Mold CNC machining guide: basic steps from CAD to first shot

• 1
  What matters most in a mold build
• 2
  Why the mold CNC machining guide starts with geometry, not the machine
• 3
  From CAD to toolpath: what happens before the spindle turns
• 4
  Roughing, semi-finishing and finishing the cavity
• 5
  Fit, spotting and bench work before the tryout
• 6
  Inspection, materials and where first shots drift
• 7
  Step by step: cutting a mold cavity
• 8
  Which process for which mold feature

Every mold shop owns machines that can hold ±0.005 mm on a good day. The reason two shops quote the same part at different prices is usually not the machine. It is how much of the cavity a cutter can actually reach. A deep rib 4 mm wide and 30 mm tall needs a cutter long enough to get down there and stiff enough not to deflect. Most of the time it cannot be both.

So the first question in any mold CNC machining guide is: what shape is this, and how do we hold it? A shallow core with open faces cuts fast on a 3-axis mill. A cavity with undercuts, side actions or curved parting lines usually needs simultaneous 5-axis work, or a reposition plus a second setup. Molds for large panels, housings and structural parts can run up to 4,000 mm on our long-travel machines.

Draft is the other early decision. Without 1–3° of draft on the walls, the part will drag and scuff on ejection no matter how well the steel is polished. Draft costs nothing at the CAD stage. Adding it after heat treatment means welding or re-cutting, and both are expensive.

Material closes the loop on the plan. Aluminium 6061 or 7075 is fine for prototype tooling and low-volume runs. Pre-hardened steel such as 4140 or 4130 suits medium runs. For high-cycle production the cavity is often hardened tool steel, and then milling is only half the story: the deep corners go to EDM after heat treatment.

• 1
  Open geometry3-axis milling, fewer setups, lower cost
• 2
  Undercuts and side actions5-axis or repositioning, plan fixtures early
• 3
  Sharp internal cornersLeave for EDM, do not force a small cutter

A mold build starts with a 3D model of the molded part, not the mold. The tooling engineer applies the shrinkage factor first, because every later operation works from the scaled solid. Crystalline plastics such as POM, PA and PP shrink far more than ABS or PC, and the rate also depends on wall thickness and gate location. Get this wrong and the mold is scrap.

Next comes parting line placement. The line decides which side of the tool carries the ejector pins, where the gate sits, and how the two halves seal. A poor line shows up as flash at the split, often on a visible cosmetic surface. Review it with a mold flow check if the part has thin ribs or long flow paths.

The CAM programmer then builds the toolpath from the scaled solid. Roughing runs a large-diameter insert cutter to remove bulk. Semi-finishing brings walls to a uniform stock allowance. Finishing uses a smaller ball or bull-nose cutter for the final surface. Every tool change should be planned so the remaining stock is smaller than the previous cutter radius, or you leave uncut ridges.

Before any of that, send the part model for a DFM review. We return a quotation and free DFM analysis within 12 hours, which usually flags draft problems, thin walls and corners that no cutter can reach.

Roughing removes most of the volume. On a 3-axis or 4-axis mill with a Ø50 mm or Ø63 mm face mill, you can take 1–3 mm depth of cut in aluminium and 0.5–1.5 mm in pre-hardened steel, depending on the insert grade and spindle load. Leave 0.3–0.5 mm of stock on all walls and floors for later passes. Cutting to final size here only creates chatter marks that finishing cannot remove.

Semi-finishing follows with a smaller cutter, typically Ø12–Ø20 mm, to even out the stock left by the roughing tool. This is the pass that decides whether the finishing cutter sees a consistent load. Skip it and the finishing pass will show witness lines where the load changed.

Finishing uses a ball-nose or bull-nose cutter at a stepover of 0.05–0.2 mm on cosmetic surfaces. That range gives Ra 0.8–1.6 μm on steel and can reach Ra 0.2–0.8 μm with a finer stepover and a good machine. A simultaneous 5-axis center keeps the cutter normal to the surface, which holds a constant stepover on curved walls and avoids the faceting you get from a 3-axis raster.

Hardened cavities go a different route. After heat treatment, milling a 50 HRC surface is slow and hard on tooling. Most shops leave 0.2–0.5 mm for the sinker EDM and cut the deep ribs and sharp corners by electrode. Plan the electrode count early, because each one needs its own rough and finish pass.

Machined plates are not a mold yet. The cavity and core blocks must sit in their pockets with the correct shut height, and the leader pins and bushings must align the two halves repeatably. Interference here shows up as heavy wear on the pins after a few thousand cycles.

Spotting is the step where the two halves are mated and checked with blueing. High spots appear as dark contact patches and are stoned or ground down by hand. This is slow, skilled work. A cavity that reads perfectly on the CMM can still show uneven contact because of plate flatness or clamping distortion.

Then come the moving parts: ejector pins, slides, lifters and the sprue puller. Every one needs to move freely by hand before the mold goes near a press. Pins that bind will gall the hole, and a seized lifter can crack a cavity block on the first cycle.

Finally, cooling lines are pressure-tested and the water circuit is checked for leaks and flow balance. Uneven cooling is the most common cause of warpage in the first shots, and it is far cheaper to fix on the bench than after the customer measures parts.

• 1
  Shut heightCheck both halves in the press platens before clamping
• 2
  Ejector travelConfirm full pin stroke clears the part without over-travel
• 3
  Water flowBalance circuits so each zone reaches a similar temperature

Inspection runs through the whole build, not just at the end. We check incoming material, monitor dimensions in process and inspect 100% of critical features before shipment, with reports on request. CMM work on the cavity is done with the block at a stable temperature, because a 300 mm steel block moves about 0.003 mm for every 1 °C change. Measuring a hot block is a common source of false out-of-tolerance calls.

Material choice is a cost-versus-cycle decision. Aluminium 6061, 6061-T6 or 7075 cuts fast and takes a good polish, which suits prototype and bridge tooling. Pre-hardened 4140 or 4130 handles medium runs without heat treatment. For high-cycle tools, hardened tool steel lasts far longer but pushes corner work to EDM and adds lead time.

Surface finish follows the same logic. As-machined surfaces run Ra 1.6–3.2 μm. A finish pass at a tighter stepover reaches Ra 0.8–1.6 μm, and Ra 0.2–0.8 μm usually needs a finer stepover plus polishing. For transparent or high-gloss parts, budget bench time for diamond polishing regardless of how good the toolpath was.

First-shot drift is normal and it is how you learn. Typical causes are short shots from venting, warpage from uneven cooling, or a dimension that moved because the shrinkage assumption was slightly off. Measure the shots, compare against the scaled model, and decide whether the fix is a steel change or a process change. Most of the time it is process.

• 1
  Temperature stabilityLet blocks settle before CMM, especially large plates
• 2
  VentingAdd vents at the last point to fill, not only at the parting line
• 3
  Cooling balanceMeasure outlet temperatures zone by zone