Die Casting Design Rules: Draft, Walls, Ribs, and Defects

Die casting design rules exist because a die-cast part forms under pressure inside two blocks of steel, shrinks as it solidifies, and then has to push clear of the very features that shaped it. The die casting hub carries the process story: hot and cold chamber machines, the alloy families, tooling life, and where the process sits against the alternatives. This page is the CAD-side rulebook. It carries the numbers a designer works with at the screen: draft by alloy, feature, and depth; wall thickness bands by casting size; rib, boss, and fillet ratios; parting-line strategy; and the tolerance logic that decides which features stay as cast, with the full as-cast bands and parting-line allowances carried on the tolerances page.

Every rule below serves one of three physical events. The die has to fill, the part has to solidify evenly, and the part has to eject. A fourth decision cuts across all three: what happens after casting, meaning which surfaces stay as cast and which are machined. Plastic parts obey a close cousin of this ruleset, covered in the injection molding design rules page, but the numbers are not interchangeable between processes. For the broader review discipline, start with design for manufacturing, and for the metal-versus-plastic selection decision, see die casting vs injection molding.

Every rule serves one of three events

Fill comes first. Molten alloy has to reach every corner of the cavity before it loses too much heat, so a section that is too thin for the alloy and the flow length produces a misrun, an unfilled corner, or a cold shut, the seam left when two flow fronts meet without fusing. Wall minimums, gradual section changes, generous radii, and ribs used as flow paths all serve this event.

Solidification comes second. A die casting shrinks as it freezes, and it shrinks unevenly wherever mass concentrates. Thick junctions at rib and boss bases hold a molten core after the surrounding skin has stiffened, and that core pulls the surface into a sink mark or closes into shrinkage porosity. Rigid, sharp corners restrain the shrinking metal and can tear it, which is the hot tear, and asymmetric sections cool unevenly and warp. Uniformity rules, rib and boss ratios, coring, and fillets all serve this event.

Ejection comes third. The casting grips the die steel that forms its inside surfaces and has to be pushed off without dragging, galling, or springing. Draft angles, parting-line placement, and ejector-pin planning serve this event, and flash lives here too, because injection pressure tries to force the die halves apart at the parting line. How these defects are found and measured once parts are running is covered under quality inspection and metrology.

Held in one view: misruns and cold shuts trace to fill, shrinkage porosity, sink, hot tears, and warpage to solidification, and drag, flash, and ejection distortion to release. Each section below opens by naming the defect it prevents, because that is the clearest way to judge whether an exception is safe.

Walls: prevent misruns, cold shuts, and shrinkage porosity

Published guidance is blunt that there are no hard and fast rules for absolute wall thickness. Walls should be as consistent as the part allows, and where variation is required the transition should be gradual rather than a step. That uniformity principle prevents more defects than any single number. A section that is too thin freezes before the die fills and leaves a misrun or a cold shut. A section that is too thick solidifies last and shrinks into porosity or sink. Aim wall stock within about 10 percent of the typical wall around cored holes and metal savers, and core out thick zones rather than letting them solidify solid.

The numbers still matter, because each alloy fills and freezes differently and casting size changes what is achievable. Capability floors are what published die-casting references list as achievable minimums, practical minimums are what a design should target on typical parts, design bands are the comfortable working range, and large castings need more than small ones.

Three patterns are worth carrying into the model. Zinc casts the thinnest walls of the common alloys, reaching roughly 0.4 to 0.6mm on small parts, which is why detailed, miniature housings and bezels so often end up in Zamak. Aluminum needs about 0.9 to 1.0mm at the floor and is usually drawn between 1.5 and 4mm, with much aluminum work landing at 2 to 4mm. Casting size moves the minimum: a large aluminum casting calls for about 2.0mm where a small one can approach 1.0mm, and a large magnesium casting about 2.5mm. Uniformity beats thinness every time, because a consistent 2.5mm wall outperforms a part that alternates between 1.0 and 4mm.

