Drawing Standards

How to Draw for CNC Machine Work: A Practical Guide

A CNC-ready drawing is not a pretty 3D render. It carries the datum scheme, tolerance bands, thread callouts and finish specs that let a machinist cut your part without guessing. This guide is for design engineers and buyers who need to know how to draw for CNC machine work and what to check before release.

Get Instant Quote Talk to an Engineer

Datum logicGD&T calloutsSTEP + PDFDFM check

On this page

Key takeaways

Model and drawing do different jobsThe 3D model defines geometry; the drawing defines which features are critical and how tight they must be.

Pick datums before dimensionsChoose 2-3 functional faces as A, B, C. Everything else references them, not an arbitrary corner.

Tolerance the function, not the whole partA ±0.005 mm band on an entire bracket triples cost. Apply it only where fit matters.

Send STEP plus PDFSTEP drives toolpaths, PDF carries notes. A PDF alone forces the shop to remodel your part.

Note threads, not just holesM6 × 1.0 depth 12 mm is machinable. A shaded hole with no pitch callout is not.

Core principles

What Makes a Drawing CNC-Ready

A CNC drawing has one purpose: remove ambiguity. The machinist sees a model, a tool list, and a set of notes. If any feature can be read two ways, you will get a call or a wrong part. The core principle is that every dimension must describe a real measurement the operator can take on the machine or on a CMM.

Start with function. Write down which faces mate, which holes take a bearing, which surfaces seal. Those features get tight tolerances and explicit datums. Cosmetic surfaces and clearance holes get general tolerances from the title block. This split is what separates a drawing that machines cleanly from one that generates fifteen clarification emails.

Units must be stated once and never mixed. Metric drawings use millimeters; if you must show inches, put them in parentheses on a secondary line. Never dimension a part partly in inches and partly in millimeters. Operators convert one unit set, not two.

The title block carries the rest: material grade, quantity, general tolerance, surface finish default, and revision. For a part like the one in our custom auto spare parts 5-axis work, material grade alone can shift tool selection, so spell out 6061-T6 rather than writing aluminum.

1
One unit systemMillimeters, stated in the title block.
2
Function-driven tolerancesTight only where fit or sealing matters.
3
No redundant dimensionsDimension each feature once to avoid stacked conflicts.
4
Revision controlEvery release gets a number and a date.

Datums and dimensions

Choosing Datums and Dimension Scheme

Datums are the reference frame for inspection. Pick the primary datum A on the largest stable face, usually the one that sits flat on the vise or fixture. Datum B is a secondary face perpendicular to A, and datum C is a third face or a pair of holes that locks rotation. With A, B, C defined, every GD&T callout has a measurable home.

Dimension scheme follows the same logic. Use baseline dimensions from datums when several features relate to one edge, and chain dimensions only for a row of equally spaced holes. Mixing the two on the same face creates stacked tolerance error, where each link adds to the next and the far feature drifts out of band.

Avoid dimensioning to a corner that gets deburred or chamfered. If the reference edge is removed, the measurement disappears with it. Dimension to a machined face or a datum hole instead.

For parts that mount to another assembly, define the mating interface as datum A and dimension from it. This is standard practice on the aerospace prototype work we run, where a bracket must align to an existing frame. The drawing then reflects how the part is actually used.

1
A on the flat faceLargest stable surface that clamps well.
2
B perpendicular to AControls tilt and one rotational axis.
3
C locks rotationUsually a hole pattern or a second edge.
4
Baseline over chainPrevents stacked tolerance drift.

Callouts

Tolerances, GD&T and Finish Callouts

General tolerance blocks are efficient but crude. A common block of ±0.1 mm on a 100 mm part is workable; ±0.05 mm on everything is not, because it forces extra setups and slower passes. Reserve tight bands for the features that need them, and let the rest ride on the general block.

GD&T pays off when you care about position rather than size. A bolt hole circle is better controlled with a position tolerance of Ø0.2 mm MMC than with plus-minus coordinates, because it allows the bonus tolerance from hole size and matches how a functional gauge checks the pattern.

Flatness and perpendicularity matter on sealing faces and mating flanges. Call them out with a value and a datum reference. A surface without a flatness callout is only as good as the general tolerance block, which may be looser than your seal can accept.

Surface finish sets both function and cost. Ra 1.6–3.2 μm is the as-machined default for most milled faces. Ra 0.8–1.6 μm suits bearing seats and sliding surfaces. Ra 0.2–0.8 μm requires finer passes or lapping and is reserved for sealing or optical contact. Mark the finish symbol only on surfaces that need it.

1
General blockDefault ±0.1 mm unless noted otherwise.
2
Position over coordinatesBetter for hole patterns and mating pins.
3
Flatness on sealsSpecify value and datum on sealing faces.
4
Finish by functionRa 0.8–1.6 μm for bearing seats, coarser elsewhere.

Notes and files

Thread Notes, File Formats and Deliverables

Thread callouts need three pieces of information: nominal size, pitch, and depth. M6 × 1.0 depth 12 mm is complete. M6 alone leaves the pitch open, and a shaded hole in the model does not tell the operator whether it is tapped or reamed. Use the standard note format so the CAM programmer can pick the tap and the peck depth without a question.

