A manufacturing drawing is the document a supplier makes a part from and inspects it against. A drawing pack is the full set for a product: a drawing for every made part, drawings showing how the parts assemble, and a bill of materials listing everything, bought-in items included. The 3D model defines the shape. The drawing adds what the model does not carry on its own, which is how accurately each feature must be made, from what material, with what finish and to which standard.
Tolerances are the core of that information. Every dimension has one, either written beside it or covered by a general note, and the tolerance is the range within which a part is acceptable. Set too loose, parts do not fit or work. Set too tight, the part costs more than it needs to and the product gains nothing.
What a drawing pack should contain
- Part drawings for every manufactured part, with all the dimensions needed to make and inspect it, its tolerances, material, finish, heat treatment and any special requirements.
- Assembly drawings showing how parts and sub-assemblies go together, with item balloons keyed to the bill of materials, fixings and tightening torques where they matter, and any dimensions to be achieved at assembly.
- General arrangement drawings for larger equipment, showing the whole product, its overall dimensions, mass, lifting points and interfaces with the site or with other equipment.
- A bill of materials with part numbers, descriptions, quantities, materials and the revision of each item, and for bought-in parts the manufacturer’s reference and an acceptable alternative where one exists.
- Fabrication information where parts are welded: weld symbols, joint preparations and, for larger structures, weld maps and cut lists.
- 3D models, usually as STEP files, for suppliers who machine or build tooling directly from the model, with a note saying whether the model or the drawing governs if they differ.
The hydrogen production prototype is an example at the larger end. Its fabrication and installation drawings ran to general arrangements, pipe spools, weld maps and assembly details, because a system of frames, process equipment and pipework needs each of them to be built and installed.
Title block and general notes
Every drawing needs a title block with the part number, title, revision, scale, units and projection symbol, together with the drawing standard it follows, such as BS 8888 or ASME Y14.5. First angle projection is the usual convention in the UK and Europe, and third angle in North America. General notes then cover the general tolerance, edge breaks and deburring, the default surface finish and anything else that applies to the whole part.
Material should be stated as a full specification, for example aluminium alloy 6082-T6 or stainless steel 1.4404 (316L). A note that says ‘aluminium’ or ‘stainless’ leaves the grade, temper and properties to the supplier. Finishes need the same precision: anodising type and thickness, powder coat colour by RAL number, or passivation and plating to a named standard.
General tolerances and specific tolerances
A general tolerance note sets the tolerance for every dimension that does not carry its own. The common reference is ISO 2768-1, which defines four classes for linear and angular dimensions: fine (f), medium (m), coarse (c) and very coarse (v). A note such as ‘general tolerances to ISO 2768-m’ applies the medium class, which for linear dimensions gives:
| Nominal size | ISO 2768-m tolerance |
|---|---|
| 0.5 mm up to 6 mm | ±0.1 mm |
| Over 6 mm up to 30 mm | ±0.2 mm |
| Over 30 mm up to 120 mm | ±0.3 mm |
| Over 120 mm up to 400 mm | ±0.5 mm |
| Over 400 mm up to 1,000 mm | ±0.8 mm |
| Over 1,000 mm up to 2,000 mm | ±1.2 mm |
Medium suits most machined parts, and coarse suits many fabrications. Specific tolerances then go on the features that affect function: bearing bores, shaft diameters, locating holes, sealing faces and any dimension in a critical chain. For fits between shafts and holes, ISO 286 codes such as H7/g6 save writing out the limits. On a 20 mm diameter, H7 gives a hole of 20.000 to 20.021 mm and g6 a shaft of 19.980 to 19.993 mm, so the clearance runs from 0.007 to 0.041 mm. That is a sliding fit, used where parts must move freely while locating accurately.
Why tight tolerances cost money
Every process has a range it holds comfortably. General CNC machining holds ±0.1 mm on most features without special effort, and around ±0.025 mm with care. Beyond that, a feature may need a finishing pass, reaming or grinding, measurement in a temperature-controlled room or on a coordinate measuring machine, and the scrap rate climbs because the process is working near its limit. Bends in sheet metal and welded frames have much wider natural ranges than machined faces, so a tolerance that is routine on a milled part can be very hard to hold on a fabrication. The rules for each process are covered in our guide to design for manufacture.
