Specifying CNC Machined Parts —
What Information Your
Machinist Needs

The majority of delays, reruns and cost overruns on machined parts trace back to the same root cause: the information provided to the machinist was incomplete, ambiguous, or wrong. A drawing with missing tolerances, an unspecified material condition, a thread call-out that could be interpreted two ways, or a surface finish requirement that appears nowhere on the drawing — each of these results in the machinist making assumptions, and those assumptions may not match the design intent.

This article covers everything a machinist needs to produce a correct first-off part, what format to provide it in, and the specific information gaps that most commonly cause problems.

Drawing vs 3D Model — What to Send

The most common question from engineers specifying machined parts for the first time is whether to send the 3D CAD model or a 2D drawing. The answer depends on the complexity and precision requirements of the part.

A 3D model (STEP, IGES or native SolidWorks / CATIA / Inventor format) conveys geometry clearly and allows the machinist to programme toolpaths directly from the model. For simple parts with generous tolerances and no critical features, a STEP file with a brief written specification is often sufficient and faster to produce than a fully dimensioned drawing.

However, a 3D model alone cannot communicate:

• Which dimensions are critical and which are not
• Tolerances on specific features (the model is nominally perfect — it contains no tolerance information)
• Surface finish requirements on individual surfaces
• Geometric tolerances (flatness, parallelism, true position etc.)
• Datum scheme — which surfaces the machinist should use as reference for setups
• Thread class of fit
• Special notes (heat treatment before or after machining, pressure testing, inspection requirements)

For any part with close-tolerance features, threads, mating surfaces, or inspection requirements, a 2D engineering drawing — produced to BS 8888 — is the correct deliverable. The drawing is the legal document of record and the basis on which the part will be inspected. The 3D model is a useful supplement, not a substitute.

The Title Block — What Must Be There

The title block is read before anything else on the drawing. Missing or incorrect information here causes confusion at every stage from ordering to inspection. A complete title block includes:

Material Specification — Be Specific

The material callout on a machined part drawing is one of the most critical and most frequently under-specified pieces of information. "Stainless steel" is not a material specification. "Aluminium" is not a material specification. The machinist needs a full grade designation sufficient to order the correct material from a stockholder.

What to include in a material callout:

• Grade: EN 1.4404 / 316L, EN 1.4301 / 304, 6082-T6, EN24T, EN8, S355J2 etc.
• Product form: Bar, plate, tube — because the same grade may have different properties in different product forms
• Condition / temper: T6 for aluminium alloys, +N (normalised) for structural steel plate, annealed vs hardened for tool steels
• Standard reference: EN 10278 (bright bar), EN 573-3 (aluminium), ASTM A276 (stainless bar) etc.
• Mill certificate requirement: Whether a 3.1 certificate is required (specify this on the drawing if the application demands it — it will be included in the price if asked for)

Examples of complete material callouts:

• 316L stainless steel bar to EN 10278 / EN 1.4404, solution annealed condition. 3.1 certificate required.
• Aluminium alloy 6082-T6 to BS EN 573-3, extruded bar.
• EN24T (817M40) alloy steel bright bar to BS EN 10278, condition T.

Tolerances — The Single Most Important Factor in Cost

Tolerances drive machining cost more than almost any other drawing requirement. A 0.01mm tolerance requires a grinding operation; a 0.1mm tolerance can be held on a standard CNC milling centre; a 0.5mm tolerance can often be held without a finish pass. The cost difference between these is significant. Specifying tighter tolerances than the function requires adds cost with no benefit.

General Tolerances — BS EN ISO 2768

BS EN ISO 2768 defines general tolerances for linear dimensions, angular dimensions, and geometric form and orientation, in four classes:

Referencing BS EN ISO 2768-m (medium) in the title block as the general tolerance provides a clear, unambiguous default for all undimensioned features. Any features requiring tighter or looser tolerances than the general class should be explicitly dimensioned on the drawing with their individual tolerance.

Representative linear tolerances for class m (medium) at common dimension ranges:

Critical Dimensions — Explicit Tolerances

Any dimension that is critical to function — a bearing bore, a shaft diameter, a sealing face width, a bolt pattern location, a register diameter — must be explicitly dimensioned with its individual tolerance. Do not rely on the general tolerance for any feature where the acceptable range is tighter than the general class provides, or where the consequence of a dimension being out of tolerance is functional failure.

