DFM-Checkliste für CNC-Teile: 18 Prüfpunkte vor der Freigabe

Most machining cost is decided in CAD, not on the shop floor. A part that has been designed with a cutter in mind can cost half as much as a functionally identical part that has not — same material, same tolerances, same quantity.

Here are the eighteen checks our process engineers run on every incoming drawing, in the order they usually find problems.

Internal geometry

1. Internal corner radii. A square internal corner cannot be milled. Every internal corner has a radius equal to the cutter radius. Specify a radius at least one third larger than the pocket depth divided by 8 — practically, use R3 or larger wherever you can. Going from R2 to R3 lets the shop use a 6 mm cutter instead of a 4 mm one, which typically cuts cycle time by 20 – 30 %.

2. Corner radius consistency. If every internal corner on the part shares one radius, the shop uses one cutter. Three different radii mean three tool changes per setup.

3. Floor radii in pockets. A pocket with a sharp floor-to-wall intersection requires a square-end mill running at reduced feed. Allow a 0.5 – 1 mm floor radius and the shop can use a bull-nose cutter at full feed.

4. Pocket depth to width ratio. Beyond 4:1 depth-to-cutter-diameter, tool deflection and chatter dominate. Beyond 6:1 you are paying for a special tool. If you need a 40 mm deep, 10 mm wide slot, consider whether it can be open-ended, or split into two components.

Walls and thickness

5. Minimum wall thickness. 0.8 mm in aluminium, 1.2 mm in stainless, 1.5 mm in plastics are realistic floors. Below that, the wall deflects away from the cutter and the dimension becomes unrepeatable.

6. Wall height to thickness ratio. A wall thinner than 1/15 of its height will vibrate. If you need a tall thin wall, add a rib, a lightening pocket on the opposite face, or accept a slower finishing pass.

7. Uniform wall thickness. Uneven walls distort after machining because residual stress is released unevenly. Keep walls within ±20 % of each other where you can.

Holes and threads

8. Hole depth to diameter. Standard drills reach 5× diameter comfortably. Beyond 10× you need gun drilling, which is a different process at a different price. A 3 mm hole 40 mm deep is a specialist operation; a 5 mm hole 40 mm deep is routine.

9. Thread depth. Threads deeper than 2× nominal diameter add cost and give no additional strength — the first three engaged threads carry most of the load. M6 × 12 deep is plenty; M6 × 30 deep is money spent for nothing.

10. Flat-bottom holes. A drill leaves a 118° or 140° point. A flat bottom requires a second operation with an end mill. Only call it out if the function needs it.

11. Thread callout completeness. State the standard (M, UNC, UNF, BSP, NPT), the class (6H, 2B), the depth and whether it is through or blind. "M6 tapped" leaves four questions unanswered.

12. Hole position tolerance. Use position tolerance with datums rather than ± on X and Y coordinates. It describes what you actually need and gives the shop a larger, correctly shaped tolerance zone.

Setups and access

13. Count the setups. Look at your model and count how many directions a cutter must approach from. Each direction is a setup; each setup adds fixture time, cost and a tolerance stack. Features on five faces are routine on a 5-axis machine; features on six faces always need at least two operations.

14. Undercuts. Internal undercuts require special tooling or EDM. Check whether the undercut is functional or a leftover from a casting-derived model.

15. Tool access to the deepest feature. A pocket that a cutter cannot reach without a 60 mm long tool will chatter. Ask whether the feature can be opened up, approached from another face, or split across two parts.

Datums and drawing hygiene

16. Datum scheme. Define A, B and C as real, contactable surfaces large enough to sit on. A datum on a 2 mm wide edge is not a datum, it is an argument waiting to happen.

17. One controlling document. Decide whether the 2D drawing or the annotated 3D model governs, and say so. Conflicts between the two are the single most common cause of rejected parts in our experience.

18. Material and finish on the drawing, not in the email. Material specification, heat treatment condition, surface finish, edge break and any required certifications belong on the drawing where they will still be found in two years.

What this is worth

On a typical enclosure or manifold, applying these checks before release saves between 15 % and 40 % of the machined cost. On a part going into production, the saving multiplies by every unit you will ever buy.

Send us your model before you release it and we will run this checklist and return specific, costed suggestions — not "reduce complexity", but "open this radius from R2 to R3 and save 22 minutes of cycle time per part."