ODM Die Casting Fabrication Process: A Step-by-Step Guide

• 1
  Key takeaways
• 2
  What ODM die casting covers before the mold is cut
• 3
  Tool design and shrinkage allowance
• 4
  Casting defects and what the parameters tell you
• 5
  Post-casting machining and finishing
• 6
  Inspection and first-article approval
• 7
  Step-by-step die casting fabrication process
• 8
  As-cast versus machined: where to put each tolerance

In an ODM program, the supplier takes on design work as well as production. That means the die casting fabrication process starts long before molten metal enters a shot sleeve. It starts with your 3D model, your functional requirements and a DFM review that decides whether the part should be cast at all.

During that review we look at four things first: nominal wall thickness, draft angle, corner radii and where the parting line can sit. A wall under 0.8 mm for aluminum ADC12 fills poorly at the far end of the cavity. A wall over 6 mm creates shrinkage porosity in the middle. Both problems show up as scrap, not as a drawing error.

We also ask what the part actually does. A housing that only holds a PCB can live with ±0.25 mm and a bead-blasted finish. A gearbox cover with a bearing bore needs a machined seat held to ±0.005 mm, and that seat changes the tool design, the datum scheme and the fixture plan.

The output of this stage is a short DFM report: recommended alloy, draft angles per face, gate and overflow positions, expected shrinkage allowance, and the list of surfaces that will be machined after casting. That report is the document the rest of the program is built on.

• 1
  Give us the functionLoad path, sealing faces and mating surfaces matter more than the model's nominal dimensions.
• 2
  Flag tight tolerances earlyEvery tolerance under ±0.1 mm becomes a machining operation and a cost line.
• 3
  Send the alloy if it is fixedADC12, A380 and AZ91D behave differently in fill and shrinkage.

The die is cut oversize to compensate for shrinkage as the part cools. For aluminum ADC12 the linear shrinkage allowance usually lands between 0.4% and 0.6%, applied per axis rather than as one global scale factor. Long, thin features shrink differently from a thick boss, so a single scale number will pull the part out of tolerance at one end.

Draft is the second decision. Standard practice is 1–2° on as-cast walls and 3° or more on deep ribs and textured surfaces. Not enough draft means the part drags on ejection, scuffs the surface and eventually cracks the die. Too much draft eats into the machining allowance on a face that still has to be milled flat.

Gate and runner position controls fill. A gate placed at the thickest section lets the metal feed the thin walls while it is still liquid. A gate on a thin wall freezes early and leaves a cold shut further down the cavity. For parts with a deep pocket, we add overflows at the last-to-fill points so gas and oxide have somewhere to go.

Tool steel selection follows volume. A 5,000-shot prototype tool and a 200,000-shot production tool are not the same purchase. If you expect a design change after the first run, ask for insert-style construction so only the affected block is recut.

Porosity is the defect most programs fight. It comes from three places: gas trapped during fill, shrinkage as thick sections cool last, and turbulence that folds oxide into the melt. You can often tell which one you have by where the void sits. Gas porosity clusters near the gate or at last-to-fill points. Shrinkage porosity sits in the thermal center of a thick boss.

Cold shuts look like a seam or a line on the surface where two metal fronts met but did not fuse. They usually mean the fill time was too long or the die was too cold at that location. Raising die temperature by 20–30 °C or moving the gate often clears it without touching the tool.

Flash at the parting line is a clamping or die-fit issue, not a metal issue. A little flash is normal. Flash that grows over a production run means the die is losing its shut-off, and that is a maintenance signal rather than a process tweak.

Warpage shows up after ejection, not during fill. It follows uneven wall thickness and uneven cooling. If a flat part bows more than 0.3 mm across 200 mm, expect to add a straightening operation or redesign the rib layout.

Castings arrive at the machine with a skin that is harder and less uniform than the core. That skin can deflect a light finishing pass, so the first cut has to get under it. We normally take 0.3–0.8 mm off a machined face in two passes rather than one heavy cut.

Datum choice decides whether the second operation matches the first. On most housings we pick a machined face plus two dowel holes as the primary datum, then hold the casting in a fixture that locates on those same features. Clamping on an as-cast surface introduces variation that no amount of machine accuracy can remove.

Finishing comes last because most coatings change dimensions slightly. Anodizing builds a few micrometers and hardcoat builds more. Mask bearing bores, threads and grounding pads before the parts leave for the finish line.

For parts that need both a cast texture and a tight fit, the practical route is to cast the texture, mask it, and machine only the fit. Trying to reproduce a cast surface by machining costs more and never looks the same.

• 1
  Light cuts firstTake the skin off in two passes instead of one deep cut.
• 2
  Locate on machined featuresFixture on the datum you machined, not on the raw casting.
• 3
  Mask before coatingBores, threads and contact pads should not see anodize or powder.

A first article is not a formality. It is where you confirm that the tool, the process window and the drawing all agree. We measure the full drawing on a CMM, including the features that are not critical, because a drift in a non-critical feature often explains a problem in a critical one.

For production lots, the inspection plan should match the risk. Cosmetic parts get a visual and finish check. Structural or sealing parts get dimensional checks on the features that matter, plus a porosity check if the application is pressure-tight.

Keep the first-article report on file with the process parameters that produced it. When a part drifts six months later, that record is what tells you whether the die moved or the machine did.

If your program has a regulatory file, plan the documentation early. Medical and automotive programs need traceability from melt lot to finished part, and that is much easier to build in than to reconstruct.