CNC machining after casting is the secondary operation that brings selected features of a die cast aluminum part from the as-cast tolerance of ±0.1 mm to ±0.02 mm. CharMax Precision machines sealing faces, bearing bores, threaded holes and datum surfaces on 3, 4 and 5-axis machining centres in the same facility that casts the part.
CNC machining after casting is the secondary operation that brings selected features of a die cast aluminum part from the as-cast tolerance of ±0.1 mm to ±0.02 mm. CharMax Precision machines sealing faces, bearing bores, threaded holes and datum surfaces on 3, 4 and 5-axis machining centres in the same facility that casts the part.
Castings need machining because die casting is a near-net-shape process, not a net-shape one. Every external wall carries 1 to 2° of draft, cast holes are tapered and deliberately undersized, and as-cast flatness of 0.1 mm per 100 mm is nowhere near what a gasket face or a bearing seat requires. The casting supplies the shape and the machining supplies the interfaces.
This service covers machining of castings only. Machining aluminum parts from solid billet in 6061, 7075, 5052 or MIC-6 is the work of our sister CNC operation at charmaxprecision.com, which exists for exactly that. Keeping the two scopes separate means a casting program gets a foundry engineer who understands where porosity lives, and a billet program gets a machinist who is not compromising around a cast datum.
| Scope | Machining of die cast aluminum parts produced in-house |
|---|---|
| Machine types | 3-axis VMC, 4-axis with rotary, 5-axis machining centres |
| Machined tolerance | ±0.02 mm on critical features |
| Bore tolerance | H7 fit achievable on bearing and seal seats |
| Flatness after machining | 0.02 mm per 100 mm |
| Surface roughness | Ra 0.8 µm standard, Ra 0.4 µm on sealing faces |
| Thread range | M2 to M20, cut or form tapped, 6H class |
| Hole position | ±0.05 mm true position from machined datums |
| Machining allowance | 0.5 to 1.0 mm on cast faces |
| Fixturing | Dedicated fixture per part, located on cast datums |
| Cutting tools | PCD and polished carbide for high-silicon aluminum |
| Verification | CMM first article, in-process sampling, printed reports |
The question is not whether a casting needs machining but which features do. Machining every surface throws away the economics of casting; machining none leaves you with a part that cannot seal, locate or accept a bearing. The right answer is usually 10 to 25% of the total surface area.
Five characteristics of a die casting are what create the need. Each of them is inherent to the process rather than a defect, and each is best resolved by identifying it on the drawing before tooling is designed.
Face milled flat within 0.02 mm per 100 mm at Ra 0.8 µm or better, with Ra 0.4 µm available where a static gasket or thermal interface material demands it. Usually the first operation, because it establishes the primary datum for everything after it.
Rough bored, then finish bored or reamed to H7 with cylindricity inside 0.01 mm. Concentricity between two bores in a housing is held by machining both in one setup rather than by relying on cast position.
M2 to M20 in 6H class, cut or form tapped from cored pilot holes. Thread depth, chamfer and gauge acceptance are set on the drawing, and thread gauges are used at first article and at sampling frequency in production.
Drilled and reamed to H7 for assembly location, held to ±0.05 mm true position from the machined datum frame. These are the features that determine whether your downstream assembly goes together without selective fitting.
Machined where the groove must control squeeze accurately, typically 15 to 30% compression on the cord. A cast groove is acceptable for a soft foam gasket but not for an O-ring on an IP67 enclosure.
Milled and bored openings that must accept a bought-in connector, gland or bulkhead fitting to its published tolerance, including the flat seating face and the threaded or clearance mounting holes around it.
Small machined pads on otherwise as-cast surfaces that give the assembly a repeatable three-point reference without machining a whole face. An economical way to control a stack-up.
Edge break of 0.2 to 0.5 mm on machined edges, lead-in chamfers on tapped and reamed holes, and removal of the burr raised where a cutter exits a cored hole. Specified rather than assumed, because it affects assembly and handling safety.
Fixturing is where machining a casting differs most from machining a billet. A billet arrives with flat, square, known reference faces. A casting arrives with drafted, curved, ±0.1 mm surfaces and no reference at all. If you clamp it in a vice and start cutting, the machine holds its own tolerance perfectly and every part still comes out different, because the datum moved.
The fix is to decide the datum scheme before the die is designed. We ask for a 3-2-1 reference defined on the part drawing: three cast pads that establish the primary plane, one cast hole or boss for the secondary location, and a second for rotational constraint. Those features are then placed in the fixed die half where position is most repeatable, and given a slightly heavier machining allowance so they can be cleaned up first if needed.
