Home / Courses / Engineering Graphics and CAD / Lesson 30

Engineering Graphics and CAD · Lesson 30 of 35

Modelling machined parts; connecting CAD to processes

Model parts the way they are made and connect geometry to machining processes and their limits.

Readiness check

Learning objectives

By the end of this lesson you can:

Relate features to machining operations (drilling, milling, turning).
Model with machinable geometry (tool access, internal radii).
Explain why some geometry cannot be machined as drawn.
Add machining-aware features (relief, radii, realistic hole ends).
Connect tolerance and finish to process capability.

Check your starting point

Five to ten minutes.

Can a milling cutter (a round tool) cut a perfectly sharp internal corner into a pocket?
When you drill a hole that does not go all the way through, is its bottom flat or pointed?
Does a tighter tolerance always cost the same to machine as a loose one?

Interpretation.

Q1: No; a round cutter leaves a radius equal to its own radius in an internal corner. Skill 30.2.
Q2: Pointed (conical), because a twist drill has a pointed tip. Skill 30.4.
Q3: No; tighter tolerances need more capable, slower processes and cost more (from L13). Skill 30.4.

You need L21-L23 (features and robustness) and L13-L14 (tolerances and fits).

0 or 1 weak itemsContinue with this lesson.

2 weak itemsReview the learning objectives above, then return.

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

The core idea

What it is. Modelling machined parts means building geometry that a machining process can actually produce, and understanding which operation makes each feature. Connecting CAD to processes means matching tolerance and finish to what a process can hold.

Why an engineer needs it. A model can show geometry that no machine can cut: a perfectly sharp internal corner, a hole with a flat bottom from a twist drill, a pocket too deep and narrow for any tool. Recognizing these keeps designs manufacturable, which is exactly what the Manufacturing Processes course (for which this course is a prerequisite) builds on.

What problem it solves. It keeps modelled geometry producible and its tolerances achievable, avoiding parts that cannot be made as drawn.

What goes wrong when it is ignored. Unmachinable geometry (sharp internal corners, inaccessible features) reaches the shop and must be redesigned; over-tight tolerances beyond process capability cause scrap or expensive processes.

A simple mechanical example. A milled pocket with sharp internal corners cannot be cut, because a round end mill leaves a radius. Modelling the corners with a fillet equal to (or larger than) the tool radius makes the pocket machinable. Likewise, a blind drilled hole has a conical bottom (about a 118-degree included angle for a standard twist drill), not a flat one, so the model should reflect that where it matters.

Features and their operations:

Drilling makes round holes (with conical bottoms on blind holes).
Milling makes pockets, slots, and flats (leaving internal radii from the cutter).
Turning makes round (axisymmetric) features on a lathe.

Machinable-geometry rules (introductory):

Internal corners of milled pockets need a radius (at least the tool radius); perfectly sharp internal corners cannot be milled.
Tool access: the tool must reach the feature; deep, narrow, or shadowed features are hard or impossible.
Drilled-hole ends are conical, not flat.
Reliefs and undercuts: threads and shoulders often need a relief groove so the tool can finish cleanly.
Tolerance and finish must be within the chosen process's capability.

Part 6: Manufacturability and engineering judgement.

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

The lesson map. Modelling machined parts; connecting CAD to processes becomes manageable when you move through the four checks in order and verify each result before continuing.

The skills, taught in order

Skill 30.1 - Map features to operations

Concept. Each feature implies a machining operation. Terminology. Drilling, milling, turning, operation. Procedure. For each feature, name the operation that would make it (hole equals drill, pocket equals mill, round shaft equals turn). Reasoning. Knowing the operation reveals its geometric limits. Failure mode. Modelling geometry without considering how it is cut. Check. Name the operation for a pocket and for a round journal.

Skill 30.2 - Model machinable internal geometry

Concept. Internal corners need a tool radius; features need tool access. Terminology. Internal radius, tool radius, tool access. Procedure. Add a fillet at least the tool radius to milled internal corners, and check the tool can reach each feature. Reasoning. A round cutter cannot make a sharp internal corner, and unreachable features cannot be cut. Failure mode. Sharp internal corners or inaccessible pockets. Check. Add a tool-radius fillet to a pocket corner.

Skill 30.3 - Add reliefs and realistic ends

Concept. Threads and shoulders need reliefs; drilled holes have conical ends. Terminology. Thread relief/undercut, drill-point angle. Procedure. Add a relief groove where a thread meets a shoulder, and model a conical bottom on blind drilled holes where it matters. Reasoning. Reliefs let tools finish cleanly; the conical end reflects the real drill. Failure mode. A thread running into a shoulder with no relief, or a flat-bottomed drilled hole. Check. Add a relief where a thread meets a shoulder.

