CNC machining after die casting brings selected features from the as-cast tolerance of ±0.1 mm to ±0.02 mm, with Ra 0.8 µm surface finish against Ra 1.6 to 3.2 µm as-cast. The right scope is 10 to 25% of the casting's surface area: leave 0.5 to 1.0 mm of allowance on flat faces, hold cuts on pressure-tight surfaces inside the dense 0.3 to 0.5 mm chill layer, and locate the first operation on cast datum pads placed in the fixed die half. Cast aluminum carries 7.5 to 12% silicon as hard particles at 1,000 to 1,150 HV, which abrades cemented carbide steadily, so PCD tooling at 600 to 1,200 m/min lasts 10 to 20 times longer on production volumes.
Die casting is a near-net-shape process, not a net-shape one. Every external wall carries 1 to 2° of draft because the part has to eject, cast holes are tapered and deliberately undersized, and as-cast flatness runs about 0.1 mm per 100 mm. None of that is a defect. It is the price of forming a complex shape in 20 to 100 milliseconds, and it means a casting arrives with its geometry finished and its interfaces unfinished.
This article is about the operation that finishes those interfaces: what to machine, how much stock to leave, where the porosity is, and why cast aluminum is harder on cutting tools than the 6061 most engineers have machining intuition for.
It covers machining of castings. Machining aluminum parts from solid billet is a different process with a different alloy set, and it belongs to our sibling operation at CharMax Precision CNC machining, which works in 6061, 7075, 5052 and MIC-6.
Why a casting needs machining at all
Five characteristics create the requirement, and each is inherent to high pressure die casting rather than fixable through process parameters.
| Cast characteristic | Typical value | What it rules out |
|---|---|---|
| Draft on every external wall | 1-2° external, 2-3° internal | Any face that must be flat and square to a datum |
| Linear tolerance | ±0.1 mm for the first 25 mm, widening with length | Bearing seats, dowel locations, tight stack-ups |
| Parting line mismatch | ±0.1 to ±0.15 mm added across the line | Dimensions taken between the two die halves |
| Flatness | 0.1 mm per 100 mm | O-ring and gasket faces, which want 0.05 mm or better |
| Surface roughness | Ra 1.6-3.2 µm | Dynamic seals and thermal interfaces, which want Ra 0.8 µm or finer |
The useful question is never whether a casting needs machining. It is which features do, and the answer is usually 10 to 25% of the surface area. Machining more than that throws away the economics that justified the die in the first place, because secondary machining is typically the largest single line in a cast piece price.
What to cast and what to machine
| Feature | Cast or machine | Reason |
|---|---|---|
| Outer walls, cosmetic surfaces | Cast | The as-cast skin is the densest and best-looking material on the part |
| Ribs, bosses, cable routes, gasket lands | Cast | Free in the steel, and no incremental piece cost |
| Non-critical holes above 4 mm | Cast, cored | A cored hole with 2-3° draft needs no machine time |
| Holes below 3 mm diameter | Machine | Core pins that slender break and heat-check the die |
| Holes deeper than 4× diameter | Machine | Long core pins deflect, wear and fail early |
| Threaded holes | Cast pilot, then tap | Internal threads cannot be cast in HPDC |
| Bearing and seal bores | Machine | ±0.1 mm as-cast cannot hold an H7 fit |
| Sealing faces below 0.1 mm flatness | Machine | Cast faces bow with length and carry draft |
| Mounting datums at ±0.1 mm | Cast | Already inside standard capability |
| Mounting datums at ±0.02 mm | Machine | Only machining reaches this |
| Side features and undercuts | Either | A slide is $2,000-5,000 of tooling; a milled slot on a face already in the fixture is often cheaper below 15,000 units a year |
The last row is the one worth arguing about on every part, because it trades tooling cost against per-part cycle time and the crossover moves with volume. The wider set of decisions that shift a part’s cost between the die and the machining cell is covered in how to reduce aluminum die casting cost.
Machining allowance
Allowance is the stock deliberately left on a cast face so it can be cut to final dimension. It is a genuine optimisation rather than a safety margin, because it has a penalty in both directions: too little and the cutter fails to clean up the as-cast surface everywhere, leaving witness patches; too much and the cutter goes through the good material into the poor material.