Fits — Shafts and Holes

For mating cylindrical features (shaft in a bore, boss in a clearance hole, interference fit), the tolerance is most clearly communicated using ISO fit designations. The system uses a letter to define the fundamental deviation and a number to define the tolerance grade:

• H7/h6 — the most common clearance fit. Used for location fits where free assembly is required (sliding fit with minimal play)
• H7/k6 — transition fit. May result in slight clearance or interference. Used for location fits where accurate positioning is needed without needing a press
• H7/p6 — interference fit. Light press or push fit. Used for bushes, bearing housings
• H7/s6 — force fit. Requires hydraulic press or heating. Used for permanent assemblies

Calling out "H7 bore" or "g6 shaft" is clearer than writing a bilateral tolerance and expecting the machinist to deduce the fit intent. It also makes inspection straightforward — go/no-go gauges are available for standard ISO fits.

Surface Finish

Surface finish is specified in terms of Ra — the arithmetic mean roughness height, in micrometres. The surface finish symbol on a drawing (a tick-mark style symbol per BS EN ISO 1302) indicates that the surface must be machined, and the Ra value is annotated alongside.

If a general machined surface finish applies to all machined surfaces except those specifically called out, state it in the title block (e.g. "All machined surfaces Ra 3.2 unless otherwise stated"). Every sealing face, every bore that accepts a seal, every surface in dynamic contact should have its surface finish individually specified.

Thread Specifications

A thread call-out that is missing information forces the machinist to make a decision that is rightly the designer's. A complete thread specification includes:

• Thread form: M (metric ISO), G (BSP parallel), R (BSP taper), NPT (American taper pipe thread), UNC, UNF
• Nominal diameter: M12, G¾, etc.
• Pitch: For metric, pitch is usually implied by the nominal diameter for coarse threads (M12 = 1.75mm pitch by default) — but fine pitch should always be explicitly stated (M12×1.25)
• Class of fit / tolerance: 6H for internal threads (nuts, tapped holes), 6g for external threads (bolts, studs) — the standard tolerance class for general engineering. State 4H6H for close tolerance or 7H for looser tolerance if required
• Thread depth or engagement length: For tapped holes, the minimum full thread depth must be stated. "Thread through" or "Thread 20mm deep minimum" avoids ambiguity
• Handedness: State LH (left hand) if applicable. Right hand is assumed if not stated

A complete thread callout example: M16×2.0 – 6H, 25mm minimum full thread depth

Datum Scheme

The datum scheme defines which surfaces or features the machinist should use as the reference for setup and measurement. Without a defined datum scheme, the machinist will choose their own references — which may not match the surfaces that matter for the part's function in the assembly.

For simple prismatic parts, three mutually perpendicular datum planes (primary, secondary, tertiary) cover most requirements. For rotational parts, the datum axis is typically the primary datum. For more complex parts, especially those with tight positional tolerances between features, a formal GD&T datum scheme using feature control frames is appropriate.

At minimum, the drawing should make clear which face or bore the critical dimensions are measured from. "Dimension from face A" is better than leaving the machinist to infer the reference from context.

Geometric Tolerances — When GD&T Is Needed

Coordinate dimensions and bilateral tolerances control the size and location of features. They do not control form — flatness, roundness, cylindricity — or orientation — parallelism, perpendicularity, angularity — or the true three-dimensional position of a feature relative to the datum scheme.

Geometric dimensioning and tolerancing (GD&T), using the symbolic system defined in BS EN ISO 1101, provides these controls. Key geometric tolerances in machining practice:

• Flatness: The entire surface must lie within two parallel planes separated by the flatness tolerance. Specified on sealing faces, precision mating faces, and any surface where waviness affects function
• Cylindricity: The bore or shaft must lie within two coaxial cylinders separated by the cylindricity tolerance. Specified on precision bores and journals
• Parallelism: One surface or axis must be parallel to the datum within the stated tolerance zone. Specified on faces that must be parallel for assembly or sealing
• Perpendicularity: A surface or axis must be perpendicular to the datum within the stated tolerance. Specified on bores that must be square to a face, or faces that must be square to each other
• True position: The centre of a hole or feature must lie within a tolerance zone (usually cylindrical) centred on the theoretically exact position from the datum scheme. The correct way to tolerance a bolt hole pattern — superior to ±X, ±Y coordinate tolerances for most applications
• Run-out / total run-out: Specified on rotating components — the surface must not deviate beyond the run-out tolerance when rotated about the datum axis. Used for shafts, flanges and any rotational surface

GD&T is a precise language — a feature control frame on a drawing has a specific, unambiguous meaning. The same cannot always be said of a note. Where the functional requirement can be expressed as a geometric tolerance, use the symbolic notation rather than a written note.

