Size shafts, bolted joints and bearings, model parts parametrically, read GD&T, sanity-check FEA, choose manufacturing processes, design for manufacturing, compute Cpk and prepare parts for 3D printing.

Machine Design & Manufacturing

## Why it matters

A part's cost, strength, accuracy and lead time depend as much on **how it is made** as on its shape. The same bracket might cost a few dollars as a stamped steel part in a run of 100,000, or many times that machined from solid aluminium as a one-off. Designers who understand processes choose sensible ones early and avoid designing parts that are expensive or impossible to make.

## The main process families

**Machining (subtractive).** Material is cut away from a solid block or bar: milling, turning (lathe), drilling, grinding. CNC machines follow programs generated by CAM software.
- Strengths: tight tolerances (around ±0.05 mm is routine on many features, and much tighter is possible at a cost), good surface finish, almost any metal or engineering plastic, no tooling cost.
- Limits: material waste, cost per part stays fairly high, internal shapes limited by tool access (cutters are round, so inside corners have a radius).

**Casting (formative, liquid).** Molten metal is poured or injected into a mould.
- *Sand casting*: cheap moulds, large parts, rough surface and loose tolerances (often around ±1 mm or more on bigger dimensions), usually machined afterwards on critical faces.
- *Investment casting*: fine detail and good finish, moderate tooling.
- *Die casting* (aluminium, zinc, magnesium): steel dies are expensive, but parts come out fast and accurate. Suits high volumes.

**Forming (solid).** Forging hammers or presses hot or cold metal into shape, giving excellent strength because the grain flow follows the shape (crankshafts, connecting rods, hand tools). Sheet metal work (cutting, punching, bending, stamping) makes enclosures, brackets and panels cheaply, especially with progressive dies at high volume.

**Injection moulding (plastics).** Molten plastic is injected into a steel or aluminium mould. Moulds are costly (from a few thousand to well over a hundred thousand dollars) and take weeks to make, but each part costs very little and cycles take seconds. Designs need uniform walls, draft angles and no undercuts unless the mould has side actions.

**Additive manufacturing (3D printing).** Parts are built layer by layer: FDM (plastic filament), SLA (resin), SLS/MJF (nylon powder), metal powder-bed fusion. No tooling, complex internal shapes are possible, but parts are slower to make, cost more per part at volume, and properties can differ by build direction. A later lesson covers it.

**Joining.** Welding, brazing, adhesives and fasteners turn several simple parts into an assembly. Sometimes a welded assembly of plate is cheaper than one complex casting.

## Volume and tooling: the break-even idea

Processes trade **fixed cost** (tooling, setup, programming) against **cost per part**. A simple model:

```text
total cost = tooling + (cost per part * quantity)
break-even quantity = (tooling_B - tooling_A) / (per_part_A - per_part_B)
```

Example: a plastic housing can be CNC machined for $15.00 each with no tooling, or injection moulded for $0.50 each after a $20,000 mould.

```text
break-even = (20,000 - 0) / (15.00 - 0.50) = 1,379 parts
```

Below about 1,400 parts, machining is cheaper; above it, moulding wins, and it wins by more as volume grows. Real quotes add lead time, mould maintenance, material and finishing, but the shape of the decision is the same.

## How to choose

Ask these questions in roughly this order:

1. **Quantity.** One, a hundred, ten thousand or a million? This narrows the field fastest.
2. **Material.** Does the function need steel, aluminium, a specific plastic? Some processes only work with some materials.
3. **Geometry and size.** Thin walls, internal channels, large flat plates, round parts (turning) or prismatic parts (milling)?
4. **Tolerance and finish.** Tight fits usually mean machining, at least on the critical features.
5. **Strength and loading.** Forgings and machined wrought metal usually beat castings for fatigue-critical parts.
6. **Lead time and budget.** Tooling takes weeks; machining and printing can take days.

Often the answer is a **combination**: cast or forge near shape, then machine the bearing bores and mating faces.

## A note on shop safety

Machine tools, presses, foundries and moulding machines can cause severe injuries: entanglement in rotating spindles and chucks, flying chips, crushing, burns and fumes. This lesson is awareness only. Never operate shop equipment without the training, supervision and guarding your school, makerspace or employer requires.

## Common mistakes

- **Designing for machining, then moulding the part.** Sharp inside corners and uneven walls that are fine for CNC cause sink marks and warping in moulding.
- **Ignoring the break-even.** Ordering an injection mould for 200 parts, or machining 50,000 of a part that could be stamped.
- **Tight tolerances everywhere.** Only the functional features need them.
- **Forgetting secondary operations.** Castings usually need machining; most parts need deburring, finishing or coating.

