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

Create a new part document and set the units to millimetres.

Create named variables: t = 6 mm, w = 50 mm, leg = 60 mm, bolt_d = 6.6 mm, edge = 12 mm (Onshape: Variable feature; FreeCAD: a Spreadsheet or VarSet with aliases).

Sketch the L profile on a side plane, anchored to the origin. Drive both leg lengths with leg and both thicknesses with t, until the sketch is fully defined.

Extrude (Pad) the profile by w, symmetric about the mid plane.

Add two clearance holes of diameter bolt_d on the base leg, each edge from the end, spaced w - 2 * edge apart using an expression.

Add an inside fillet of radius t at the bend as a separate, late feature, and give every feature a meaningful name.

Flex the model: change w to 70 and t to 8. Check that the holes stay centred and spaced correctly and nothing fails. Change them back.

Make a quick drawing (or screenshot) with the key dimensions and note the part's volume or mass from the tool's mass properties.

## Why it matters

In Technical Drawing & CAD Basics you sketched shapes and turned them into solids. Professional CAD goes one step further: the model remembers **why** it has its shape. If the customer asks for a bracket 10 mm wider, or the bolt changes from M6 to M8, you change one number and the whole part, its drawing and the assembly update. That is **parametric modelling**, and it is how almost all mechanical design work is done in tools such as SolidWorks, Creo, Inventor, Fusion, Onshape and FreeCAD.

## The core ideas

**Sketches, constraints and dimensions.** A sketch is a 2D profile on a plane. *Geometric constraints* fix relationships (horizontal, parallel, tangent, coincident, symmetric, equal). *Dimensional constraints* fix sizes and positions. A sketch is **fully defined** when nothing can move without breaking a constraint; most tools show this by changing the line colour (for example, from blue to black in SolidWorks and Onshape, or green in FreeCAD's Sketcher).

**Features.** Each solid operation (extrude/pad, revolve, cut/pocket, hole, fillet, chamfer, pattern, mirror) is a feature that builds on the ones before. The ordered list is the **feature tree** (or history).

**Variables and equations.** You can name key values, such as `thickness = 6 mm` or `hole_spacing = 40 mm`, and drive dimensions with them or with expressions like `width = hole_spacing + 2 * edge_distance`. Onshape calls these variables (and Configurations for families of parts); FreeCAD uses expressions and spreadsheets or VarSets.

**Design intent.** The skill is not clicking tools; it is choosing constraints that behave sensibly when something changes. Ask: what should stay fixed, and what should follow?

## Worked example: an L-bracket

Suppose you need a 90° bracket to hold a small motor to a frame with two M6 bolts.

1. **Name the drivers**: `t = 6 mm` (thickness), `w = 50 mm` (width), `leg = 60 mm`, `bolt_d = 6.6 mm` (an M6 clearance hole, medium fit per ISO 273), `edge = 12 mm` (hole centre to edge).
2. **Sketch the L profile** on the side plane, constrained to the origin, with the leg lengths set to `leg` and the thickness set to `t` on both legs (use an *equal* constraint so you only change one number).
3. **Extrude** the profile by `w`, symmetric about the mid plane, so the part stays centred if the width changes.
4. **Add the holes** with a Hole feature, positioned from the edges by `edge` and spaced `w - 2 * edge` apart. Because the spacing is an expression, changing `w` moves the holes correctly.
5. **Add an inside fillet** of radius `t` at the bend to reduce stress concentration (and to match how sheet or bent parts are made).
6. **Test the intent**: change `w` to 70 and `t` to 8. If anything breaks, flips or ends up in the wrong place, your constraints are not capturing the intent yet.

## Good habits

- **Sketch simple, add detail with features.** Put fillets and chamfers in their own features near the end, not inside the sketch. They are the features most likely to fail when geometry changes.
- **Reference stable geometry.** Constrain to the origin and default planes, not to edges created by later features. Edges referenced by later features can be renamed internally when the model changes, causing the "topological naming" breakages FreeCAD users know well.
- **Name features and variables.** `Pocket003` tells nobody anything; `motor_mount_holes` does.
- **Fully define every sketch.** An under-defined sketch can shift silently when you edit something else.
- **Model in real units and real sizes.** Use the units you will manufacture in and real standard sizes (hole sizes, material thicknesses).