Special Notes — What Gets Missed

The notes section of a drawing is where requirements that cannot be expressed dimensionally are communicated. Common notes that are frequently omitted:

• Deburr and break sharp edges: Always include this unless sharp edges are functionally required. An unspecified edge state is a safety and sealing risk.
• Heat treatment: If the part requires heat treatment (case hardening, through hardening, stress relief) — state whether this occurs before or after final machining. Heat treatment after machining may cause distortion requiring a finish pass; heat treatment before machining means the hardened stock must be machined, increasing tool wear.
• Surface treatment: Anodising, hard chrome, electroless nickel, black oxide, zinc plate — state the process, the thickness where relevant, and whether masking of any features (threads, precision bores, sealing faces) is required during treatment.
• Identification marking: Part number, serial number, or heat number stamped or engraved — state the method (stamp, laser, electro-etch), location, character height, and depth where relevant. Do not leave this as an afterthought — engraving after surface treatment defeats the purpose.
• Inspection requirements: Dimensional report, CMM report, pressure test, NDT (dye penetrant, magnetic particle, ultrasonic) — state the requirement on the drawing. First article inspection vs. 100% inspection vs. spot check should be stated if it matters.
• Cleanliness: For fluid-carrying or precision components — maximum allowable particulate contamination class if relevant, or simply "components to be clean and free of machining debris, cutting fluid and swarf on delivery".

What to Do Without a Drawing

Sometimes a part is needed without the time or resource to produce a fully dimensioned drawing. In these situations, the minimum information that should accompany a STEP file to a machinist is:

1. Material grade — fully specified as above
2. General tolerance class — e.g. "BS EN ISO 2768-m"
3. Critical features — a written list of the features whose tolerances matter, with their individual tolerances explicitly stated
4. Surface finish requirement — a blanket Ra value, and any tighter requirement on specific surfaces called out explicitly
5. Thread specifications — for every tapped hole and threaded feature
6. Finish notes — deburr, surface treatment, marking
7. Mill certificate requirement — yes or no

This does not replace a drawing for any precision or safety-critical part. But it provides a machinist with enough information to quote and produce a part that has a reasonable chance of being correct first time.

Common Specification Mistakes

1. Writing "stainless steel" or "aluminium" as the material. The machinist will order what is cheapest or most available. This may not be the grade you need.
2. No general tolerance stated. Without a stated general tolerance, every machinist applies their own default — which varies. The result is inconsistent parts from different suppliers.
3. Applying tight tolerances everywhere. Specifying H7 bores and ±0.05mm on non-functional dimensions adds cost with no benefit and signals to the machinist that the designer does not understand their own part.
4. Incomplete thread callouts. "M12 thread" leaves pitch, class of fit and depth unspecified. Any of those three being wrong will cause assembly problems.
5. No datum scheme. Positional tolerances without a datum reference are meaningless. The machinist cannot inspect the part to a positional tolerance without knowing what the position is measured from.
6. Omitting surface finish on sealing faces. A sealing face machined to Ra 6.3 instead of Ra 1.6 will not seal. This is one of the most common causes of first-off rejection on valves, flanges and housings.
7. Not stating heat treatment timing. "Case harden" as a note does not tell the machinist whether to machine before or after hardening. The default assumption may be wrong.
8. Sending a PDF of the drawing without the STEP file. The machinist then has to create the 3D geometry from 2D projections before they can programme the part — adding time and introducing risk of geometry errors.

Summary

A good machined part specification tells the machinist everything they need to produce the part correctly without having to interpret, assume, or phone for clarification. Every query the machinist raises is either a delay, a risk, or both. The investment in a complete drawing and specification is recovered many times over in reduced reruns, faster first-off approval, and parts that assemble without adjustment.

The essentials: full material specification including grade, condition and certificate requirement; a general tolerance reference; explicit tolerances on all critical features using ISO fit designations where appropriate; surface finish stated on all machined faces; complete thread callouts; a defined datum scheme; and notes covering deburr, treatment, marking and inspection. Send the STEP file alongside the drawing. Do not rely on the machinist to make decisions that belong in the design office.