That asymmetry deserves stating plainly. The as-cast skin is the best material in the casting. Rapid solidification against the cold die produces a fine-grained, near fully dense layer roughly 0.3 to 0.5 mm thick. Below it the grain coarsens and both gas and shrinkage porosity increase. Machining is therefore a process of removing the part’s strongest material to reach a dimension, and the design goal is to remove as little of it as the tolerance allows.
| Feature | Allowance | Reason |
|---|---|---|
| Flat face up to 100 mm | 0.5-0.8 mm | Covers cast flatness plus cast position tolerance |
| Flat face over 150 mm | 0.8-1.2 mm | Cast flatness accumulates with length |
| Bore to be finish machined | 1.0-1.5 mm on diameter | Removes draft and the taper inherent to a cored hole |
| Cored hole to be tapped | Cast 1.0-1.5 mm under tap drill | The drill must cut full depth to remove draft before the tap enters |
| Fastener seating pad | 0.5 mm | Small area, cleans up reliably with minimal stock |
| Datum pad | 0.5-0.8 mm | Slightly heavier so it can be skimmed into a true reference first |
| Any face that must stay pressure tight | 0.3-0.5 mm | Deliberately minimal, to keep the cut inside the chill layer |
Specify allowance per feature on the casting drawing, not globally, and mark the faces that stay as-cast so no stock is added where none is needed.
Porosity: the risk that decides where you can machine
Every high pressure die casting entrains some gas. It is controlled to acceptable levels and usually invisible, but it is present, and it is not evenly distributed. Gas and shrinkage porosity concentrate in the last regions to solidify: the thickest sections, the thermal centre of any heavy boss, and the areas furthest from the gate.
Remove the chill layer over one of those regions and the porosity appears as pits on the machined face. On a bracket that is cosmetic. On a hydraulic sealing face it is a leak path, and it will be found by a leak test rather than by an inspector.
Designing machined faces away from porosity
The critical point is that this is settled at die design stage, not at the machine. Once the gate is cut, the location of the last-to-freeze region is fixed in steel. Moving it costs a die modification; moving your machined face costs a drawing revision. So the two decisions have to be reviewed together, which is the practical reason the machining plan and the flow simulation are looked at in the same meeting rather than in sequence.
Five rules that come out of that review:
- Put machined faces on walls of uniform thickness, not on heavy bosses. A boss thick enough to have a thermal centre will have porosity at that centre, and a face milled across it will find it.
- Where a thick boss must be drilled, size the cored hole so the drill removes the thermal centre entirely rather than exposing it in a wall.
- Keep machined sealing faces away from the gate and the biscuit. Oxide films and the leading edge of the fill front collect near both.
- Position overflows so the gas-rich leading metal ends up in material that gets trimmed off, not underneath a face you intend to cut.
- Specify A360 aluminum where the part must be pressure tight. Its low copper content and better feeding behaviour give the best pressure tightness of the common die casting alloys.
Where a sealing face has to be machined more than 1 mm below the skin, vacuum assist during casting is the process answer, cutting gas content from 15-25 cm³ per 100 g to under 5. Where a part passes dimensionally but fails a leak test, vacuum resin impregnation seals interconnected microporosity without affecting dimensions. Both are worth qualifying up front rather than negotiating after a failure. The mechanisms and the fixes are catalogued in common aluminum die casting defects.
Fixturing a casting
This is where machining a casting differs most from machining a billet, and it is where most tolerance problems on cast parts actually originate.
A billet arrives flat, square and known. A casting arrives drafted, curved, ±0.1 mm and with no reference surface at all. Clamp it in a vice and start cutting and the machine will hold its own tolerance perfectly while every part comes out different, because the datum moved.
Why cast datum features matter
The fix is to decide the datum scheme before the die is designed, not before the fixture is built. What that means in practice:
- Define a 3-2-1 reference on the part drawing. Three cast pads establish the primary plane, one cast hole or boss gives secondary location, a second gives rotational constraint.
- Put all of them in the same die half, and never across the parting line. Parting line mismatch of 0.1 to 0.15 mm is normal, and a datum scheme that straddles the line inherits that mismatch as fixture error on every part.