## Free tools

- **Onshape** (browser-based) has a free plan for hobby and non-commercial use. Documents in the free plan are **public**, so never put an employer's or client's design in it. Check the current plan terms on onshape.com. Checked on 2026-10-23.
- **FreeCAD** is free, open source and runs on Windows, macOS and Linux. Its Part Design workbench covers sketch-based solid modelling.

## Common mistakes

- **Over-constraining.** Adding a dimension that conflicts with an existing constraint. The tool will complain; delete one rather than forcing it.
- **Dimensioning to the wrong thing.** Dimension the hole position from the edge the assembly cares about (the datum), not from whatever edge was handy. The next lesson explains datums.
- **Building everything in one sketch.** Huge sketches are fragile and hard to edit.
- **Never flexing the model.** If you have not changed the drivers, you do not know whether the model is really parametric.

## Recap

- Parametric models are driven by constraints, dimensions and named variables.
- The feature tree is a recipe; order and references matter.
- Design intent means the model changes the way the design should.
- Test every model by changing its key parameters.

## Try it

On the Do tab, build the L-bracket in Onshape or FreeCAD, drive it with variables and check that it updates cleanly.


Build a part driven by constraints and named variables so it changes the way the design should.

Parametric CAD

Parametric Modeling in Onshape

FreeCAD - Intro to Parametric Modelling

## Why it matters

A drawing that says "hole at 40 ± 0.1 from the edge" seems clear until two inspectors measure the same part and get different answers because they measured from different edges, or until a perfectly good part is rejected because a square tolerance zone was stricter than the assembly needed. **Geometric Dimensioning and Tolerancing (GD&T)** is a symbolic language that says exactly which features matter, how to measure them, and how much variation is allowed. In the US it is defined by **ASME Y14.5** (the current edition is Y14.5-2018); internationally, the ISO GPS standards such as **ISO 1101** cover similar ground with some differences. See asme.org and iso.org for the current editions. Checked on 2026-10-23.

## Datums: where measurement starts

A **datum** is a theoretically exact reference (a plane, an axis or a point) established from a real feature on the part, labelled with a letter in a box such as **A**. Datums are chosen from how the part is located in its assembly: the face that sits on the frame, the bore that goes over a shaft, the edge that butts against a stop.

The **datum reference frame** uses up to three datums in order of precedence:

- **Primary (A)**: the part rests on it with at least 3 points of contact. It stops 3 degrees of freedom (one translation, two rotations).
- **Secondary (B)**: at least 2 points of contact, perpendicular to A. It stops 2 more.
- **Tertiary (C)**: at least 1 point of contact. It stops the last one.

This is the **3-2-1 rule**. The order matters: a part fixtured on A first and then B can measure differently from one fixtured on B first.

## Basic dimensions and the feature control frame

GD&T locates features with **basic dimensions**, shown in a box (for example, a boxed 40). A basic dimension is the theoretically exact distance: it has no tolerance of its own. The tolerance lives in a **feature control frame** attached to the feature, read left to right:

```text
| position | dia 0.2 (M) | A | B | C |
```

That reads: "the axis of this hole must lie within a cylinder of diameter 0.2 mm, at maximum material condition, located by the basic dimensions from datums A, B and C."

## Position tolerance

With classic ± coordinate tolerances, each direction gets its own band, so the zone is a **square**. Position uses a **cylindrical zone** around the true position. A circle that just encloses a ±0.1 mm square has a diameter of 0.2 × sqrt(2) = 0.283 mm, so the round zone accepts about 57 % more area than the ±0.1 mm square while still guaranteeing the part fits (a hole that is 0.14 mm off diagonally fits just as well as one 0.14 mm off in x).

Checking position from measured coordinates:

```text
dx = measured x - basic x,  dy = measured y - basic y
actual position (diameter) = 2 * sqrt(dx^2 + dy^2)
```

Example: the hole's basic location is (40, 25). A CMM measures its axis at (40.03, 25.04).

```text
dx = 0.03, dy = 0.04
position = 2 * sqrt(0.03^2 + 0.04^2) = 2 * 0.05 = 0.10 mm    (within dia 0.2: accept)
```

Note the factor of 2: the axis is 0.05 mm from true position, but the zone is specified as a diameter.

