failure mode. Cutting a plain circle where a counterbored or tapped hole is intended, losing the callout. Check. Choose the tool to make a counterbored screw hole (hole tool).

Skill 21.3 - Apply and order fillets and chamfers

Concept. Fillets round edges and chamfers bevel them; both are finishing features placed late. Terminology. Fillet, chamfer, dress-up feature. Procedure. Build the main shape first; add fillets and chamfers near the end of the tree, selecting the edges to modify. Reasoning. Late placement keeps early edges clean for references and avoids complicating the base shape. Failure mode. Filleting early, then referencing the changed edge, creating fragile dependencies. Check. State why a fillet belongs late in the tree.

Skill 21.4 - Choose add versus remove deliberately

Concept. Decide whether each feature adds or removes material to build the shape efficiently. Terminology. Boss/add, cut/remove. Procedure. Start from a base solid, then add bosses and remove cuts/holes to reach the final shape. Reasoning. A clear add/remove sequence keeps the model simple and legible. Failure mode. Overcomplicating with unnecessary features. Check. For a slotted block, decide which features add and which remove.

Worked example 1: model the L-bracket

Problem. Model the L-bracket: extrude the fully constrained L profile to a width of 30, cut a mounting hole of diameter 12 in the foot with the hole tool, and add a fillet of radius 5 to the inside corner.

Planning. Extrude the base, place the hole with the hole tool, then add the fillet last.

Solution.

Extrude the base. Take the fully constrained L profile (from L20) and extrude it 30 (the bracket width). Use a blind 30 depth, since the width is a fixed design size. This is feature 1.
Cut the mounting hole. On the foot's top face (or from a plane), use the hole tool to make a diameter-12 hole through the foot. The hole tool carries the callout (diameter 12, through). This is feature 2.
Add the fillet. Select the inside corner edge of the L and add a fillet of radius 5. Place it last, after the shape and hole are done. This is feature 3.
Order rationale. Base (shape) first, hole (function) second, fillet (finish) last, so the fillet does not complicate the hole's placement or the base's edges.
Result tree. Extrude, hole, fillet: three clean features.

Result. A modelled L-bracket: an extruded L base 30 wide, a diameter-12 mounting hole from the hole tool, and a radius-5 inside fillet added last.

Why the method works. Building shape, then function, then finish keeps each feature's references clean and the tree easy to edit.

How to verify independently. Edit the foot length: the hole (placed from the foot) and the fillet should update cleanly if referenced well. If the fillet or hole errors, its reference needs revisiting (a preview of L23).

Worked example 2: model the flanged shaft, revolve versus extrudes

Problem. Model the flanged shaft (a round part: a flange, then a shaft body, then a smaller journal, stepping down in diameter) by revolving a profile, and add a chamfer to the lead end and a fillet at a shoulder. Compare this with building the shaft as a stack of extruded cylinders. The complication is choosing the modelling approach for a round part.

Planning. Revolve a stepped half-profile about the axis; add the chamfer and fillet last. Then contrast with stacked extrudes.

Solution.

Revolve approach. Sketch the shaft's half-profile (the outline of one side, from the axis outward: flange radius and width, body radius and length, journal radius and length) on a plane containing the axis. Fully constrain it. Revolve it 360 degrees about the axis. One feature produces the whole stepped round shaft.
Chamfer and fillet. Add a chamfer (say 2 by 45 degrees) to the lead end of the journal to start a nut or bearing, and a fillet (say radius 3) at the shoulder between body and journal to reduce stress. Place both last.
Stacked-extrude alternative. Alternatively, extrude a flange cylinder, then extrude a body cylinder on its face, then a journal cylinder on that. Three add features plus the chamfer and fillet.
Compare. The revolve captures the whole axisymmetric shape in one feature, and editing any diameter or length is a single sketch edit; it directly expresses "this is a round, stepped shaft." The stacked extrudes use more features, each depending on the previous face (more parent-child links), and diameters are edited in separate features.
Choose revolve. For an axisymmetric part, revolve is usually cleaner and more robust: one intentional profile, easy diameter edits, fewer dependencies.

Comparison. Revolve models the round shaft as one profile (clean, editable, few dependencies); stacked extrudes use more features and more parent-child links. For axisymmetric parts, revolve better expresses and maintains the design. (Stacked extrudes can still be reasonable for parts that are not purely axisymmetric.)

Result. Revolve the stepped half-profile for the flanged shaft, then add the lead chamfer and shoulder fillet last; revolve is preferred over stacked extrudes for this axisymmetric part.

Independent check. Change the journal diameter: with the revolve, it is one sketch dimension edit and the chamfer/fillet update; with stacked extrudes, it is a separate feature edit. The single clean edit confirms revolve's advantage here.

