CNC Processing Drawings: What Buyers Should Check First

• 1
  Key takeaways
• 2
  What each drawing element costs you
• 3
  Start with function, not with the tightest number
• 4
  Tolerance stack-up: where drawings quietly go wrong
• 5
  GD&T: use it where it helps, skip it where it does not
• 6
  Surface finish and material callouts that survive quoting
• 7
  Drawing format, revision control and what to send
• 8
  How to compare quotes on CNC processing drawings
• 9
  7 checks before you send CNC processing drawings out

The most common mistake we see in incoming CNC processing drawings is a tolerance block that says ±0.01 mm everywhere because nobody wanted to think about which dimensions actually matter. Every one of those callouts gets machined the same way, inspected the same way, and priced the same way. On a 200 mm aluminum bracket, holding ±0.01 mm on an outside profile that bolts to a rubber gasket is wasted money.

Go through the part and mark the three to five dimensions that decide whether it works. A bearing bore. A mounting hole pattern. A sealing face. Those get the tight tolerance. Everything else can sit at ±0.1 mm and nobody will notice at assembly.

This is also where you decide the datum. Pick the surface that touches the mating part first, make it datum A, and build the rest of the chain from there. If your drawing has three datums all fighting for priority, the machinist has to guess which one to set up on.

One more thing: check that your tightest tolerance is actually measurable. If the feature is a 0.5 mm wide slot, a ±0.005 mm callout is not a spec, it is a wish. Contact measurement needs room for the stylus.

• 1
  Mark functional dimensionsCircle the 3–5 dimensions that control fit. Tighten only those.
• 2
  Set datum A from the mating faceThe first surface that touches the assembly is usually the right primary datum.
• 3
  Confirm the feature is measurableIf a CMM stylus or micrometer cannot reach it, the tolerance is unverifiable.

A drawing can look clean and still produce parts that do not assemble. This happens when tolerances are assigned dimension by dimension without checking the stack. Five dimensions at ±0.05 mm can add up to ±0.25 mm at the far end of a chain, which is often outside the fit you need.

There are two ways to handle this. The simple one is to tighten the chain. The better one is to re-dimension from a single datum so the tolerances do not stack. If hole A and hole B are both located from datum A, the distance between them varies by the sum of two tolerances, not by five.

For hole patterns, use position tolerance instead of plus/minus on X and Y. A true position callout of Ø0.1 mm M gives the shop a circular zone and lets them use the maximum material condition bonus, which is often cheaper than a rectangular ±0.05 mm box.

If the part goes into a fixture or a mating assembly, run the stack before you release the drawing. It takes twenty minutes and it prevents the rework loop that costs two weeks.

• 1
  Re-dimension from one datumLocate related features from the same reference to cut stack-up.
• 2
  Use true position for holesØ0.1 mm M gives a round zone and allows MMC bonus.
• 3
  Run the stack on paperAdd the worst-case deviations before you release the revision.

GD&T is a language, and like any language it only helps if both sides speak it. A well-applied flatness or perpendicularity callout tells the machinist exactly what the surface needs to do. A drawing covered in fourteen control frames that nobody inspects is worse than a simple plus/minus drawing, because it hides the two callouts that matter.

Use flatness when a surface needs to seal. Use perpendicularity when a bore has to sit square to a face. Use position for hole patterns. Use profile of a surface when a curved contour has to match a mating part. These four cover most machined parts.

What to avoid: concentricity when runout or position will do, since concentricity is harder to verify and rarely changes function. Avoid profile callouts on non-critical cosmetic surfaces. And avoid bilateral tolerance zones on a unilateral feature, which just confuses the setup.

If your shop does not have a CMM with the right software, a complex GD&T scheme becomes a negotiation at inspection time. Ask what they can measure before you finalize the frames.

• 1
  Flatness for sealing facesKeeps a gasket or O-ring seated without over-specifying the whole surface.
• 2
  Position for hole patternsSimpler to inspect and machine than stacked plus/minus dimensions.
• 3
  Skip concentricityRunout or position usually covers the same function at lower cost.

Finish is where quotes diverge the most. One shop reads "machined finish" as Ra 3.2 μm, another as Ra 1.6 μm, and the price difference is real. Write the Ra number on the drawing. As-machined is Ra 1.6–3.2 μm, a good production finish is Ra 0.8–1.6 μm, and fine finishing reaches Ra 0.2–0.8 μm. Each step adds time.

Material spec matters too. "Aluminum" is not enough. 6061-T6 and 7075 have different machinability, different distortion behavior, and different prices. On thin walls, 7075 will move more after machining than 6061. If the drawing just says aluminum, the shop picks what is on the shelf, and your fit may change.

Heat treatment and stress relief belong on the drawing if the part is thin or has tight flatness. A 4140 plate machined to ±0.02 mm flatness without stress relief will move after you ship it, no matter how good the setup was.

Finally, call out the finish process, not just the finish value. Anodizing adds thickness, typically 5–25 μm depending on type, and that changes a bore diameter. If a bore has to stay at tolerance after anodizing, mask it or machine it undersize.

• 1
  Write the Ra numberRa 0.8–1.6 μm is a normal production finish; finer costs more.
• 2
  Specify the alloy and temper6061-T6, 7075, 316L, 17-4PH. Not just "aluminum" or "stainless".
• 3
  Note anodize thicknessHardcoat can add 25 μm per surface. Mask tight bores.

Send a 3D model and a 2D drawing. The model defines the shape; the drawing defines the tolerances, datums, and finish. If you only send a STEP file, the shop has to guess every tolerance, and the quote will either be padded or wrong. If you only send a PDF, the shop has to rebuild the geometry, which adds a day and a risk of misreading a radius.

Keep one master revision. We regularly receive a drawing revision C with a model from revision B. The difference is usually small, but small differences on a tight feature cause scrap. Name both files with the same revision code.

Include a title block with material, finish, revision, and a contact for questions. Add a notes block for deburring, edge break, and any masking. Deburring is not optional on machined parts; if the drawing does not say it, someone still has to do it.

For assemblies, mark the critical interface dimensions on the individual part drawings, not only on the assembly. The machinist works from the part drawing, not the assembly.

• 1
  STEP plus PDFModel for geometry, drawing for tolerance and finish.
• 2
  Match revision codesSame rev letter on the model and the drawing file names.
• 3
  State deburring and edge breakA 0.3 mm edge break note prevents sharp edges and inspection arguments.

Two quotes for the same part can differ by 40 percent and both be honest. The difference is usually in what each shop assumed. One assumed a ±0.1 mm tolerance block, the other read your ±0.02 mm callout and added a finishing operation. Before you compare price, compare assumptions.

Ask each supplier to return the drawing with their DFM notes. A shop that flags a tight corner radius, a deep pocket, or an unmeasurable callout is reading your drawing. A shop that returns only a number is quoting a guess.

Check the inspection plan. For a part with a ±0.005 mm bore, you want a CMM report, not a caliper check. For a cosmetic part, you want a finish sample or a Ra reading. If the quote does not mention inspection, ask.

Certifications matter when your part goes into a regulated product. ISO 9001 covers general quality systems, IATF 16949 covers automotive, ISO 13485 covers medical devices, and ISO 27001 covers information security for your files. Match the certificate to your industry, not to the largest logo on the website.

• 1
  Compare assumptions, not just priceAsk what tolerance block and finish each shop quoted against.
• 2
  Request marked-up DFM notesA returned drawing with comments shows the quote was read.
• 3
  Match certification to industryIATF 16949 for automotive, ISO 13485 for medical, ISO 27001 for data.