Large integrated die-castings change the machining plan. Once the part cools, you are no longer cutting a small, rigid block—you are cutting a thin-walled, high-stiffness structure with uneven stock and residual stress. In practice, face milling should be split into rough and finish passes: rough with a Ø80–Ø100 mm face mill, 4–6 inserts, 1.5–2.0 mm depth of cut, and 0.15–0.25 mm/tooth feed; finish with a wiper insert at 0.3–0.5 mm depth and 0.08–0.12 mm/tooth. Clamping force must be controlled—over-clamping distorts the casting and spring-back after unclamping throws flatness out. Use floating supports or vacuum fixtures where possible, and verify flatness within 0.1–0.2 mm before drilling.
Drilling is where scrap risk concentrates. For Ø6–Ø12 mm holes in AlSi10MnMg-type alloys, run carbide drills at 80–120 m/min surface speed and 0.15–0.25 mm/rev feed, with through-tool coolant at 20–40 bar. Watch for porosity and cold shuts—they push the drill off-line and snap small tools. Peck drilling is not always needed, but a 0.5–1.0 mm pilot spot is. Position tolerance should be held to ±0.1 mm and hole diameter to H9–H10 where bolting interfaces demand it. Deburr immediately; burrs at parting lines and ejector marks are common on die-cast surfaces.
Tool life and thermal management decide cost per part. Keep a wear land limit of 0.2–0.3 mm on carbide inserts and change drills at 0.15 mm flank wear to avoid hole taper. Avoid dry cutting; minimum quantity lubrication is acceptable only for shallow milling. If you are quoting integrated die-cast machining, build in 10–15% extra cycle time for stock variation and probe checks. For more mold sourcing and machining supplier information, visit MoldSo at www.moldso.com.