Wall thickness also sets the economics of the cycle. Thinner uniform walls carry less metal and freeze faster, which raises shots per hour and lowers material cost, so the commercial incentive runs the same direction as the defect prevention. Where a design genuinely needs local mass, such as a bearing seat, core the back side out and keep the functional wall uniform rather than thickening the whole section.

Draft: prevent drag, galling, and stuck parts

Draft is taper built into every face parallel to the die opening so the casting releases instead of dragging. The reason inside faces need more of it is shrink direction: as the casting solidifies it shrinks onto the die steel that forms its inside surfaces, usually in the ejector half, and away from the steel that forms outside surfaces. NADCA guidance recommends about twice as much draft on inside walls as on outside walls, and untapped cored holes grip hardest of all, since the casting shrinks around the steel pin that forms them. Holes and windows need more draft than any other die-cast feature.

The part most designers get wrong is the relationship between draft and depth. The NADCA Product Specification Standards method does not assign one angle per alloy. It works from feature depth, and the angle comes out smaller as the feature gets deeper, because the taper distance grows with the square root of depth while the depth itself grows linearly. In the standards’ own worked example for an aluminum inside wall at the Standard tolerance class, the required draft is about 6 degrees at 2.5mm of depth, about 1.9 degrees at 25mm, and about 0.85 degrees at 127mm. The Precision class runs shallower still, about 3.6 degrees at 2.5mm and about 1.1 degrees at 25mm on the same feature. Short features are the steep ones, which is the opposite of the add-draft-with-depth rule of thumb that circulates in some vendor guides.

The draft-angle guidance tabulated on this page carries those values across zinc, aluminum, and magnesium at three depths for outside walls, inside walls, and cored holes. The aluminum inside-wall column is the standard’s published worked example itself; the other cells are calculated from the standard’s published constants by the same formula, so treat them as method values to confirm with your die caster rather than shop-floor settings. For engineers who want one number per surface, the standards offer their own general-note guidance: an aluminum casting with most features at least 25mm deep can be covered by a general note of 2 degrees minimum draft on inside surfaces and 1 degree minimum on outside surfaces, with exceptions called out per feature. Commonly cited vendor bands run in the same territory, about 1 to 2 degrees per side on aluminum outside walls and 2 to 3 degrees on aluminum inside walls, roughly half those values in zinc, with magnesium tracking aluminum.

Two floors and one adder complete the rule. The published precision floor is 0.75 degrees per side on inside walls and about half that, 0.375 degrees, outside; below it the casting drags and galls the steel, and the tool pays for it in repair and lost availability. Textured or etched surfaces take extra draft on top of the base value, with a commonly quoted rule of about 1 degree per 0.025mm of texture depth, so a coarse finish near 0.10mm deep can add roughly 4 degrees. Cast lettering and logos sit outside the depth method and are examined individually; published guidance puts recessed or raised text at 0.3mm minimum depth with at least 10 degrees of draft so it both fills and releases.

For example, take an A380 electronics housing with a cored inner cavity 25mm deep and outside walls of similar height. At the Standard class the method gives roughly 1.9 degrees per side on the cavity walls and about half that, near 0.95 degrees, on the outside. Shorten that inside feature to a 2.5mm deep pocket and its required angle climbs to about 6 degrees, which is why one flat draft callout across a whole drawing is a defect waiting to happen.

From the model to the foundry quote

What leaves the desk for a die-casting review is a solid model exported as STEP, with units stated explicitly in millimeters on both the model and the drawing, because a unit mismatch rescales every wall, rib, and draft value above at once. CAD file formats covers the exchange formats die casters actually open and how to package native files alongside the neutral export, so this page does not restate that list. The 2D drawing carries the intent the model cannot state on its own: the draft callout per surface, the as-cast versus machined-stock split, and the alloy and tolerance-tier choice per feature, which is exactly the set of decisions the sections above walk through. Send the drawing with the model rather than after it, since the foundry quotes the casting and any machining against both together.

