How to Prepare a Technical Drawing for CNC Machining
A drawing is the only contract between your design intent and the machine. This guide walks through the seven checks we run on every file that lands in our quoting queue, from view layout to thread callouts. It is written for design engineers and buyers who want fewer clarification emails and a first-pass part that fits.
Key takeaways
Start with the sheet, not the geometry
Most drawing problems start before anyone dimensions a feature. Set the sheet size to match the part: A3 for anything over 200 mm, A4 for small brackets and bushings. Then pick the scale so the part fills roughly two thirds of the frame. A 1:1 view of a 12 mm pin on an A3 sheet wastes space and hides the detail you actually care about.
The title block carries the part number, part name, current revision letter, material callout, and the name of the person who approved the release. Keep it filled in completely. If a shop has to guess which revision it is quoting, the quote stops. We have seen two-week delays caused by nothing more than a missing revision letter in the corner box.
Put the projection symbol in the title block. First-angle and third-angle produce mirror-image parts. Most of our North American customers use third-angle; European and Asian drawings often arrive as first-angle. The symbol removes all doubt. If your CAD tool exports only one convention, add a note next to the title block spelling it out.
List every file you are sending on the sheet: STEP, PDF, and any inspection report. The drawing is the authority when there is a conflict, and saying so explicitly on the sheet prevents a long email thread later. One short note — 'PDF governs, STEP is reference geometry' — is enough.
Choose the minimum set of views
A good drawing shows each feature once, in the view where it is clearest. Orthographic front, top, and right side cover most prismatic parts. Add an isometric view for orientation only, not for dimensions. When a feature is not visible in any of the three standard views, cut a section rather than adding a fourth and fifth view.
Section views are the right tool for internal pockets, cross-drilled holes, and O-ring grooves. Label them A-A, B-B, and mark the cut line on the parent view. Keep hatching consistent: the same part gets the same hatch angle in every section. If two adjacent parts are shown, use different angles or the reader will assume they are one piece.
Detail views handle small radii, undercuts, and thread relief. Circle the zone on the parent view, label it Detail C, and set the scale to 4:1 or 5:1. Do not dimension a 0.4 mm corner radius in a 1:1 view; nobody can read it, and the machinist will call you.
Hidden lines slow a drawing down. Leave them in only where they carry information the solid views do not. On a busy housing with twenty holes, hidden line clutter is the fastest way to get a wrong part. Use a section instead.
Dimension from datums, not from edges
Pick three datum features and stick to them. Typically A is the mounting face, B is a primary hole or slot, and C is a secondary edge. Every dimension that matters should trace back to that scheme. Chain dimensioning from one edge to the next accumulates error; a stack of five ±0.1 mm steps can put the last hole 0.5 mm out of place.
Dimension to the feature, not to the tool path. Say 'Ø10 H7 hole, 25 mm from datum B' rather than describing how to cut it. The machine shop chooses the tool, the speed, and the order of operations. If you specify the process, you own the result and you remove the shop's ability to optimize.
Keep units consistent and state them. Mixed metric and imperial drawings are a common source of scrapped parts. Put 'Dimensions in mm' in the title block, then never mix. If a legacy feature is truly imperial, call it out in a note rather than switching the whole sheet.
Avoid double dimensioning. The same distance given in two views, or in both a linear and an angular form, will eventually disagree after an edit. When the two values conflict, the shop has to stop and ask which one is correct.
Match tolerance to function
The title-block tolerance is a default, not a plan. A blanket ±0.1 mm on every dimension forces the shop to inspect everything to that band and drives cost up for no benefit. Reserve tight tolerances for the features that mate, seal, or locate. Everything else can run looser.
Use GD&T where position or form genuinely matters. A position tolerance of Ø0.05 mm at MMC on a bolt pattern tells us exactly what to control. Plus/minus dimensions on the same pattern leave the diagonal distance uncontrolled, and a mating plate may not fit.
Our general machining capability is ±0.005 mm, but that number should sit on the two or three features that need it. A part with a ±0.005 mm bore and ±0.1 mm everywhere else is normal. A part with ±0.005 mm on all forty dimensions will be quoted high and inspected slowly.
Angular tolerances are easy to forget. A 30° chamfer with no tolerance defaults to whatever the title block says, and on a long edge that can move the tip by a millimetre. Add the angular band when the chamfer meets another surface.