## Material condition modifiers and bonus tolerance

**Maximum material condition (MMC)**, symbol (M), is the size at which the feature contains the most material: the *smallest* hole or the *largest* pin. When position is specified at MMC, the tolerance applies at MMC and grows as the feature departs from MMC. This extra is the **bonus tolerance**, and it reflects real assembly: a bigger hole can be a little further off and the bolt still fits.

Example: a hole sized dia 10.0 to 10.2, position dia 0.1 at MMC.

```text
MMC (smallest hole)       = 10.0
actual hole size          = 10.15
bonus                     = 10.15 - 10.0 = 0.15
allowed position          = 0.1 + 0.15 = 0.25 mm
```

**Least material condition (LMC)**, symbol (L), is the opposite (largest hole, smallest pin) and is used when wall thickness or edge distance must be protected. With no modifier, the tolerance is fixed regardless of feature size (RFS, the default in ASME Y14.5).

## Other common controls

- **Form**: flatness, straightness, circularity, cylindricity (no datum needed).
- **Orientation**: perpendicularity, parallelism, angularity (to a datum).
- **Profile** of a surface or line: the most versatile control, often used for complex shapes.
- **Runout**: circular and total runout for rotating parts, measured relative to a datum axis.

## Common mistakes

- **Choosing datums for convenience.** Datums should come from how the part functions and is assembled, then inspection follows them.
- **Forgetting the diameter symbol.** Without it, a position zone is two parallel planes, not a cylinder.
- **Tolerancing everything tightly.** Each tight tolerance costs machining time and inspection. Tolerance what the function needs.
- **Mixing ASME and ISO rules.** Some defaults differ (for example, how size and form interact). State which standard the drawing follows.

## Recap

- Datums A, B, C build a reference frame by the 3-2-1 rule, chosen from function.
- Basic dimensions are exact; tolerances live in feature control frames.
- Position = 2·sqrt(dx² + dy²) against a cylindrical zone.
- At MMC, bonus tolerance = departure from MMC size.

## Try it

The Do tab has a quiz on reading datums, computing position and finding bonus tolerance.


Read datum reference frames and feature control frames, check a hole's position, and work out bonus tolerance at MMC.

GD&T in practice

Understanding GD&T

How to Apply GD&T Position Tolerance to a Hole

Write down the hand results first: I = 1,666.7 mm^4, tip deflection 0.80 mm, root bending stress 60 MPa, reactions 100 N and 20 N·m.

Model the bar in Part Design (a 20 × 10 mm rectangle padded 200 mm) and switch to the FEM workbench.

Create an analysis container with the CalculiX solver, add a solid material (steel, E = 200 GPa, Poisson's ratio 0.3).

Add a fixed constraint on one end face and a 100 N force on the opposite end face, pointing down across the 10 mm depth.

Create a mesh (Gmsh or Netgen) with a maximum element size of about 5 mm and run the solver.

Read the maximum displacement and compare it with 0.80 mm. Record the percentage difference.

Probe the stress on the top surface about 20 to 30 mm from the fixed end and compare it with the hand value at that point (M = 100 N × remaining length; for 25 mm from the support, M = 17,500 N·mm and stress = 52.5 MPa).

Refine the mesh (for example 2.5 mm, then about 1.5 mm) and re-run. Note how displacement settles, while the peak stress at the fixed-end corner keeps rising: that is a singularity.

## Why it matters

Hand calculations work for shafts, beams and bolts with simple shapes. Real parts have holes, fillets, ribs and odd loads. **Finite element analysis (FEA)** estimates the stresses and deflections in such parts by splitting the geometry into many small, simple pieces (**elements**) joined at **nodes**, writing the stiffness equations for each piece, assembling them into one large system of equations (K·u = F), and solving for the node displacements u. Stresses come from those displacements.

FEA is powerful and easy to misuse. A colourful stress plot looks convincing whether the model is right or wildly wrong. The most important skill in this lesson is **sanity-checking**.