## Recap

- Machining: accurate, no tooling, higher cost per part.
- Casting, forging, stamping and moulding: tooling up front, cheap parts at volume.
- Additive: no tooling, complex shapes, best at low volume.
- Choose by quantity, material, geometry, tolerance, strength and lead time; break-even analysis compares options.

## Try it

The Do tab has a quiz on matching parts to processes and working out a break-even quantity.


Compare machining, casting, forming, moulding and additive processes, and use break-even analysis to choose between them.

Manufacturing processes

How Things Are Made | An Animated Introduction to Manufacturing Processes

Plastic Injection Molding

Write down the part's function: what it holds, what it mates with, and which features really need tight tolerances.

Pick the intended process and quantity (for example, CNC machining, 50 parts in aluminium 6061).

Check every inside corner: is its radius larger than a standard cutter radius? Mark any that are sharp.

Check pocket and hole depths against tool diameter (aim for about 3 to 4 times diameter or less) and hole sizes against standard drill and tap sizes.

Count the setups: list the faces with features. Move or remove features to reduce the number of faces that need machining.

List every toleranced dimension. Keep tight tolerances only on functional features and put the rest under a general tolerance note (for example ISO 2768-m).

Count fastener types and parts in the assembly. Could any parts be combined or fasteners standardised?

Update the model or sketch with your changes, and write a before/after list of what changed and why.

Optional: upload both versions to an online quoting service (no order needed) and compare the instant prices and DFM warnings.

## Why it matters

Most of a product's cost is locked in during design, long before anyone cuts metal. A feature that takes a designer ten seconds to draw can add a second machine setup, a special tool or a scrapped mould. **Design for manufacturing (DFM)** means designing parts that are easy to make well, and **design for assembly (DFA)** means making them easy to put together. Good DFM does not make parts worse; it removes cost and risk that add nothing to function.

## DFM for CNC machining

- **Inside corner radii.** Milling cutters are round, so pockets always have radiused inside corners. Give inside corners a radius a little larger than a standard cutter radius (for example, R3.5 mm when a 6 mm cutter is used) so the tool does not have to stop in the corner.
- **Pocket depth.** Deep, narrow pockets need long tools that deflect and chatter. A common rule of thumb is to keep pocket depth within about 3 to 4 times the cutter diameter.
- **Standard hole sizes.** Use standard drill and tap sizes. Specify thread depth rather than threading to the bottom of a blind hole, and give tapped holes room for the drill point.
- **Minimise setups.** Every time the part is flipped or re-clamped costs time and adds error. Put features on as few faces as possible.
- **Wall thickness.** Very thin walls vibrate and bend during cutting. In metals, walls under about 1 mm are difficult; plastics need more.
- **Tolerance only what matters.** Use a general tolerance note (such as ISO 2768-m) for everything else.

## DFM for sheet metal

- Keep **bend radii** at or above the material thickness for most steels and aluminium, and use the same radius throughout so one tool does all bends.
- Keep holes at least about 2 times the thickness away from bends, or they distort.
- Add **bend reliefs** where a bend meets an edge to stop tearing.

## DFM for injection moulding

- **Uniform wall thickness.** Thick sections cool slowly, causing sink marks, voids and warping. Core out thick regions and use ribs instead.
- **Draft.** Add a draft angle (often 1 to 2 degrees, more for textured surfaces) to walls in the direction the mould opens so the part releases.
- **Ribs** are typically about 50 to 60 % of the wall thickness they join to avoid sink on the other face.
- **Avoid undercuts** that need side actions in the mould, or design snap fits that can be moulded simply.

## DFA in brief

- **Fewer parts.** Ask of each part: does it move relative to its neighbours, does it need a different material, or does it have to come apart for service? If not, it might be combined with another.
- **Fewer fastener types.** One screw size throughout means one driver and fewer mistakes.
- **Self-locating features** (pins, tabs, chamfers) and **mistake-proofing** (poka-yoke): parts that only fit one way.
- **Top-down assembly** so gravity helps.

## Worked example: improving a machined bracket

A first design of an aluminium bracket has:

1. A rectangular pocket 40 mm deep with **sharp inside corners**.
2. Tapped holes on **four different faces**.
3. Every dimension at **±0.01 mm**.
4. Two M5 and two M6 tapped holes.