Ribs and bosses: prevent sink marks and junction porosity

Ribs buy stiffness without buying wall thickness, and they double as flow paths that help the die fill. The price of a rib is mass at its base, so keep the rib section below the wall it rises from. The working rule sizes ribs at about 60 percent of the nominal wall, inside a published band of 40 to 60 percent, because a thicker rib creates a thermal mass that solidifies after the surrounding wall, shrinks, and pulls the show surface into a sink mark. A 3.0mm wall therefore takes ribs up to about 1.8mm, and thinner is safer on cosmetic faces.

The rest of rib geometry follows the same mechanics. Keep ribs no taller than about three wall thicknesses, space parallel ribs three to five wall thicknesses apart, fillet the base at 0.3 to 0.5mm minimum, and give them 1 to 3 degrees of draft per side. Published NADCA guidance adds two cautions with real content: use ribs in odd numbers where several run together, so the stresses from adjacent ribs do not stack, and do not rib a part that does not need it, because unnecessary ribs add die complexity and cost without adding function. Where a panel needs stiffening, a pattern of thinner ribs beats one heavy rib on every count: less mass, less sink under the base, and shorter flow paths for the metal.

Bosses are the problem child of this section, because a solid boss is the thickest junction on most parts and a near-certain porosity site. Core a center hole through every boss so its wall stays near the nominal wall, surround it with generous fillets, and feed it with ribs so molten metal flows into the area instead of stagnating. Both the inner and outer boss surfaces need draft like any other inside and outside feature.

The wall around a cored hole follows a published ratio. For holes under 6.4mm diameter, keep at least half the hole diameter of wall stock around them; for larger holes, revert to the nominal wall. Radius the junction generously: published guidance calls for at least a 1.5mm radius around metal savers and clearance holes and at least 0.8mm at functional or locating holes, using as large a radius as uniform wall thickness allows.

For example, a gear case drawn at a 3.0mm nominal wall takes stiffening ribs up to 1.8mm thick, spaced 9 to 15mm apart, and no taller than about 9mm. Its 5mm cored fixing holes need at least 2.5mm of surrounding wall stock, while a 10mm hole drops back to the nominal wall. Checking those three numbers at the CAD stage is what keeps sink off the sealing face and porosity out of the pressure-tight zones.

Fillets: prevent hot tears and let the die fill

The published rule leaves exactly one sharp edge on a die casting: the perimeter at the parting line. Every other corner, including the smallest corner features, gets a fillet. Two failure modes make this non-negotiable. Mechanically, a sharp inside corner is a rigid point that restrains the casting as it shrinks, and restrained metal tears, which is the hot tear. In the fill, a sharp corner forces the metal flow to turn hard, losing heat and encouraging the cold shuts and misruns covered in the wall section. A practical published minimum is 0.5mm at all corners, and larger is better wherever uniform wall thickness permits, because generous radii promote efficient metal flow.

Magnesium raises the stakes. It solidifies rapidly and is more sensitive to sharp corners than aluminum or zinc, so on magnesium parts the fillet pass deserves extra attention during design review. Corner radii also interact with the junction ratios above: the 1.5mm and 0.8mm values at cored features are floors, and as large a radius as uniform wall thickness allows is the published preference.

Holes, windows, and threads

Cored holes are formed by steel pins standing in moving metal, and their limits reflect that. Published minimums run about 2.0mm diameter in aluminum, 1.3mm in zinc, and 6.4mm in brass, and depth scales with diameter: a 6.4mm hole cores reliably to about 25mm deep, a 12.7mm hole to 50mm, and a 25.4mm hole to about 150mm. Below those diameters, do not fight the die. Drilling or piercing small holes after casting is usually the lower-cost route, and it protects slender pins that would otherwise bend or break. Through holes and windows can also obstruct metal flow, so where they sit across a flow path, published practice bridges them with cross feeders and overflows.

Threads can be cast within limits. Classic industry guidance caps cast external threads at about 32 threads per inch in zinc and 24 in aluminum and magnesium, and recommends cast threads over cut threads where the change yields a net savings. Commercial trimming leaves the trim edge on through holes within about 0.4mm, which belongs on the drawing wherever a trimmed edge mates with something. For how cast threads sit against cut and rolled alternatives, see thread standards.