Counterbores and countersinks need their own notes too. A c'bore Ø12 × 6 deep for an M6 socket head cap screw is clear. A shaded recess is not. If you use a standard fastener, name the standard, for example ISO 4762 M6 × 20, so the shop can verify clearance.

File format matters as much as the drawing. Send a STEP AP214 or AP242 file for the solid, plus a PDF of the drawing for notes and tolerances. Native CAD files are welcome but not required. A PDF alone forces the shop to remodel the part from scratch, which adds hours and risk.

Add the quantity and any finish requirements to the package. If you need anodizing or laser marking, say it up front. Laser marking has a minimum character height of 1.5 mm, so plan the marking layout accordingly. For assemblies, include a simple exploded view or a note that lists the mating parts.

1
Thread formatM6 × 1.0 depth 12 mm, always with pitch.
2
Fastener standardName ISO or DIN number for clearance checks.
3
STEP + PDFAP214 or AP242 solid plus annotated drawing.
4
Finish in notesAnodize type, color, and marking height.

Workflow

Step by Step: Building the Drawing

1
1. Define the function of each featureList mating faces, bearing bores, sealing surfaces and clearance holes. Mark them on a sketch before opening CAD. This list drives every tolerance decision later.
2
2. Model the part as a solidBuild a clean parametric solid with sharp internal corners where possible. Avoid zero-thickness walls and long thin ribs under 1 mm. Keep fillets consistent so the CAM programmer can use one tool.
3
3. Set datums A, B, CPick the primary mounting face as A, a perpendicular face as B, and a hole or second edge as C. Attach GD&T to these datums, not to arbitrary corners.
4
4. Dimension only what mattersApply tight tolerances (±0.005 to ±0.02 mm) to functional fits. Leave everything else on the general block, typically ±0.1 mm. Remove duplicate dimensions that conflict.
5
5. Add GD&T calloutsUse position for hole patterns, perpendicularity for upright faces, and flatness for sealing surfaces. Reference the datums you set in step 3. Keep the callouts readable, not stacked.
6
6. Write thread and feature notesCall out every tapped hole with size, pitch and depth. Note counterbores, countersinks and any required fastener standard. Add surface finish symbols to functional faces only.
7
7. Complete the title blockFill in material grade, quantity, general tolerance, units, default finish, revision and date. Sign and release. Missing title block data is the most common cause of quote delays.
8
8. Export STEP plus PDF and reviewExport a STEP AP214 or AP242 file and a PDF drawing. Check that the model and drawing match. If you can, run a DFM review before sending; it catches thin walls and deep pockets early.

Decision table

Which Tolerance and Finish to Call Out

Match the callout to the function. Tighter than needed adds cost without adding value.

Feature type	Typical tolerance	Finish	Why
Bearing bore	±0.005 to ±0.01 mm	Ra 0.8–1.6 μm	Controls fit and running clearance
Bolt clearance hole	±0.1 mm	Ra 1.6–3.2 μm	Only needs to pass the fastener
Sealing face	Flatness 0.02 mm	Ra 0.2–0.8 μm	Prevents leak paths under pressure
Mating flange	±0.02 mm	Ra 0.8–1.6 μm	Aligns two assemblies without shimming
Cosmetic surface	General block	Ra 1.6–3.2 μm	Appearance only, no fit function
Threaded hole	Class 6H	As tapped	Pitch and depth must be noted
Slot for adjustment	±0.05 mm	Ra 1.6–3.2 μm	Allows travel without binding

Get the drawing right, and the part follows

A clean drawing with clear datums, functional tolerances and complete notes is the cheapest tool you will ever use. Send us your STEP and PDF for a free DFM review and a quote within 12 hours.

Get Instant Quote Talk to an Engineer

FAQs

Frequently Asked Questions

What file formats should I send for a CNC quote?

Send a STEP AP214 or AP242 solid model plus a PDF drawing with notes and tolerances. Native CAD files are fine as a backup. A PDF alone is not enough because the shop would have to remodel the part.

How tight a tolerance can a CNC shop actually hold?

On a well-fixtured 3-axis or 5-axis machine, ±0.005 mm is achievable on critical features. The limit depends on feature size, material and access. Very deep pockets or thin walls may need a looser band. Always ask before locking in a number.

Do I need GD&T on every drawing?

No. Simple parts with a few fits work fine with plus-minus dimensions and a general tolerance block. GD&T earns its place on hole patterns, mating interfaces and any feature where position matters more than size.

How do I note a tapped hole correctly?

Give nominal size, pitch and depth: M6 × 1.0 depth 12 mm. Add the thread class if it matters. Never rely on a shaded hole in the model to convey that a hole is tapped.

What surface finish should I specify?

Start with Ra 1.6–3.2 μm as the as-machined default. Use Ra 0.8–1.6 μm for bearing seats and sliding surfaces. Reserve Ra 0.2–0.8 μm for seals and optical contact, since it adds finishing time.

Can the shop help fix my drawing before machining?

Yes. A DFM review checks wall thickness, tool access, thread depth and tolerance stack before the first cut. Catching these at the drawing stage avoids a second setup or a rework loop.