Every casting gets a dedicated fixture built to that scheme. First operation locates on the cast datums and machines the reference face and two dowel holes; every operation after that locates on machined features, so the tolerance stack collapses to what the machine can hold. Clamping force is kept deliberately low with support directly beneath the cutting zone, because a 1.5 mm wall will deflect under a clamp and spring back flat once it is released, leaving a face that measured perfectly in the fixture and fails on the bench.
Machining allowance is the stock deliberately left on a cast surface so it can be cut to final dimension. Getting it right is a genuine optimisation rather than a safety margin: 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 dense chill layer into the more porous subsurface material.
The as-cast skin of a high pressure die casting is its best material. Rapid solidification against the cold die produces a fine-grained, near fully dense layer roughly 0.3 to 0.5 mm thick. Below that the grain coarsens and gas and shrinkage porosity increase. That is why 0.5 to 1.0 mm is the standard allowance: enough to guarantee clean-up given cast tolerance, not so much that you are cutting deep into the part's weakest material.
| Feature | Allowance | Reason |
|---|---|---|
| Flat sealing or mating face, up to 100 mm | 0.5-0.8 mm | Covers cast flatness of 0.1 mm per 100 mm plus cast position tolerance |
| Flat face over 150 mm | 0.8-1.2 mm | Cast flatness accumulates with length, so larger faces need more stock to clean up |
| Bore to be finish machined | 1.0-1.5 mm on diameter | Removes cast 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 skim machined into a true reference first |
| Feature that must stay pressure tight | 0.3-0.5 mm | Deliberately minimal to keep the cut inside the dense chill layer |
Allowance is specified on the casting drawing per feature, not applied globally. Faces that stay as-cast should be marked as such so no stock is added where it is not needed.
Machining a die casting exposes what is underneath the skin. High pressure die casting always entrains some gas, and it concentrates in the last regions to solidify, usually the thickest sections and the areas furthest from the gate. When a cutter removes the dense chill layer over one of those regions, the porosity appears as small pits on the machined face. On a bracket that is cosmetic; on a hydraulic sealing face it is a leak path.
The important point is that this is managed at die design stage, not at the machine. Once the gate is cut, the location of the last-to-freeze region is fixed, so it has to be moved away from your machined faces before steel is ordered. This is precisely why the simulation and the machining plan are reviewed together rather than in sequence.
Threads in die cast aluminum are cut or formed into a cored boss on the machining centre. Threads are never cast directly: a cast thread would carry draft, be dimensionally unreliable and require an unwinding mechanism in the die.
Boss design decides whether the thread holds. In aluminum, thread engagement should be 1.5 to 2 times the nominal diameter, so an M6 fastener wants 9 to 12 mm of engaged thread, and boss outer diameter should be at least twice the thread diameter so the wall around the thread does not split. Both dimensions have to be in the casting from the start, which is another reason fastening should be decided before tooling.
Where a joint will be assembled and disassembled repeatedly, or where the required torque is close to what an aluminum thread will strip, a threaded insert is the better answer. Insert selection and installation are handled as part of assembly work rather than on the machining centre.
| 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 and higher torque, produces no chips to trap in the part |
| Drilled and reamed dowel hole | 3-12 mm, H7 | Not a thread | Assembly location where position matters more than clamping |
| 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, or high torque in a thin boss |
| Cast thread | Not offered | Unreliable | Not used, because draft and die complexity make it impractical |
Thread class is 6H unless the drawing states otherwise. Threads are checked with go and no-go gauges at first article and at the agreed sampling frequency in production.
Die cast aluminum machines differently from wrought aluminum, and the reason is silicon. A380 carries 7.5 to 9.5% silicon and ADC12 carries 9.6 to 12%, present as hard primary silicon particles distributed through a soft matrix. The effect on cutting tools is abrasive rather than mechanical: tools do not chip, they wear, and a carbide end mill that would last a full shift in 6061 loses its edge much faster in ADC12.
The response is tool material and geometry rather than reduced speed. Polished, uncoated carbide with high positive rake handles moderate volumes and resists the built-up edge that aluminum forms readily. For sustained production and for finishing operations where surface quality has to hold across thousands of parts, PCD tipped tools are the economical answer despite costing several times more per tool, because they last 10 to 20 times longer between changes.
This capability exists to finish castings we produce. Casting and machining under one roof means a single company owns the whole tolerance stack, from the cast datum pad through the fixture to the finished bore, and there is no argument about whose tolerance consumed the budget when something is out of specification. It also removes an inter-factory shipment and the handling damage that comes with it.
