CNC Mold Parts Processing: How Mold Components Are Machined

• 1
  Key takeaways
• 2
  What CNC Mold Parts Processing Actually Covers
• 3
  Where Tolerance Really Belongs on a Mold Drawing
• 4
  How the Cutting Sequence Is Built
• 5
  Fits, Shrinkage and the Assembly Side of Mold Parts
• 6
  Step by Step: From Block to Finished Mold Part
• 7
  Tolerance and Finish by Mold Feature

A mold is not one part. It is a stack of machined components that must locate against each other within microns and still open and close a few hundred thousand times. CNC mold parts processing is the cutting work that turns blocks of steel, aluminium or copper alloy into the cavity insert, the core, the slides, the lifters, the ejector plates, the runner plate and the leader-pin bores that hold the whole assembly in line.

The work splits into two phases, and confusing them is the most common mistake we see in incoming drawings. Phase one cuts soft stock: pockets, screw holes, water lines, rough cavity forms, locating bores. Phase two happens after heat treatment and grinds or mills the sealing faces, the parting line, the shutoffs and any surface that touches plastic. Dimensions that only matter in phase one can be loose. Dimensions that seal must be tight.

Mold shops care about a short list of features. Cavity and core geometry sets the part shape. Shutoffs and parting lines stop flash. Sliding surfaces on slides and lifters set wear life. Guide-pin and guide-bushing bores set alignment. Ejector-pin holes set whether the part releases cleanly or drags. Cooling channels set cycle time. Each of those has a different tolerance appetite, and a good drawing says so instead of stamping the same ±0.01 mm on everything.

Most of the steel we cut for tooling is P20, 718H, NAK80, H13, S136 and 1.2344. Pre-hardened grades around 30–38 HRC machine well with carbide and hold a polish. Hardened grades at 48–52 HRC need CBN or coated carbide and lighter stepovers. Copper alloys such as beryllium copper are used where heat has to leave a hot spot fast, and they cut very differently from steel: higher surface speed, sharper edges, no dwell.

GreatLight runs 127 high-precision CNC machines across three wholly-owned plants, including 16 simultaneous 5-axis machining centers, 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers. Maximum processing size reaches 4,000 mm, so large mold bases and long inserts are not a problem. We hold ±0.005 mm on critical features and Ra 0.8–1.6 μm as a standard machined finish, with Ra 0.2–0.8 μm available on request.

Toolmakers do not treat every dimension the same, and neither should a drawing. Split the features into three groups before you dimension anything. Sealing features carry the tightest numbers. Locating features carry a fit callout. Everything else is general tolerance.

Sealing features are the parting line, shutoffs, the gate land, and any face where two steel surfaces must meet under clamp pressure. These get the tightest callout, typically ±0.005 mm on flatness and parallel, and they get ground or milled after heat treatment. If the drawing leaves the parting line at general tolerance, the tool will flash and someone will spend a week spotting it in by hand.

Locating features are guide-pin bores, guide-bushing bores, leader-pin holes and dowel holes. Here a fit callout beats a plus-minus number. An H7 bore for an h6 pin tells the machinist the clearance range and the surface finish in one symbol. A ±0.01 mm number on the same bore tells them almost nothing about how the pin will actually seat, because it does not define the hole size distribution.

Wear surfaces on slides and lifters want a different treatment again. The critical dimension is not absolute size but the fit between the slide and its pocket, plus the surface finish that decides whether it galls. Hard-chrome plate or a nitrided surface plus Ra 0.4 μm on the sliding face buys more life than tightening the size tolerance by another 5 μm.

Cooling channels are the exception that proves the rule. Their diameter and position matter, but their finish does not. A drilled water line at Ra 3.2 μm moves heat just as well as a reamed one at Ra 1.6 μm. Spend the money on shutoffs instead.

The sequence follows the heat treatment, not the geometry. Everything that can be cut in the annealed state is cut first, because annealed steel removes three to five times faster and does not wear the tool. That means roughing the cavity, drilling water lines, cutting screw holes and dowel holes, and pre-boring the guide-pin locations with stock left for finishing.

After heat treatment, the part comes back at 48–52 HRC and the rules change. Depth of cut drops, spindle speed rises, and the tool path avoids sharp internal corners where a small-radius cutter would chatter. We leave 0.2–0.3 mm of stock on sealing faces for grinding and 0.05–0.1 mm on cavity surfaces for the finishing pass. Trying to leave less usually means the heat-treat scale eats the allowance.

Hard milling has largely replaced ram EDM for cavities that used to be burned. A coated carbide ball nose at 8,000–12,000 rpm with a 0.1–0.3 mm stepover can hold ±0.01 mm on a 50 HRC cavity and leaves a finish that polishes in a fraction of the time. EDM still wins where geometry needs a sharp internal corner, a deep rib narrower than 1 mm, or a surface that a ball nose cannot reach. The choice is geometry-driven, not habit-driven.

For parts with angled faces, undercuts or features on several sides, 5-axis machining changes the economics. One setup on a simultaneous 5-axis center can reach five faces of a core block without re-fixturing. On a 3-axis machine the same part needs three or four setups, each one adding a datum shift and a chance to lose the relationship between the cavity and the guide bores. When the tolerance between those features is tight, the extra setups cost more than the 5-axis time.

A mold insert that measures perfectly on its own can still fail in assembly. The reason is usually stack-up. Every plate in the stack has a thickness tolerance, every pocket has a depth tolerance, and they add. If the cavity insert sits 0.03 mm proud of the plate, the clamp load goes into the insert instead of the parting line and the tool crushes itself over time.

Pocket depth is where we see the most stack-up trouble. A common approach is to machine the insert pocket to a depth that leaves the insert 0.02–0.05 mm below the plate surface, then shim or spot it in. Shims sound crude, but they let the toolmaker correct a stack-up after assembly without re-cutting steel. Drawings that call for a dead-flush insert with no adjustment range leave no room to fix anything.

Shrinkage is the other assembly-side number. Cavity dimensions are cut oversize by the resin shrinkage factor, which runs roughly 0.4–0.7% for unfilled ABS and PC, and drops to 0.2–0.4% or lower for glass-filled grades. The exact value comes from the resin supplier and the wall thickness, not from a generic table. Cutting the cavity to nominal and hoping the molder compensates is a mistake that costs a re-cut.

Guide pins and bushings set alignment, and their fit is a wear decision. A tighter fit holds the parting line better when the tool is new but galls sooner if lubrication is marginal. A slightly looser fit runs cooler and lasts longer but lets the plates shift a few microns under off-center injection pressure. For a tool that runs millions of cycles, the looser fit with good lubrication is usually the right call.