- Prefer the fixed die half, which does not move and holds position more consistently shot to shot.
- Raise datum pads above the surrounding surface and give them extra stock, 0.5 to 0.8 mm, so flash and draft cannot interfere and so they can be skimmed into a true reference on the first operation.
- Trim and blast before fixturing. A 0.2 mm flash line under a locator is a 0.2 mm error, and it will not be repeatable.
The first operation locates on cast datums and creates a machined reference face plus two dowel holes. Every operation after that locates on machined features, so the cast ±0.1 mm drops out of the stack entirely.
Clamping deserves its own warning. Clamp force is kept deliberately low with support directly beneath the cutting zone, because a 1.5 to 2 mm wall will deflect under a clamp and spring back once released. The face measures perfectly in the fixture and fails on the bench.
Threads in cast aluminum
Threads are cut or formed into a cored boss on the machining centre. The boss design decides whether the thread holds, and it has to be in the casting from the start.
Thread engagement in aluminum should be 1.5 to 2 times nominal diameter, so an M6 fastener wants 9 to 12 mm of engaged thread against the 6 mm you would use in steel. Boss outside diameter should be at least twice the thread diameter so the wall around the thread does not split under torque.
| Method | Size range | Relative strength | Best for |
|---|---|---|---|
| Cut tap into cored boss | M2-M20 | Baseline | General fastening, single or occasional assembly |
| Form (roll) tap | M3-M8 | +15-30% over cut thread | Thin bosses, higher torque, produces no chips |
| Self-tapping screw into cored hole | M3-M6 | Below cut thread | Cost-driven joints assembled once and never serviced |
| Threaded insert | M2-M10 | 2-3× cut thread strip torque | Repeated assembly, vibration, high torque in a thin boss |
| Cast thread | Not offered | Unreliable | Not used: draft and die complexity make it impractical |
Two casting-specific notes. Form tapping displaces material rather than cutting it, so it needs a sound boss; tapping into a porous boss produces incomplete threads whichever method you use, which is another reason to keep heavy bosses away from the last-to-freeze region. And where a joint will be opened repeatedly in service, an insert is the correct answer rather than a deeper thread, because the failure mode is thread stripping in a soft matrix and more engagement only delays it.
Sealing faces and bearing bores
These are the two features that most often justify the machining operation in the first place, and they behave differently.
Sealing faces are face milled flat within 0.02 mm per 100 mm at Ra 0.8 µm, with Ra 0.4 µm available where a dynamic seal or a thermal interface material requires it. A single-insert fly cut usually produces the best flatness on a large face, because it removes insert-to-insert height variation from the result. This is normally the first machined feature on a part, since it becomes the primary datum for everything after.
Bearing and seal bores on parts like motor and pump housings are rough bored then finish bored or reamed to H7, with cylindricity inside 0.01 mm. Where two bores in a housing have to be concentric, machine both in one setup. Concentricity then comes from the machine’s own accuracy, typically 0.008 to 0.02 mm, rather than from fixture repeatability, which on a second setup will consume 0.05 to 0.08 mm before any cutting happens.
The general principle behind both: any dimensional relationship that matters should be created in a single setup wherever the machine envelope allows it.
Tool wear: why cast Al-Si is harder on carbide than 6061
Engineers who have machined a lot of 6061 arrive with a tool life expectation that cast aluminum will not meet, and the reason is silicon.
Die casting alloys need 7.5 to 12% silicon by weight. That is what gives the melt enough fluidity to fill a 1.5 mm wall in milliseconds and what suppresses hot tearing as the casting shrinks against rigid steel. Because silicon is less dense than aluminum, that weight fraction is roughly 11 to 14% by volume, present as coarse eutectic plates and primary particles rather than in solution.