If you need aluminum parts machined from solid billet, that is a different process with a different alloy set and it belongs to our sister operation, CharMax Precision CNC machining at charmaxprecision.com. They work in 6061, 7075, 5052 and MIC-6 plate, and they are the right choice for prototypes, low volumes below roughly 500 pieces per year, and parts whose geometry does not suit casting at all.
The two operations are the same company, so the transition is straightforward in both directions. A common pattern is to machine the first few hundred units from billet while a design is being validated, then move to casting once annual volume justifies tooling, with the same engineering team carrying the drawing across.
The equipment, controls and finished-part evidence used to deliver this operation in production.
Real parts we have manufactured that involved this capability.
A European industrial pump manufacturer converted a billet-machined housing to A360 die casting to reach 8,000 units a year, holding 6 bar pressure tightness, an H7 bearing bore and a 0.05 mm sealing face.
A collaborative robot manufacturer moved a joint housing from machined prototypes to ADC12 die casting at 12,000 units a year, cutting 180 g per joint while holding ±0.02 mm concentricity between the harmonic drive seat and the encoder bore.
An LED lighting brand replaced a bonded two-piece design, an extruded heat sink adhered to a die cast housing, with a single A413 casting, removing the thermal interface and taking 11 °C off the LED junction temperature at 60,000 units a year.
Die casting pays for itself above roughly 1,000 parts per year. Below that, or while you are still validating a design, CNC machining from billet is usually the faster and cheaper route. CharMax Precision runs a dedicated aluminum CNC machining operation for exactly that work, so you can prototype machined, then move to casting when volume justifies tooling.
Die casting is a near-net-shape process, so features requiring better than about ±0.05 mm, a controlled flatness, or a fine surface finish have to be machined afterwards. Every as-cast wall carries 1 to 2° of draft, cast holes are tapered and undersized on purpose, and as-cast flatness is 0.1 mm per 100 mm. Typically 10 to 25% of a casting's surface area is machined, covering sealing faces, bearing bores, threaded holes and datum features.
±0.02 mm on machined features, with H7 fits on bores, 0.02 mm per 100 mm flatness and Ra 0.8 µm surface finish as standard. Reaching that consistently depends on the fixture and the datum scheme rather than the machine: the first operation locates on cast datum pads and creates a machined reference, and every operation after that locates on machined features so the cast ±0.1 mm never enters the stack.
Porosity shows up as small pits on the machined face, which is cosmetic on a bracket and a leak path on a sealing surface. It is prevented at die design stage by positioning gates and overflows so the last-to-freeze regions do not sit under machined faces, and by keeping the cut inside the 0.3 to 0.5 mm dense chill layer on pressure-tight surfaces. Where a part passes dimensionally but fails a leak test, vacuum resin impregnation seals interconnected microporosity without changing dimensions.
0.5 to 1.0 mm on flat faces is the standard allowance, rising to 0.8 to 1.2 mm on faces longer than 150 mm and 1.0 to 1.5 mm on diameter for bores. On surfaces that must stay pressure tight, use 0.3 to 0.5 mm deliberately, so the cut stays inside the dense chill layer. Specify allowance per feature on the casting drawing rather than globally, and mark which faces stay as-cast so no stock is added where it is not needed.
Not on this site. Machining here is a secondary operation on castings we produce, so a single company owns the tolerance stack from cast datum to finished bore. Aluminum CNC machining from billet in 6061, 7075, 5052 and MIC-6 is handled by our sister operation, CharMax Precision CNC machining at charmaxprecision.com. It is the same company, so moving a program from machined prototypes to cast production, or the reverse, is straightforward.
Yes, and it is the standard approach for M2 to M20 threads. Thread engagement should be 1.5 to 2 times the nominal diameter and boss outer diameter at least twice the thread diameter, both of which must be designed into the casting. Form tapping gives 15 to 30% more strength than cut tapping and produces no chips. For joints that are assembled repeatedly or carry high torque, a threaded insert delivering 2 to 3 times the strip torque is the better answer.
Porosity is controlled at three stages: melt preparation with degassing and filtration, die design with engineered overflows, vents and gate geometry validated by flow simulation, and process control with logged shot profiles and die temperatures. Where parts must be pressure tight or heavily machined in critical areas, we design vacuum assist or use A360 alloy, and verify with leak testing or X-ray inspection.
A 3D model in STEP, IGES, X_T, SLDPRT or native CAD format, plus a 2D drawing showing critical dimensions, tolerances, surface finish, alloy and any inspection requirements. If you only have a 3D model we can still quote, but a drawing that marks which features are critical to function will get you a more accurate price and prevent misunderstandings later.
Send a 3D model and a drawing marking which features are critical. You will get casting and machining quoted together, a proposed datum scheme, and a written note on any machined face that risks intersecting porosity.