An engineering drawing for machining – why you still need one
Many people think a STEP file is enough. It shows the shape exactly, but not which dimensions matter, which tolerances apply, which thread the hole should have or which material the part should be made from. That information is on the drawing.
A workshop that receives an unclear drawing does one of two things: adds a margin for the uncertainty or asks questions that delay the quote. A good technical drawing gets you an accurate price first time.
The drawing is also a contract. It defines what the workshop must deliver and what you can reject. If a requirement is not on the drawing, it is hard to claim it afterwards. So it pays to spend an extra hour on a clear drawing before it goes out for quotes.
Views, projection and sections
Show as few views as needed, but enough for every feature to be visible. A simple part often manages with a main view and a side view. Choose as the main view the one that shows most of the part's shape.
In the UK and most of Europe, first-angle projection (method 1) to ISO 5456-2 is used. Show the symbol in the title block, because American drawings often use third-angle projection and the views then end up on the other side.
Internal geometry – holes, pockets and channels – is best shown in a section. Use enlarged details for small features such as grooves and undercuts. An isometric view in the corner helps the reader understand the shape quickly. Line types and views are governed by ISO 128.
Choose a scale that lets every dimension fit and be read – 1:1, 1:2, 2:1 or 5:1 are common. Put the drawing on a standard sheet size, usually A3 or A4. Small parts are better drawn enlarged than with cramped dimensions.
Dimensioning from datums
Dimension from the faces that matter for the function – the datums. This is often the face the part is mounted against and a centre hole. All hole positions are then measured from the same datum, not from hole to hole. Chain dimensioning makes tolerances stack up and forces the workshop to guess which dimension matters most.
Each dimension should appear once. Duplicate dimensions create contradictions when tolerances are added together. If you need to show a dimension for information, put it in brackets as a reference dimension. The rules for dimensioning are in ISO 129-1.
Give dimensions that can be measured. A dimension to an imaginary intersection between two fillets is hard to check – measure to a real edge instead.
Tolerances: general and individual
State a general tolerance class in the title block, for example ISO 2768-m. It applies to every dimension without its own tolerance. Then put individual tolerances only on the dimensions that affect the function: fits, hole spacings for bolted joints and sealing faces.
Fits are given with an ISO 286 designation, for example Ø12 H7. Form and position tolerances – flatness, perpendicularity, coaxiality, position – are given in a feature control frame to ISO 1101 and refer to datums A, B and C. Use them where a ± dimension is not enough. More on values and classes in the guide ISO tolerances and fits.
Threads, surface roughness and material
Specify threads with their standard designation: M8 for a coarse metric thread, M8×1 for a fine thread, plus depth, for example “M8 – 15 deep”. Metric threads follow ISO 68-1 and ISO 965. Pipe threads are given as G 1/4. State whether the hole goes through and whether it is countersunk.
Surface roughness is given as Ra in micrometres, to ISO 21920, which has replaced ISO 1302. As a guide, Ra 3.2 µm suits ordinary milling, Ra 1.6 µm fine milling and turning, and Ra 0.8 µm or lower grinding and sealing faces. State a general roughness for the whole part and tighten it only where needed. Specifying Ra 0.4 µm everywhere can double the machine time.
Write the material with its standard designation, for example aluminium EN AW-6082-T6 or stainless steel 1.4404. State the surface treatment: anodising and colour, galvanising, powder coating or blasting. Also say whether edges should be deburred – “all edges broken 0.2–0.5 mm” is a common note.
Quantity affects the price more than anything. State how many you want now and whether more may follow. A quote for 1, 10 and 100 pieces shows how the set-up time is spread and helps you choose the right batch size.
The title block to ISO 7200
The title block is the drawing's identity. ISO 7200 specifies the fields needed: owner, title, drawing number, revision, date, created by, approved by, scale and sheet. Add material, general tolerance, projection symbol and unit.
The revision matters. Every change should get a new revision and a short description in a revision field. Then both you and the workshop know you are talking about the same version, and that the STEP file belongs to the right drawing.
Drawings for sheet metal and 3D printing
A sheet metal part needs a drawing showing the bent part with dimensions, and ideally a flat pattern with bend lines. State sheet thickness, material, inside radius and bend direction – up or down. Dimension flanges to the outside or inside edge, but be consistent. Send a DXF of the flat pattern with the drawing, so the workshop can check its own calculations. Read more about sheet metal design.
For 3D-printed parts a simpler drawing is often enough. State material, colour, the dimensions that matter for fit and which faces will be visible. Also give tolerances the method can achieve – a guide value is ±0.1–0.2 mm – and whether holes are to be drilled out after printing.
How to send the drawing – and common mistakes
Send the drawing as a PDF and the 3D model as STEP. Use the same number and revision in both file names, for example “1024-02_flange_revB.pdf” and “1024-02_flange_revB.step”. That way the files never get mixed up.
Say in the email how many you want, when you need them and whether material certificates or inspection reports are required. Ask for prices on several quantities. The workshop can often suggest small changes that lower the price – a larger radius in a pocket or a different tolerance class. Be open to such suggestions, but let the designer judge whether the function is affected.
The most common mistakes are a missing general tolerance, duplicate dimensions, chain dimensioning, threads without depth and tolerances tighter than the function requires. Another common mistake is a drawing and 3D model showing different versions.
We produce drawings in Autodesk Fusion with views, sections, tolerances and a title block. Read more about technical drawings from NordiTeq, about machine parts for CNC or request a quote for your drawing.
Surface roughness – guide values by process
| Ra (µm) | Typical process | Example of use |
|---|---|---|
| 6.3 | Rough milling, sawing | Non-functional surfaces |
| 3.2 | Normal milling and turning | General roughness on machine parts |
| 1.6 | Fine milling, fine turning | Mating faces, clearance fits |
| 0.8 | Grinding, very fine turning | Bearing seats, sealing faces |
| 0.4 and lower | Fine grinding, honing, polishing | Hydraulics, high-demand sliding surfaces |
Guide values. Actual roughness depends on material, tooling and machine. Surface requirements are specified to ISO 21920 (formerly ISO 1302).
Checklist: a drawing ready for quoting
- Main view, necessary side views, sections and details
- Projection symbol (first angle in Europe)
- Dimensioning from datums, each dimension once
- General tolerance, e.g. ISO 2768-m
- Individual tolerances and fits where the function requires
- Threads with designation, depth and countersink
- General Ra surface roughness and tighter requirements where needed
- Material, surface treatment and deburring
- Title block with number, revision and date
- Quantity now and any future volume
Frequently asked questions
What should a technical drawing contain?
Views and sections showing the whole shape, dimensions from datums, a general tolerance and individual tolerances where needed. Also threads, surface roughness, material, surface treatment and a title block with number and revision. State the quantity too.
Is a STEP file enough for the workshop?
For simple parts without special requirements it may be. As soon as fits, threads or surface requirements matter, a drawing is needed, because the STEP file does not show tolerances. Most workshops want both.
Which projection method is used in the UK and Europe?
First-angle projection (method 1) to ISO 5456-2. The symbol should be in the title block. American drawings often use third-angle projection, where the views end up on the opposite side.
What does Ra 3.2 mean on a drawing?
Ra is the arithmetic mean deviation of the surface profile, given in micrometres. Ra 3.2 µm corresponds to a normally milled or turned surface and is a common general requirement. A lower value gives a smoother surface but a longer machining time.