## The workflow

1. **Define the question.** What do you need: peak stress, deflection, stiffness, a natural frequency? This decides the type of study (linear static, modal, thermal...).
2. **Prepare the geometry.** Remove details that do not affect the answer (small cosmetic fillets, text, threads) but keep details near the region of interest.
3. **Assign materials.** Young's modulus E and Poisson's ratio for stiffness; yield strength for comparison. For structural steel, E is about 200 GPa and Poisson's ratio about 0.3.
4. **Apply boundary conditions.** Fixtures (where the part is held) and loads (forces, pressures, bolt preload). This is where most errors come from: a real bolted face is not perfectly rigid.
5. **Mesh.** Choose element type and size. Finer meshes are more accurate and slower.
6. **Solve, then check before you believe it.**

## Worked example: a cantilever you can check by hand

A steel bar is fixed at one end and loaded at the other. Length L = 200 mm, rectangular section b = 20 mm wide by h = 10 mm deep (load acting across the 10 mm depth), tip load F = 100 N, E = 200,000 MPa.

```text
second moment   I = b * h^3 / 12 = 20 * 10^3 / 12   = 1,666.7 mm^4
tip deflection  d = F * L^3 / (3 * E * I)
                  = 100 * 200^3 / (3 * 200,000 * 1,666.7) = 0.80 mm
root stress     s = M * c / I = (100 * 200) * 5 / 1,666.7 = 60 MPa
```

An FEA of this bar should give a tip deflection very close to 0.80 mm (slightly more if the model includes shear deformation and the real fixed-end behaviour). The stress at the top surface near the fixed end, away from the corner, should be close to 60 MPa.

## How to sanity-check any FEA result

- **Compare with a hand calculation** of a simplified version, as above. If FEA and the hand calculation differ by a factor of 2 or 10, find out why before going further.
- **Check reaction forces.** The solver reports the forces at fixtures. They must balance the applied loads (here, 100 N and a 20 N·m moment at the fixed end).
- **Look at the deformed shape** (with exaggerated scale). Does it bend the way you expect? Parts flying off or bending the wrong way mean missing or wrong constraints.
- **Check units.** A mm model with loads entered as if in metres gives results off by factors of 1,000 or more.
- **Run a mesh convergence study.** Refine the mesh in the region of interest and re-solve. Displacement should settle quickly; stress should settle to within a few percent. If it keeps rising with every refinement, you are probably looking at a singularity.

## Singularities

At a perfectly sharp re-entrant corner, or at a point load or a point fixture, the theoretical stress is infinite. FEA shows a "hot spot" there that grows every time you refine the mesh. That number is not real. In the cantilever, the corners where the bar meets the fixed support do this. Real parts have fillet radii and real supports are not perfectly rigid, so the fix is to model the real fillet, read stress a small distance away, or treat the support more realistically, not to report the peak.

## Free tools

- **FreeCAD FEM workbench** with the CalculiX solver is free and handles linear static and modal studies. Meshing uses Gmsh or Netgen, bundled with FreeCAD.
- Several commercial packages offer free student or limited editions; check their current terms. Checked on 2026-10-23.

## Common mistakes

- **Over-constraining.** Fixing every face of a bolt hole makes the part far too stiff.
- **Reading peak stress at a singularity.**
- **Using linear analysis beyond yield.** Linear static FEA assumes stress is proportional to strain. Once the result is above yield, the answer is no longer valid (non-linear analysis is a separate topic).
- **Trusting defaults.** Default mesh sizes and contact settings are not chosen for your problem.

## A note on real design

FEA supports engineering judgement; it does not replace it. Results for real products are checked by experienced engineers, validated by testing where it matters, and, for designs that affect public safety, reviewed and signed by a licensed professional engineer.

## Recap

- FEA solves K·u = F on a mesh of elements; stresses come from displacements.
- Most errors come from boundary conditions, units and meshing.
- Always compare with a hand calculation, check reactions and deformed shape, and run a mesh convergence study.
- Hot spots at sharp corners and point loads are singularities, not real stresses.

## Try it

On the Do tab, model the cantilever in FreeCAD, run it, and compare the result with the hand calculation.


Run a simple linear static finite element analysis and sanity-check it with a hand calculation, reactions and a mesh study.

Intro to FEA

Understanding the Finite Element Method

Convergence Testing — Lesson 3

Model parts that change the way the design should with parametric CAD, communicate tolerances with datums and position (GD&T), and run and sanity-check a simple finite element analysis.