Tightening a tolerance that sits comfortably inside the process range costs little. Past that range, it can multiply the cost of the feature. The practical rule is to give each feature the widest tolerance that still lets the product work, and to be able to say why each tight one is there. Surface finish behaves the same way: Ra 3.2 µm is a normal milled finish, Ra 1.6 µm needs more care, and Ra 0.8 µm or below usually means grinding or another fine finishing operation.
A simple tolerance stack-up
A stack-up adds the tolerances along a chain of dimensions to find the variation in a gap or fit that matters. Take a housing with a bore of depth A, into which three machined parts are stacked: a collar B, a spacer C and a gear hub D. The space left at the top is the end float, and the specification asks for 0.25 to 0.75 mm.
| Dimension | Nominal | Tolerance |
|---|---|---|
| A, housing bore depth | 40.00 mm | ±0.10 mm |
| B, collar length | 12.00 mm | ±0.05 mm |
| C, spacer length | 15.00 mm | ±0.10 mm |
| D, gear hub length | 12.50 mm | ±0.05 mm |
The nominal gap is 40.00 − (12.00 + 15.00 + 12.50) = 0.50 mm.
Worst case. The tolerances add directly, 0.10 + 0.05 + 0.10 + 0.05 = ±0.30 mm, so the gap can range from 0.20 to 0.80 mm. That falls outside the requirement at both ends.
Root sum square (RSS). If each dimension varies randomly and independently about its nominal value, the likely variation is the square root of the sum of the squares:
√(0.10² + 0.05² + 0.10² + 0.05²) = √0.025 ≈ ±0.16 mm
That gives a gap of about 0.34 to 0.66 mm, comfortably inside the requirement.
The two answers lead to different decisions. For a few dozen assemblies, or where the end float affects safety, worst case is the sounder basis, and the fix is to tighten the largest contributors. Holding the spacer to ±0.05 mm brings the worst case to ±0.25 mm and the gap to 0.25 to 0.75 mm, exactly the requirement. For volume production from processes known to be capable and centred, RSS is a reasonable basis and the original tolerances can stand, accepting that a small fraction of assemblies may fall outside if those assumptions do not hold. Low-volume machinery often takes a third route and sets the gap at assembly with a shim or a selected spacer.
Basic geometric tolerancing
Plus-and-minus dimensions control size well and location poorly. Geometric dimensioning and tolerancing (GD&T), defined in ISO 1101 and related standards or in ASME Y14.5, controls form, orientation, location and runout relative to datums. Datums are the faces or features that locate the part when it is assembled and when it is measured.
- Datums come from the functional features, such as the face a part bolts down on or the bore it locates on. Dimensions and geometric tolerances refer back to them, so inspection reproduces the way the part is used.
- Form tolerances (flatness, straightness, roundness and cylindricity) control the shape of a feature on its own.
- Orientation tolerances such as perpendicularity and parallelism control a feature relative to a datum.
- Position controls where a feature such as a hole sits relative to datums, within a zone around its true position.
- Profile and runout cover curved surfaces and rotating features.
Position tolerancing shows why this helps. A hole located at ±0.1 mm in X and Y has a square tolerance zone 0.2 mm across. One that sits 0.14 mm off centre along the diagonal is accepted, while one 0.11 mm off along an axis is rejected, even though it is closer. A circular position zone that just encloses that square, about Ø0.28 mm, has 57% more area, and so accepts more parts that will assemble at no cost to the fit. Adding a maximum material condition modifier lets the zone grow as a hole is made larger than its smallest permitted size, which suits clearance holes for bolts.
How SixGate™ can help
The Engineering Pack stage produces detailed manufacturing drawings and the manufacturing process for your product, ready for suppliers to quote and build from. You receive a pack in which each tolerance follows from the feature’s function and the process that will make it, with the critical stack-ups already resolved. On the bulk material handling project, that meant full drawing packages and bills of materials for fabrication. A pack can also be produced on its own for a design you already have, including one that exists only as paper drawings or as a physical part to be reverse engineered.