Skill 30.4 - Match tolerance and finish to process capability

Concept. Tolerance and finish must be within the process's capability. Terminology. Process capability, achievable tolerance. Procedure. Assign tolerances and finishes the chosen process can hold; tighten only where function needs it (from L13). Reasoning. Requirements beyond a process's capability cause scrap or force costly processes. Failure mode. Specifying a tolerance a process cannot achieve. Check. State whether a very tight tolerance suits a rough process.

Worked example 1: make a milled pocket machinable

Problem. A model has a rectangular milled pocket with perfectly sharp internal corners. Revise it so it can be machined, and explain the reason.

Planning. Add a fillet to each internal corner sized to a sensible cutter radius.

Solution.

Diagnose. A pocket is milled with a round end mill. A round cutter cannot reach into a perfectly sharp internal corner; it always leaves a radius equal to its own radius. So sharp internal corners are not machinable.
Choose a tool radius. Pick a sensible cutter, say a 6 mm diameter end mill (3 mm radius). The internal corners must have a radius of at least 3 mm.
Revise the model. Add a 3 mm (or slightly larger) fillet to each internal corner of the pocket. The pocket is now machinable with that cutter.
Note the mating implication. If a part must fit into the pocket with a sharp corner, that mating part needs a corner relief (a small cut) so it seats despite the pocket's radius. This is a common design detail.
Result. A pocket with tool-radius internal fillets, machinable as drawn.

Result. The pocket's sharp internal corners are replaced with fillets of at least the tool radius (3 mm for a 6 mm cutter), making it machinable; a mating part would need a corner relief.

Why the method works. Matching the internal radius to the cutter radius reflects how milling actually works, so the geometry can be produced.

How to verify independently. Check every internal corner has a radius at least the cutter radius. If any is sharp, it cannot be milled with that tool.

Worked example 2: a turned shaft with a thread relief and a realistic hole

Problem. A turned shaft has an external thread that runs up to a shoulder, and a blind drilled hole in its end. Add a thread relief so the thread can be cut cleanly, model the drilled hole with a realistic conical end, and check the bearing-seat tolerance against a reasonable turning capability. The complication combines a relief, a realistic hole end, and a tolerance-capability check.

Planning. Add a relief groove at the thread-shoulder junction, a conical-ended blind hole, and verify the seat tolerance is achievable.

Solution.

Thread relief. A single-point or die-cut thread cannot cleanly run all the way into a shoulder; the tool needs room to run out. Add a small relief groove (an undercut) at the thread-shoulder junction so the thread finishes cleanly. Model it as a shallow groove of the thread depth.
Realistic drilled hole. The blind hole is drilled, so its bottom is conical (about a 118-degree included angle for a standard twist drill). Model the conical bottom where it matters (for depth or clearance); if only the cylindrical depth matters, a note may suffice.
Bearing-seat tolerance. The journal that seats a bearing carries a fit (say H7/g6-class, from L14). Turning can hold such tolerances on a good lathe, so the seat tolerance is achievable; a much tighter tolerance might need grinding (a different, costlier process).
Capability check. Confirm the seat tolerance is within normal turning capability; if function demanded far tighter, the process (and cost) would change, which the designer should flag.
Result. A turned shaft with a thread relief, a realistically modelled drilled hole, and a seat tolerance matched to turning.

Comparison. Running the thread into the shoulder with no relief cannot be cut cleanly; a flat-bottomed blind hole misrepresents the drill; a seat tolerance beyond turning capability would force grinding. Each machining-aware detail keeps the shaft producible at reasonable cost.

Result. Add a thread relief at the shoulder, model the drilled hole's conical bottom, and keep the seat tolerance within turning capability; ignoring any of these would make the shaft harder or costlier to make.

Independent check. Confirm the thread has run-out room (a relief), the blind hole is conical (or noted), and the seat tolerance is one turning can hold. All three confirm the shaft is machining-aware.