Parting line, ejection, and undercuts

The parting line is where the two die halves meet, and it is the most consequential decision on this page because it sets flash location, dimensional behavior, die life, and half the tolerance story at once. Place most of the part geometry in the ejector half so the casting does not stick in the cover half, and put cosmetic surfaces on the cover side. Injection pressure tries to force the halves apart, so flash forms at the parting line and is removed in a trim die; a straight, simple parting line makes that trim easy.

Dimensions behave differently across that line. Features carried entirely by one die half are cut into a single block of steel, while a dimension that crosses the parting line or passes over a moving slide also inherits die closure, parting-line shift, and slide motion as error sources. Keep critical relationships on one side of the line. Parting-line placement also affects die life: metal injected straight onto a die surface erodes it faster, so a placement that keeps impingement off flat steel improves both die life and casting quality.

Ejection is a design input, not an afterthought. Where and how much the casting shrinks onto the die largely determines where ejector pins must land, so pin locations belong in the model and the resulting marks must be acceptable on those faces, with published references putting the marks on the order of 0.4mm. Ejection applies point loads, and thin sections or large unsupported flats can spring under them, so a slight crown is more desirable than a large flat face wherever the part allows one.

Undercuts close out this decision set. Each one forces a side core or moving slide into the die, and every moving component adds tooling cost, a wear surface, a maintenance item, and tolerance variation. Classic guidance is blunt: avoid undercuts unless the savings fully warrant the extra die and operating cost, and design the cores that remain for easy withdrawal. Challenge every undercut in review, first by trying to move the feature to the parting line, then by asking whether two simpler castings or a machined feature would serve the part better.

Tolerances and machining stock: decide what stays as cast

Die casting holds respectable tolerances as cast, but only if the drawing respects how the process works. The NADCA Product Specification Standards define two as-cast tiers for linear dimensions formed within one die half with no moving components involved. The Standard tier runs about ±0.25mm for the first 25mm of dimension plus about ±0.025mm for each additional 25mm, so a 127mm dimension carries roughly ±0.35mm. The Precision tier reaches about ±0.05mm for the first 25mm, giving roughly ±0.15mm on that same 127mm dimension, and it applies to radii, diameters, and wall thicknesses as well.

Crossing the parting line or passing over a moving slide opens those windows, with published adders in the region of 0.30mm Standard and 0.13mm Precision across the parting line, comparable adders for die slides, and parting-line shift looked up by projected area. Precision tolerances cost real money, typically 10 to 25 percent on the part through higher scrap, more inspection, and faster tool wear, so the discipline is to default the whole part to Standard and promote only the features whose function demands more. Anything tighter than the Precision tier is a machining decision, and machining brings critical features to roughly ±0.025mm. Machining tolerances covers that territory and CNC machining covers the operations themselves.

Machining brings its own design rules. Leave a minimum of about 0.25mm of stock so the cutter clears the dense cast skin rather than skimming it, because the skin is the densest, strongest zone and the metal beneath it is coarser and may carry micro-porosity. Published per-surface guidance on aluminum puts sealing faces around 0.8 to 1.5mm, non-sealing bolt flanges at 0.5 to 0.8mm, bores to be drilled or reamed at 0.5 to 1.0mm on diameter, and blind threaded holes at 1.5 to 2.0mm under the tap drill. Zinc parts often need no machining at all, and where they do, published allowances run about 0.3 to 0.5mm per surface. Locate the casting from datum points in the same die half as the feature being machined, so the machined dimension does not inherit parting-line variation. Technical drawing requirements covers how to state the datums and tier choices so a die caster can actually quote them.

