How much die casting machining allowance should you leave on a machined face?

What does the machining allowance on a die casting have to cover?

It has to cover every way the cast surface can end up away from its nominal position, plus the minimum depth a cutter needs to leave a clean, fully machined surface. If any one of those is left out, some castings in the lot will show a black, unmachined patch on a face that should be bright.

Think of the allowance as a budget with separate lines. Each line is a reason the real surface may sit higher or lower than the model says:

• The as-cast tolerance of that surface. A die casting is not exactly its nominal size, and the stock must cover the case where the surface is cast at the low side of its tolerance.
• Features that cross the parting line or a moving core. NADCA notes that flash at the parting line changes dimensions measured across it, and recommends keeping critical dimensions in one die half (NADCA, parting line). A machined face located from a datum in the other die half needs extra stock for that shift.
• Draft. Walls parallel to the die opening are tapered, so a face that must be machined square over its full depth has more metal at one end than the other.
• Distortion. Flatness and straightness errors from cooling and ejection, which grow with the size of the face.
• Location error in the fixture. The casting is clamped against cast surfaces, and any error in those surfaces moves the whole machined pattern.
• Clean-up. The small depth below which a cutter rubs instead of cutting, or leaves the cast texture visible in low spots.

The cutter does not care which of these lines produced the extra metal. The designer does, because the lines that dominate tell you where to spend effort: tighter casting control, a better datum scheme, or more stock.

How do you work out the allowance for one machined face?

Add the clean-up depth to the worst-case low position of the cast surface, measured from the datums the machining fixture will actually use. Do it face by face, because a small face close to the datums needs far less stock than a large face across the parting line.

A simple worksheet for each machined face:

1. Pick the machining datums first. Name the cast surfaces the fixture will locate on. The allowance is only meaningful relative to those surfaces.
2. Take the as-cast tolerance of the face relative to those datums. For an equal-bilateral tolerance, half of the band is the amount the surface can sit low.
3. Add the draft effect if the face runs along the die opening. The extra metal at the thick end is the depth of the wall multiplied by the tangent of the draft angle. With tan 1° close to 0.0175, each degree of draft adds a little under two hundredths of the wall depth.
4. Add a flatness allowance for large faces and a parting-line allowance if the face and its datums are in different die halves.
5. Add the clean-up depth your machining process needs to produce the specified surface texture.
6. Check the total against the skin. If the result is well beyond the skin depth reported by NADCA, look for a way to reduce the variation instead of accepting a deep cut on a critical face.

Straight addition is the conservative method and suits low volumes and first articles. On a stable production process some teams combine the variation terms statistically, but that needs real measured data from the die, not assumptions. Whichever method you use, write the resulting cast dimension on the casting drawing so the die caster and the machinist are working to the same number.

The same thinking applies to cored holes. A hole cored close to size keeps its skin, and a light reaming or boring pass only corrects the draft taper. NADCA notes that holes need more draft than any other die-cast feature because the casting shrinks onto the core pin (NADCA, holes and windows), so the stock on the wall of a cored hole is set largely by that taper.

How should the drawing show machining stock and datums?

Show the casting and the machined part as two defined conditions, and choose cast datums that stay on the part or are machined first in a known sequence. A single drawing that shows only the finished part leaves the die caster to guess how much metal to add.

There are two common layouts. One is a separate casting drawing, with the stock already added to every machined face, plus a machining drawing of the finished part. The other is a single combined drawing that shows the finished geometry and marks the cast outline and allowance on each machined face, which is what the symbols in ISO 10135 are for (ISO 10135:2007 scope). Either works; what fails is a finished-part drawing with no statement of the cast condition.

Datums deserve the most care. The first machining operation has to locate on cast surfaces, so pick surfaces that are flat, well away from the parting line and gates, and in the same die half as the faces they locate. Small cast locating pads, bosses or datum targets make fixturing repeatable and can be kept out of cosmetic areas. ISO 8062-4 states that it does not apply when cast datum surfaces are machined (ISO 8062-4:2023 scope), which is a useful reminder that once a datum is cut, the tolerance scheme has to say what the new datum is.

Finally, mark every machined surface with the texture symbol that requires material removal, per ISO 21920-1 or ASME Y14.36 as your drawing system uses, and leave the rest as cast. That makes the allowance visible, and it stops a supplier from machining faces that were meant to keep their skin.

What should you agree with an offshore supplier about machining stock?

Agree the casting drawing, the machining datums and the first-article checks before the die is built, because the die fixes the stock for its whole life. Changing an allowance later means changing die steel.

When parts come from Vietnam or anywhere far from your plant, three things prevent most disputes. First, confirm who owns the casting drawing and who approves it, especially if casting and machining happen at different companies. Second, ask for a first-article report that measures the remaining stock on each machined face across several cavities or shots, not only the finished dimensions. Third, section a first-article part through the critical faces so you can see whether the cut stayed in dense metal.

Having one supplier answer for both casting and machining shortens that loop, because a face that will not clean up can be traced to a die, a cavity and a shot while the cause is still fresh. Saola sources die castings in ADC12 aluminum and Zamak 3 zinc from partner foundries it manages and machines them on the CNC milling and CNC turning equipment at its lead CNC plant; the quote names the production site and origin. ISO 9001 certification is in progress, not yet held. The RFQ preparation guide lists what else to include, and you can send the drawing for a quote with the machined faces marked.