Improvements:

1. Add R5 inside corner radii (a little larger than the 4 mm radius of an 8 mm cutter) and, if function allows, reduce the pocket depth to 24 mm so a standard 8 mm cutter stays within about 3 times its diameter.
2. Move the holes onto two opposite faces, so the part needs two setups instead of four.
3. Keep ±0.01 mm only on the bore that locates a bearing; put the rest under a general tolerance note.
4. Use four M6 holes, so one tap and one screw size cover the assembly.

Each change is small; together they can cut machining time substantially. The best way to confirm is to ask a machinist or get quotes before and after: many online manufacturing services give instant quotes and automated DFM feedback.

## Talk to the people who make it

Machinists, toolmakers and moulders know what is easy and what is expensive. Showing them a design early, and asking "what would make this easier to make?", is one of the most valuable habits an engineer can build. Their workshops are also hazardous places: visit with permission, wear the required PPE and never touch machines you have not been trained and authorised to use.

## Common mistakes

- **DFM at the end.** By the time a design is "finished", changes are expensive.
- **Copying a part designed for another process.** A machined design rarely moulds well.
- **Cutting cost by removing function.** DFM keeps the function and removes the waste.
- **Ignoring inspection.** A feature you cannot measure is a feature you cannot accept.

## Recap

- Design inside corners, pocket depths, holes and walls for the tools that will make them.
- Sheet metal: consistent bend radii, holes away from bends, reliefs.
- Moulding: uniform walls, draft, thin ribs, no unnecessary undercuts.
- DFA: fewer parts, fewer fastener types, self-locating, mistake-proof.

## Try it

On the Do tab, review a part design against a DFM checklist and redesign it in CAD or on paper.


Apply DFM and DFA rules for machining, sheet metal and moulding to make a part cheaper and easier to make without losing function.

Design for manufacturing

What is Design for Manufacturing? DFM (engineer must know)

How to Design Parts for CNC Machining

## Why it matters

No two manufactured parts are identical. Tool wear, temperature, material batches and operators all add variation. Quality engineering asks two questions: **is the process stable**, and **is it capable** of making parts inside the tolerance? Customers, especially in automotive, aerospace and medical work, often require proof in the form of capability indices such as **Cpk**. As a design engineer you need to read these numbers, because they tell you whether your tolerances can actually be met.

## Inspection basics

- **Measuring tools**: calipers (good to about 0.02 mm with care), micrometers (0.001 to 0.01 mm), height gauges, pin and thread gauges, go/no-go gauges, and coordinate measuring machines (CMMs) for GD&T.
- **A gauge must be much better than the tolerance.** A common rule of thumb is that measurement uncertainty should be no more than about 10 % of the tolerance (sometimes 25 % is accepted). A caliper is not the right tool for a ±0.005 mm bore.
- **Gauge R&R** (repeatability and reproducibility) studies check how much of the observed variation comes from the measurement system itself.
- **First article inspection** checks every dimension on the first part off a new process before production starts.

## Statistical process control (SPC)

SPC watches a process over time with **control charts**. The common X-bar and R chart takes small subgroups (often 5 consecutive parts) at regular intervals and plots each subgroup's mean and range. Control limits (roughly ±3 sigma of the process) come from the data, not from the drawing. A point outside the limits, or patterns such as long runs on one side of the centre line, signal a **special cause** (a worn tool, a new material lot) to investigate.

Control limits and specification limits are different things. A process can be in control (stable) but not capable (its natural spread is wider than the tolerance), or capable but drifting out of control.

## Capability indices

For a feature with lower and upper specification limits LSL and USL, process mean mu and process standard deviation sigma:

```text
Cp  = (USL - LSL) / (6 * sigma)                  potential: spread vs tolerance
Cpk = min(USL - mu, mu - LSL) / (3 * sigma)       actual: also accounts for centring
```

- Cp ignores where the process is centred; Cpk uses the distance to the **nearest** limit.
- Cpk is never larger than Cp. They are equal only when the process is perfectly centred.
- Cpk = 1.0 means the nearest limit is 3 sigma away (roughly 0.13 % out of spec on that side if the data are normal). Many customers ask for **Cpk >= 1.33** (4 sigma), and often 1.67 for critical features. Check the customer's requirements.

**Which sigma?** Strictly, Cp and Cpk use the short-term, **within-subgroup** sigma, often estimated as R-bar / d2 (d2 = 2.326 for subgroups of 5). Using the overall sample standard deviation of all the data gives the **performance** indices **Pp and Ppk**. The two are close for a stable process and differ when the process drifts between subgroups. Capability indices also assume the process is stable and the data are roughly normal; check the control chart first.