Alloy choice shifts every number above

Alloy selection moves draft, walls, tolerances, tooling economics, and part weight together, which is why it belongs at the start of a design rather than the end. Zinc is the most forgiving to cast: it needs the least draft, holds the thinnest walls and the tightest tolerances, takes fine detail and plating, and runs small detailed parts at 200 to 550 shots per hour against 40 to 200 for aluminum, with die life averaging on the order of 500,000 shots in zinc versus about 125,000 in aluminum and roughly 100,000 to 200,000 shots in magnesium. Aluminum sits in the middle on tolerance and wall. Magnesium solidifies fast, behaves well dimensionally, and punishes sharp corners as the fillet section notes. Weight differs by a factor of nearly four across the family, with relative weights of about 1.0 for magnesium, 1.5 for aluminum, and 3.7 for zinc, a real lever on weight-critical assemblies.

Inside aluminum, grade choice is a design input too. ADC12, the common grade in Asian supply, carries 9.6 to 12.0 percent silicon against 7.5 to 9.5 percent for A380, the North American workhorse covered by ASTM B85, and the higher silicon gives ADC12 better fluidity into thin, intricate features. A380 carries more copper, 3.0 to 4.0 percent against 1.5 to 3.5 percent, with slightly higher published yield strength, roughly 160 to 180 MPa against 150 to 170 MPa, which suits structural parts. Treat ADC12 as closest to the A383-class alloys and commonly quoted against A380, not as a drop-in equivalent. In zinc, Zamak 3 is the general-purpose grade with the best ductility and long-term dimensional stability, while Zamak 5 trades some ductility for higher strength and hardness. The materials overview grounds these families by property.

Die casting design checklist

Run this pass before the file leaves the desk. Each item names the defect it prevents, because that is the surest way to judge whether an exception is safe to make.

Walls and fill:

• Wall thickness inside the alloy’s design band, uniform within about 10 percent around cored holes and metal savers, with gradual transitions where thickness changes. Prevents misruns, cold shuts, shrinkage porosity, sink, and warp.
• Thick zones cored out rather than left solid, and local mass such as bearing seats cored from the back. Prevents porosity and sink at mass concentrations.

Draft:

• Every face parallel to the die opening drafted, inside faces at about twice the outside value, holes more than either. Prevents drag, galling, and stuck parts.
• Draft checked at feature depth rather than as one flat number, with short features steeper than deep ones.
• Textured surfaces carrying the texture adder of about 1 degree per 0.025mm of texture depth.
• Cast lettering at 0.3mm minimum depth and 10 degrees minimum draft, examined outside the depth method.

Ribs, bosses, and fillets:

• Ribs at 40 to 60 percent of the wall, no taller than three wall thicknesses, spaced three to five wall thicknesses apart, base filleted at 0.3 to 0.5mm. Prevents sink and junction porosity.
• Bosses cored, filleted, and rib-fed, with wall stock around cored holes under 6.4mm at least half the hole diameter. Prevents boss porosity.
• All inside corners filleted, 1.5mm minimum at metal savers and clearance holes, 0.8mm at functional and locating holes, with only the parting-line perimeter left sharp. Prevents hot tears and aids fill.

Holes:

• Cored holes above the alloy minimum diameter and within the depth-to-diameter guidance, with smaller holes flagged for drilling after casting.

Parting line and ejection:

• Straight parting line where possible, most geometry in the ejector half, cosmetic faces on the cover side.
• Critical dimensions within one die half, with none tightly toleranced across the parting line or a slide.
• Ejector-pin locations planned, with marks acceptable on the faces that carry them.
• Every undercut challenged, and each survivor justified against the slide it forces into the die.

Tolerances and machining:

• Tolerance tier set per feature: Standard by default, Precision only where function demands it, machined where tighter. Precision typically adds 10 to 25 percent.
• Machining stock specified at 0.25mm minimum and 0.5 to 1.5mm typical on aluminum faces, with the datum in the same die half as the machined feature.

Export the model with explicit units and a drawing that states the alloy, the tolerance tier per feature, and the datum scheme; CAD file formats covers what die casters actually read. The vocabulary shared with the rest of the site’s process pages sits in the manufacturing glossary, and the process fundamentals behind every rule here are on the die casting hub.