Those particles are hard. The comparison that explains everything:
| Material | Hardness |
|---|---|
| Aluminum matrix | 40-80 HV |
| Silicon particles in cast Al-Si | 1,000-1,150 HV |
| Cemented carbide cutting edge | 1,300-1,800 HV |
| PCD (polycrystalline diamond) | 6,000-8,000 HV |
Silicon at 1,000 to 1,150 HV against a carbide edge at 1,300 to 1,800 HV is in the range where abrasion proceeds steadily. Each particle the edge meets is close enough in hardness to remove a little of it, so the failure mode is not chipping but continuous edge rounding: the tool wears rather than breaks, surface finish degrades, cutting forces rise and the inspected dimension drifts. It behaves like machining with a lapping compound mixed into the workpiece.
Wrought 6061 carries 0.4 to 0.8% silicon, most of it in solid solution or as fine Mg2Si precipitates rather than coarse particles, so under 1% by volume presents as an abrasive. That single difference is why a carbide end mill that lasts a full shift in 6061 loses its edge much sooner in ADC12 at 9.6 to 12% silicon.
The response is tool material and geometry rather than reduced speed:
- Polished, uncoated carbide with high positive rake at 250 to 600 m/min for low and medium volume work. Polished flutes matter because aluminum forms a built-up edge readily, and built-up edge is the main cause of finish deterioration.
- PCD tipped tools at 600 to 1,200 m/min for production volume and for any finishing pass whose surface quality has to hold across thousands of parts. PCD costs several times more per tool and lasts 10 to 20 times longer, so it wins on cost per part well before it wins on cost per tool.
- Feed per tooth of 0.05 to 0.20 mm depending on tool diameter and rigidity.
- Through-tool coolant on deep holes, because aluminum chips weld to each other and pack in a blind hole.
- Tool life managed by scheduled part count rather than by waiting for a dimension to drift out on an inspected feature.
Alloy choice interacts with this. A380 at 7.5 to 9.5% silicon has the highest machinability rating of the common die casting alloys, ADC12 and A360 sit below it, and A413 at 11 to 13% silicon is the most abrasive of the four. On a part with heavy machining, that difference is a legitimate input to alloy selection.
What you actually get
| Attribute | As-cast | Machined |
|---|---|---|
| Linear tolerance | ±0.1 mm | ±0.02 mm |
| Flatness | 0.1 mm per 100 mm | 0.02 mm per 100 mm |
| Bore fit | Not capable | H7, cylindricity within 0.01 mm |
| Hole true position | ±0.15 mm | ±0.05 mm from machined datums |
| Surface roughness | Ra 1.6-3.2 µm | Ra 0.8 µm, Ra 0.4 µm on sealing faces |
| Threads | Not cast | M2-M20, 6H class |
A cast part is not disqualified by a tight tolerance. It is disqualified by many tight tolerances on faces that cannot be reached in one or two fixtures, because each extra setup pushes the cast route toward the machined price. One bearing bore and one sealing face is normal practice. Fourteen features at ±0.03 mm across five faces is a machined part in a casting’s clothing, and the honest recommendation there is to machine it from billet.
Why one roof matters for the tolerance stack
When the caster and the machine shop are separate companies, an out-of-tolerance machined feature has no owner. The caster demonstrates that the casting is inside ±0.1 mm. The machine shop demonstrates that the allowance ran out on one side. Both are correct, the part is still wrong, and the engineering time spent establishing that is worse than the scrap.
Casting and machining in one plant collapses that. The fixture is designed alongside the die, so the datum pads exist because the fixture needs them rather than because someone remembered. A steel-safe change to move a locating pad 0.15 mm is a day’s work rather than a commercial negotiation. The first article report covers cast and machined features together against one drawing. And there is no inter-factory shipment, which removes a handling damage mode that castings are particularly exposed to before their edges are broken.
That is the argument for the combined route, and it is the reason our CNC machining after casting capability exists only to finish parts we cast.
Where to send a part
Send the 3D model with a 2D drawing marking which features are critical, and the DFM report will come back with a proposed 3-2-1 datum scheme, the allowance we would add per feature, and a written note on any machined face that risks intersecting a last-to-freeze region. Where the answer is that the part has too many precision features to cast economically, that is what the report will say, and the aluminum die casting versus CNC machining comparison covers where that line sits.
For parts machined from solid billet in 6061, 7075, 5052 or MIC-6, including prototypes and volumes below roughly 500 pieces a year, go to charmaxprecision.com. Same company, different process, and no advantage in steering a part into the wrong one.
