You Can't Design Without Knowing Machining - Practical Machining Allowances and Geometric Limits

Milling corner radii (tool R), lathe center holes, grinding allowance (0.2–0.5mm), EDM limits, minimum ID grinding diameter, boring depth limits, undercuts/relief grooves — machining process constraints every designer must know

If a designer doesn't understand machining processes, drawings become disasters instead of blueprints. CAD can draw any shape, but machine tools have physical limits. To avoid hearing "this shape can't be machined" from the shop floor, master the following.

1. Milling — Internal Corners Must Have Radii

When milling pockets, internal corners always have a radius equal to the end mill radius. Perfectly sharp internal corners are physically impossible.

Practical rule: Internal R ≥ tool radius (typically R1–R3). Deep pockets (>3D depth) require larger R due to tool rigidity
Tip: If sharp corners are essential, switch to EDM or add relief cuts (dog-bone features) at corners

2. Turning — Don't Forget Center Holes

Long shafts (L/D > 4) on a lathe require center holes (KS B 1011 Type A/B) at both ends. Without specification on drawings, machinists improvise or skip centers, causing runout.

Practical rule: Ø10–30 shaft → A2.5 center, Ø30–60 shaft → A4 center
Tip: If center holes can't remain on finished parts, note "remove center holes after machining" or "center holes permitted" on the drawing

3. Grinding — Leave Stock Allowance

Grinding corrects post-heat-treatment distortion and achieves high precision (IT6 or better). Turning/milling stages must leave grinding stock.

OD grinding: 0.1–0.3mm per side on diameter (0.2–0.6mm total)
ID grinding: 0.1–0.25mm per side. Minimum bore Ø15 (small grinding wheel limit)
Surface grinding: 0.1–0.3mm per side. Up to 0.5mm if heat treatment distortion is large

4. EDM (Electrical Discharge Machining) — Not a Silver Bullet

EDM machines regardless of hardness but is slow and expensive. Surface finish Ra 1.6 or better needs additional finishing. Electrode (copper, graphite) fabrication cost must be factored in.

Wire EDM: Minimum corner R 0.1mm (based on Ø0.2mm wire). Ideal for through-cuts in plate
Sinker EDM: Micro-holes, complex cavities. Account for electrode wear (copper: 1–3%)

5. Boring — Depth and Diameter Limits

Boring bars develop chatter as the L/D ratio increases.

Practical rule: Standard boring bar L/D ≤ 4, anti-vibration boring bar L/D ≤ 7
Tip: For deep holes, consider BTA drills or gun drills. For tight tolerances, add honing

6. Undercuts and Relief Grooves — Essential for Grinding and Threading

Grinding wheels need relief grooves to reach shoulder faces. Threading also requires undercuts to avoid incomplete threads at the end.

Grinding relief groove: Width 3–5mm, depth 0.5–1mm (ref. JIS B 0612)
Thread undercut: Width = pitch × 2–3, depth = at or below minor diameter

💡 Expert Advice
"If you want to design well, visit the factory. A designer who has watched milling even once adds radii to pocket corners. A designer who has seen lathe work puts center holes on drawings. Staring only at a CAD monitor means forever drawing un-machinable parts."

Machining Allowance — US Casting and Forging Standards

NAFA (North American Aluminum Foundry Association) and SFSA (Steel Founders' Society of America) publish machining allowance tables for US castings. Typical: 1.5 mm allowance per surface for sand casting under 100 mm; 0.5 mm for investment casting; 3 mm for forgings under 200 mm. ASTM A788 governs forging tolerance.

Practical Application

For US-made castings, specify machining allowance on the as-cast drawing per AFS (American Foundry Society) recommendations. Common error: insufficient allowance on bosses or thin features, leading to "machine-thru" rejections. For 5-axis CNC of as-cast aluminum, 2 mm uniform allowance is typical; for steel forgings, 4 mm to allow for scale removal. Quality 1st-Inspection compares as-machined to nominal per ASME Y14.5.