Step by step: seven checks before you send
- 11. Confirm the release stateCheck the revision letter in the title block matches the file name and the STEP. Re-export the PDF after any model change so the two never drift apart.
- 22. Verify the projection symbolThird-angle for North America, first-angle for most of Europe and Asia. If the symbol is missing, add a note stating which convention the views follow.
- 33. Walk the datum schemeTrace every tight dimension back to A, B, or C. If a dimension floats without a datum, re-anchor it. Chain dimensions should not exceed three links.
- 44. Audit the tolerance spreadMark which features need ±0.005 mm to ±0.02 mm and which can run ±0.1 mm. Move the tight band onto mating and sealing surfaces only.
- 55. Fix every thread calloutWrite nominal size, pitch, class, and depth: M6 × 1.0 - 6H, 12 mm deep. Add the tap drill note if the hole is blind and the depth is critical.
- 66. Set the finish per surfaceRa 0.8–1.6 μm covers most sealing faces; Ra 1.6–3.2 μm is fine for non-critical surfaces. State cosmetics on the specific face, not on the whole part.
- 77. Run a last read-throughPrint the PDF at 100% and read it on paper. Missing leaders, doubled dimensions, and stray notes show up on paper far more often than on screen.
What to call out, and how tight
Use this as a starting point, then adjust for the mating part.
| Feature | Typical callout | When to tighten |
|---|---|---|
| Mating bore | Ø20 H7 | Press fit or bearing seat: Ø20 H6 |
| Bolt pattern | Ø0.2 mm position | Locating dowels: Ø0.05 mm at MMC |
| Flat mounting face | 0.1 mm flatness | Sealing face: 0.02 mm flatness |
| Sealing groove | Ra 0.8 μm | Dynamic seal: Ra 0.2–0.4 μm |
| Cosmetic face | Ra 1.6 μm, no marks | Visible anodized part: note texture |
| Chamfer | 0.5 mm × 45° ±0.2 mm | Edge break for safety: 0.3 mm min |
| Blind thread | M6 × 1.0 - 6H, 12 mm deep | Thin wall: add drill depth note |
Common questions
Do I need a drawing if I send a STEP file?
For simple parts, a STEP file with a few notes can be enough to quote and cut. Once a feature has a tolerance, a thread class, or a surface finish requirement, that information has no home in the solid model. It has to live on a drawing or in a signed specification sheet.
Our rule is simple: the model carries geometry, the drawing carries intent. When they conflict, the drawing wins, and we say so on the quote.
How tight can tolerances realistically go?
Our general capability is ±0.005 mm on critical features, with surface finish down to Ra 0.2 μm where the process supports it. Those numbers apply to features you identify, not to every dimension on the sheet.
Tightening forty dimensions to ±0.005 mm does not improve the part. It increases inspection time, raises scrap risk, and slows the run. Put the tight band where the part functions.
What file formats should I send?
Send a STEP or Parasolid for the geometry, plus a PDF of the drawing. Native CAD files are useful for DFM review but should not be the only file. If you have an inspection report from a previous run, include it.
Large assemblies are better sent one part per file with clear names. A single PDF containing twelve drawings slows quoting and invites mix-ups.
How do I handle a part with no flat datum face?
Use a machined boss, a hole pattern, or a three-point target as your primary datum. Note it on the drawing as a target datum with the specific points called out.
Castings and forgings often need this treatment. Without it, the shop picks its own reference and your position tolerances shift with the setup.
Can you review the drawing before I release it?
Yes. Our DFM review runs on the first submission and comes back with the quote, typically within 12 hours. We flag missing datums, over-tight tolerance bands, thread callouts without depth, and features that will need a second setup.
The review is free and does not commit you to an order. Uploads are secure and confidential, and we can work under an NDA on request.
What about surface finish and color on the same part?
Call out the finish per surface and the color separately in the notes. Anodizing color and Ra value are different requirements and are often achieved at different steps.
If a face must stay raw for electrical contact or bonding, say so. Masking notes belong on the drawing, not in a separate email that gets lost.
Send the drawing, get a DFM read in 12 hours
Upload your PDF and STEP. We return a quote plus a free DFM analysis, and production can start within 24 hours.
12-hour quoteNo MOQ, one part to 10,000+100% inspection before shipment
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