Misconceptions and diagnostics

Misconception	Why it seems reasonable	Why it is wrong	Evidence that reveals it	Correction	Diagnostic question
"Always extrude blind to a fixed depth."	It is simple and explicit.	Blind depth does not follow the part; up-to-face or through-all survive resizing.	A blind cut stops short after the wall thickens.	Use up-to-face or through-all when the feature should follow the part.	"Should this feature follow another face, or stay a fixed size?"
"A plain circular cut equals a hole."	Both make a round hole.	The hole tool carries the standard callout (counterbore, tapped); a plain cut does not.	The drawing lacks the hole callout.	Use the hole tool for standard holes.	"Does this hole need a standard callout?"
"Add fillets early."	Round it as you go.	Early fillets change edges that later features reference, creating fragility.	A later feature breaks when the fillet changes.	Add fillets and chamfers late.	"Is this a finishing feature that should come last?"

Practice ladder

Level A - Recognition

Task. Match eight features to the correct tool (extrude, revolve, cut, hole, fillet, chamfer) and end condition. Deliverable. Eight matches. Success criteria. At least six correct. Answer guidance. Round parts revolve; standard holes use the hole tool; edges get fillets/chamfers. Common errors. Using extrude for an axisymmetric part where revolve is cleaner. Difficulty. Low.

Level B - Guided application

Task. Model a scaffolded extrude-plus-cut part, choosing end conditions, with prompts. Deliverable. The modelled part. Success criteria. Correct features and end conditions; hole tool used for the hole. Answer guidance. Prefer through-all/up-to-face where the feature should follow the part. Common errors. Blind depth where through-all is meant. Difficulty. Medium.

Level C - Independent application

Task. Model the flanged shaft (Project P3) by revolve, adding a lead chamfer and a shoulder fillet. Deliverable. The modelled shaft. Success criteria. One revolve for the body; chamfer and fillet added last; diameters editable from the profile. Answer guidance. Sketch the half-profile about the axis; finish features last. Common errors. Building the shaft as many extrudes when revolve is cleaner. Difficulty. Medium.

Level D - Transfer and design

Task. For a supplied part, choose features and end conditions for robustness and justify each choice against a likely edit. Deliverable. The model plus a justification. Success criteria. Features and end conditions survive the stated edits; justification is sound. Answer guidance. Match end conditions to how the feature should track the part. Common errors. Fixed blind depths that break on resizing. Difficulty. Medium to high.

Working with AI, and proving it yourself

Use AI as a tutor

Useful AI support:

Ask it to explain end conditions and when each is robust.
Ask it to suggest features for a described part, then check for robustness.
Ask it to compare revolve and extrude for a round part.

Limits:

A text assistant cannot see whether your end conditions survive edits.
It may default to blind depths.

Verify AI output against: the end-condition robustness principle, the hole-tool-for-standard-holes rule, and the fillets-late rule.

Prove it yourself

A plausible but incorrect AI answer, and how to catch it. You ask, "Should I fillet all the edges first so the model looks finished, then add the holes?" and the assistant replies: "Yes, add all fillets first so the shape is complete before detailing."

This creates fragile references. Detect it with the order rule: fillets modify edges, and holes or features referenced to a filleted edge break when the fillet changes. The evidence is the edit test: change a fillet radius and a hole placed on that edge errors. Correct conclusion: build the shape and functional features first, add fillets and chamfers late.

Retrieval and spaced review

When would you revolve rather than extrude?
Name the four extrude end conditions.
Why use the hole tool instead of a plain cut?
Why add fillets and chamfers late?
Which end condition keeps a cut through a wall of changing thickness?
What is the difference between a fillet and a chamfer?
Cumulative (L20): Why must the sketch be fully constrained before extruding or revolving?
Reconstruction task: From memory, list the three features of the L-bracket in order.

Answers. 1: for axisymmetric (round) parts, to capture the shape in one editable profile. 2: blind, through-all, up-to-face, symmetric. 3: it carries the standard hole callout (counterbore, countersink, tapped). 4: they modify edges, so late placement keeps earlier references clean. 5: through-all. 6: a fillet rounds an edge; a chamfer bevels it. 7: an under-constrained sketch can shift, making the feature unpredictable; a fully constrained sketch gives a deterministic feature.

Suggested review intervals. 1 day, 3 days, 7 days.

Reference mapping and next step

Read further

Onshape docs (features)
Giesecke ch.5.

Standards details must be checked against the current official edition used by your institution or employer.

Finish the lesson

You can now: extrude and revolve with correct end conditions; cut and use the hole tool; apply fillets and chamfers; and order finishing features late.

Self-assessment checklist.

I choose extrude or revolve by the part's shape.
I pick end conditions for robustness (up-to-face, through-all).
I use the hole tool for standard holes.
I add fillets and chamfers late.
I sequence add and remove features deliberately.

Next lesson: L22 - Patterns, mirrors, and repeated geometry. Why it follows: many parts repeat features (bolt circles, rows of holes, symmetric ribs). Rather than modelling each by hand, you will create them as parametric patterns and mirrors that update together.

Required files or submissions: submit your Level C flanged-shaft model (Project P3). Optional extension: in Onshape, model the L-bracket and confirm the fillet updates when you change the foot length.