## Worked example 1: by hand

A shaft diameter is specified as 25.00 ± 0.05 mm, so LSL = 24.95 and USL = 25.05. The process mean is 25.02 mm and sigma is 0.01 mm.

```text
Cp  = (25.05 - 24.95) / (6 * 0.01)               = 0.10 / 0.06 = 1.67
Cpk = min(25.05 - 25.02, 25.02 - 24.95) / 0.03   = min(0.03, 0.07) / 0.03 = 1.00
```

The spread is fine (Cp 1.67), but the process runs 0.02 mm high, so it fails a 1.33 Cpk requirement. **Re-centring** the process (an offset on the CNC) would fix it without buying a better machine. That is the value of comparing Cp with Cpk.

## Worked example 2: from data

The Do tab holds 40 measured diameters in 8 subgroups of 5. Their mean is about 25.013 mm and the average subgroup range is about 0.0184 mm, so:

```text
sigma_within = R-bar / d2 = 0.0184 / 2.326 = 0.0079 mm
Cp  = 0.10 / (6 * 0.0079)              = 2.11
Cpk = (25.05 - 25.013) / (3 * 0.0079)  = 1.57
```

Here the process is capable and only slightly off centre.

## Design takeaways

- **Tolerances set the denominator.** If the process cannot hold a tolerance with Cpk >= 1.33, either the tolerance, the process, or the design has to change.
- **Talk to quality early** about which features are critical-to-quality and how they will be measured.
- **Tolerance stack-ups** add variation from several parts; a statistical (root-sum-square) stack assumes capable, centred processes, so it depends on these numbers.

## Common mistakes

- **Computing Cpk on an unstable process.** The number means nothing if the process is drifting.
- **Confusing control limits with specification limits.**
- **Tiny samples.** Capability from 10 parts is very uncertain; studies commonly use at least 25 subgroups or 100 or more parts.
- **Measurement system too coarse.** If the gauge cannot resolve the variation, the sigma you compute is mostly gauge noise.

## Recap

- Inspection needs gauges much better than the tolerance; Gauge R&R checks this.
- SPC control charts show stability; capability indices show fit within the tolerance.
- Cp = (USL − LSL)/6σ; Cpk = nearest-limit distance / 3σ; Cpk ≤ Cp.
- Cp and Cpk use within-subgroup sigma; Pp and Ppk use the overall sigma.

## Try it

On the Do tab, finish the Cpk function and compare Cp, Cpk and Ppk for the measured shaft data.


Choose suitable gauges, read control charts, and compute Cp, Cpk and Ppk for a machined feature.

Quality and inspection

PROCESS CAPABILITY: Explaining Cp, Cpk, Pp, Ppk and HOW TO INTERPRET THOSE RESULTS

What is Cpk (Simple Explanation of Cp and Cpk)

Pick a part: the L-bracket from Parametric CAD, or a simple clip that fits over a 20 mm tube.

Add a parametric clearance variable for any fit (start with 0.4 mm on diameter) and model a small test coupon with openings at +0.0, +0.2, +0.4 and +0.6 mm.

Export the part and the coupon as 3MF (or STL) and import them into the slicer. Check the dimensions shown in the slicer match the CAD model in millimetres.

Orient the part so it sits on a large flat face, overhangs stay under about 45 degrees, and the main load runs along the layers, not across them.

Choose a material profile (PLA or PETG), 0.2 mm layers, 3 to 4 perimeters and 20 to 40 % infill. Add supports only where the preview shows unsupported areas.

Slice and step through the layer preview. Look for gaps, unsupported islands and thin walls. Record the estimated time and material.

Change the orientation once and slice again. Compare time, material and the amount of support.

Write a short print plan: settings, orientation and what question the prototype will answer (fit, function or looks).

## Why it matters

A prototype answers questions that CAD cannot: does it fit, does it feel right, does the mechanism move, will the customer understand it? **Rapid prototyping** makes those answers cheap and fast. Desktop 3D printers, laser cutters and online quoting services let an engineer hold a part days or even hours after modelling it. The skill is knowing what question each prototype should answer, and preparing the part so the print is right the first time.

## Kinds of prototype

- **Looks-like**: appearance and ergonomics (often printed and painted).
- **Works-like**: mechanism and function, often ugly.
- **Fit check**: does it assemble with the real mating parts?
- **Engineering or pre-production**: made with (or close to) the production process and material for testing.