Misconceptions and diagnostics

Misconception	Why it seems reasonable	Why it is wrong	Evidence that reveals it	Correction	Diagnostic question
"Any modelled shape can be machined."	CAD drew it.	Tool geometry and access limit what can be cut (sharp internal corners, deep narrow pockets).	A round cutter cannot make a sharp internal corner.	Model tool-radius internal corners and reachable features.	"What tool cuts this, and can it reach and shape it?"
"A blind hole has a flat bottom."	It looks flat in a sketch.	A twist drill leaves a conical bottom.	The drilled bottom is pointed, not flat.	Model the conical end (or note it).	"How is this hole actually made?"
"Tolerance is free to tighten."	Tighter sounds better.	Tolerances beyond process capability cause scrap or force costly processes.	A tolerance too tight for turning needs grinding.	Match tolerance to the process (from L13).	"Can the chosen process hold this tolerance?"

Practice ladder

Level A - Recognition

Task. For eight features, name the machining operation and flag any unmachinable geometry. Deliverable. Eight labelled features. Success criteria. At least six operations correct; unmachinable geometry flagged. Answer guidance. Hole equals drill; pocket equals mill; round equals turn. Common errors. Missing a sharp internal corner. Difficulty. Low.

Level B - Guided application

Task. Fix a scaffolded non-machinable feature (sharp corners) by adding tool-radius fillets, with prompts. Deliverable. The corrected feature. Success criteria. Internal corners have at least the tool radius. Answer guidance. Choose a cutter, fillet to its radius. Common errors. Fillet smaller than the tool radius. Difficulty. Medium.

Level C - Independent application

Task. Make a supplied part machinable independently (corners, access, reliefs, realistic holes). Deliverable. The revised part. Success criteria. All internal corners machinable; features accessible; reliefs and realistic hole ends added. Answer guidance. Work through each feature's operation and limits. Common errors. Missing a thread relief. Difficulty. Medium to high.

Level D - Transfer and design

Task. Review a part for machinability, revise it, and justify each change against tool geometry, access, and process capability. Deliverable. The revised part plus a justification. Success criteria. All machinability issues fixed; justification ties to tools and capability. Answer guidance. Consider tool, access, and tolerance for each feature. Common errors. Ignoring process capability on tolerances. Difficulty. High.

Working with AI, and proving it yourself

Use AI as a tutor

Useful AI support:

Ask it to map features to operations for a described part.
Ask it to list machinability issues to check.
Ask it to explain why sharp internal corners are not millable.

Limits:

A text assistant cannot see your model or its tool access.
It may miss a specific unmachinable feature.

Verify AI output against: tool geometry (round cutters leave radii), tool access, and process-capability limits on tolerance (from L13).

Prove it yourself

A plausible but incorrect AI answer, and how to catch it. You ask, "My pocket has sharp internal corners. Is that fine to machine?" and the assistant replies: "Yes, a mill can cut sharp internal corners."

This is wrong. Detect it with the tool-geometry principle: a milling cutter is round, so it always leaves a radius in an internal corner equal to its own radius. The evidence is geometric: no round tool fits into a zero-radius corner. Correct conclusion: add an internal fillet at least the cutter radius; sharp internal corners cannot be milled.

Retrieval and spaced review

Which operation makes a round hole? A pocket? A round journal?
Why can a mill not cut a sharp internal corner?
What shape is the bottom of a blind drilled hole?
What is a thread relief for?
How should tolerance relate to process capability?
What limits whether a feature can be machined besides its shape?
Cumulative (L13): How does the cost-versus-tolerance idea from L13 appear in process choice here?
Reconstruction task: From memory, explain how to make a sharp-cornered pocket machinable.

Answers. 1: drilling, milling, turning. 2: a round cutter leaves a radius equal to its own radius. 3: conical (from the twist-drill point). 4: to give the cutting tool room to finish the thread cleanly at a shoulder. 5: it must be within the process's capability; tighten only where function needs it. 6: tool access (the tool must reach the feature). 7: tighter tolerances force more capable, costlier processes (turning to grinding), raising cost.

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

Reference mapping and next step

Read further

Giesecke ch.9/ch.13
links to Manufacturing Processes (Course 13).

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

Finish the lesson

You can now: map features to machining operations; model machinable internal geometry and access; add reliefs and realistic hole ends; and match tolerance and finish to process capability.

Self-assessment checklist.

I know which operation makes each feature.
I add tool-radius fillets to milled internal corners.
I check tool access.
I add reliefs and realistic hole ends.
I keep tolerances within process capability.

Next lesson: L31 - Sheet-metal and fabricated parts (introduction). Why it follows: machining removes material; many parts are instead made from bent sheet. L31 introduces sheet-metal modelling and its distinct rules (constant thickness, bends, flat patterns), broadening your manufacturing judgement.

Required files or submissions: submit your Level C machinable part revision. Optional extension: take one of your models and make every internal corner and hole machining-aware.