How to Prepare a Technical Drawing for CNC Machining Quoting

Every week we get drawings that are missing basic information. The result: we have to email back asking for clarification, the quote gets delayed, and the pricing ends up with a risk premium because we had to assume the worst case on ambiguous tolerances.

Here's what we actually need to see on a drawing to quote accurately on the first pass.

1. Complete Dimensions (All of Them)

This sounds obvious, but you'd be surprised how often we get drawings with missing dimensions. If you're providing a 3D model (STEP/IGES), we can extract dimensions from that — but we still need the drawing for tolerances and notes. The 3D model shows the nominal geometry. The drawing shows what's acceptable.

2. Tolerances — Be Specific

A note in the title block that says "±0.1mm unless otherwise specified" is fine for general dimensions. But critical features need individual tolerance callouts. We need to know which surfaces mate with other parts, which holes are clearance vs. press-fit, and which features affect assembly.

If every dimension has ±0.01mm, the part becomes unnecessarily expensive. If no dimensions have tolerances, we have to assume the tightest your title block allows. Neither is ideal.

3. Material Specification

Don't just write "aluminium". Write "6061-T6" or "7075-T7351". The difference matters for cost, lead time, and machinability. Include the spec standard if applicable: ASTM B211, AMS 4127, etc.

If you're flexible on grade — consider noting that too. If you write "Aluminium 6061 or 6082", we can quote whichever is more available and cheaper.

4. Surface Finish Requirements

Specify Ra values for critical surfaces. Don't put Ra 0.4µm on a surface that's just a cosmetic face plate. Do put Ra 0.4µm on a sealing surface or a bearing bore. If you don't specify, we'll quote as-machined finish, which is usually Ra 1.6–3.2µm depending on material.

5. Thread Specifications

Don't just write "M6 thread". Write "M6×1.0 — 6H". Include depth: "M6×1.0 — 6H, 12mm deep, bottom tap" vs "M6×1.0 — 6H, through hole". Bottom tapping costs more and takes longer. If it doesn't need to be bottom tapped, don't specify it.

6. Quantity and Volume

Tell us the quantity. Even if it's a range: "1-5 for prototype, 500-1000 for production". This changes how we approach the job. For a prototype we use standard stock sizes and generic CAM. For production, we order custom stock lengths and invest in cycle time optimisation.

7. What NOT to Do

Don't dimension from multiple reference points. Pick one datum structure (per GD&T or simple X/Y baseline) and dimension everything from there. Every time we see dimensions from three different corners of the part, we know the designer didn't think about how the part will be machined.

Don't put critical tolerances on features that can't be measured. If the tolerance requires a CMM program, that's fine — just know it adds cost. If it requires a custom gauge, flag that early.

Don't over-specify. We've seen drawings with ±0.01mm on a chamfer that's just for deburring. That chamfer adds 30% to the inspection cost for zero functional benefit.