A 3D-printed prototype rarely matches a production part's strength. Printed parts are usually weaker between layers than along them, and plastics creep under load. Use printed parts to answer geometry and function questions; test production-intent parts for strength.

## Common processes

- **FDM / FFF** (fused filament): melts plastic filament (PLA, PETG, ABS, nylon). Cheap and widely available; visible layer lines; parts are weakest between layers.
- **SLA / resin**: cures liquid resin with light. Fine detail and smooth surfaces; parts can be brittle; uncured resin is a skin and eye irritant, so handle it with gloves and follow the resin maker's safety data sheet.
- **SLS / MJF** (powder bed nylon): strong, no support structures needed, usually through a service bureau.
- **Metal printing**: powder-bed fusion for complex metal parts; expensive and usually a service.
- **Laser cutting and CNC routing** of flat sheet are also rapid prototyping, and often faster for flat parts.

## Preparing a part for FDM printing

1. **Export correctly.** Export STL or 3MF from CAD. Check the **units** when you import into the slicer (a 50 mm part arriving as 50 inches or 0.05 mm is a classic error). 3MF stores units; STL does not.
2. **Check the mesh** is closed (watertight). Most slicers warn about errors and can repair simple ones.
3. **Orient the part.** Choose a large flat face on the bed; keep overhangs small; and, because layers are weakest in tension between them, orient so the main load runs along the layers, not across them.
4. **Overhangs and supports.** Most FDM printers handle overhangs up to about 45 degrees from vertical without support. Steeper overhangs and bridges longer than roughly 10 mm (it varies by printer) need supports, which leave rough surfaces.
5. **Holes and fits.** Printed holes usually come out undersize. Add clearance (often roughly 0.2 to 0.4 mm on diameter for a sliding fit, depending on the printer) or drill or ream to size afterwards. Better: print a small **test coupon** with a range of hole sizes first.
6. **Walls and infill.** Strength comes mostly from perimeters (walls), not infill. Three or four perimeters with 20 to 40 % infill is a common starting point for functional parts.
7. **Slice and preview.** Check the layer preview for gaps, unsupported islands and estimated time and material.

## Worked example: a sensor bracket

A small PETG bracket must clip over a 20.0 mm aluminium tube. If we model the clip at exactly 20.0 mm, a printed hole will likely come out a little small and the tube will not fit. Print a coupon with openings of 20.0, 20.2, 20.4 and 20.6 mm first, find the one that slides on firmly (say 20.4 mm on this printer), then set that as a **parametric variable** (`tube_clearance = 0.4 mm`) in the CAD model. When the design moves to injection moulding later, change the variable back to the moulding clearance rather than redrawing.

## Safety and good practice

- Printer nozzles (around 200 to 260 °C) and heated beds are hot enough to burn; keep hands clear while printing.
- Some filaments, especially ABS and ASA, release fumes and particles while printing. Print in a ventilated space or an enclosure with filtration, following the manufacturer's guidance.
- Never leave a printer running unattended unless your space's rules allow it.
- Follow your school, makerspace or employer's equipment rules and training requirements.

## Free and low-cost tools

- **PrusaSlicer**, **Cura** and **OrcaSlicer** are free slicers. You can slice and preview a part, including time and material estimates, without owning a printer.
- Libraries, schools and makerspaces often have printers you can use after an induction.
- Online manufacturing services give instant quotes for printing, CNC and moulding by uploading a model.

## Common mistakes

- **Wrong units on import.**
- **Printing to answer a strength question** a printed part cannot answer.
- **Modelling fits at nominal size** and being surprised they do not fit.
- **Ignoring orientation**, which changes both strength and surface quality.

## Recap

- Decide what question each prototype answers.
- Export with the right units, check the mesh, orient for strength and minimal support.
- Plan clearance for fits; test with a coupon; capture the result as a parameter.
- Treat hot parts and fumes seriously and follow your space's rules.

## Try it

On the Do tab, prepare a part for printing in a free slicer, from export to a checked layer preview.


Pick the right kind of prototype and prepare a CAD part for 3D printing: units, orientation, supports, fits and slicer checks.

Prototyping and 3D printing

How to optimize your 3d model for FDM 3D printing

PrusaSlicer Beginner Tutorial: Learn the basics

Choose between machining, casting, forming, moulding and additive processes, design parts that are easy to make and assemble, measure process capability, and prototype with 3D printing.