Die casting design guidelines

Die castings typically use uniform walls of 0.060–0.150 in (1.5–3.8 mm) in aluminum and 0.040–0.100 in (1.0–2.5 mm) in zinc, draft of about 1° outside and 2° inside for aluminum and half that for zinc, and inside radii of at least 0.040 in (1 mm). Linear tolerances run ±0.002–0.010 in (±0.05–0.25 mm) on the first inch per NADCA.

Try the interactive lab Check a part in the builder

Aluminum wall: 0.060–0.150 in
Zinc wall: 0.040–0.100 in
Aluminum draft: 1° outside, 2° inside
Linear tolerance: ±0.002–0.010 in

SSG MFG · design guideDG-07 · 12 rules

What are the die casting design rules?

12 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.

Design rules and typical values
#	Rule	Typical value
01	Keep walls uniformAluminum 0.060–0.150 in (1.5–3.8 mm); zinc 0.040–0.100 in (1.0–2.5 mm); minimum about 0.040 in (1.0 mm) aluminum, 0.020 in (0.5 mm) zinc	Aluminum 0.060–0.150 in (1.5–3.8 mm); zinc 0.040–0.100 in (1.0–2.5 mm); minimum about 0.040 in (1.0 mm) aluminum, 0.020 in (0.5 mm) zinc
02	Core out heavy sectionsPocket any section more than about 1.5× nominal wall from the back side, leaving ribs	Pocket any section more than about 1.5× nominal wall from the back side, leaving ribs
03	Add draft to every wall in the line of drawAluminum about 1° outside, 2° inside; zinc about 0.5° outside, 1° inside; deep cores need more	Aluminum about 1° outside, 2° inside; zinc about 0.5° outside, 1° inside; deep cores need more
04	Radius corners and filletsInside radius at least 0.040 in (1 mm); outside radius equals inside radius plus wall	Inside radius at least 0.040 in (1 mm); outside radius equals inside radius plus wall
05	Stiffen with ribs, not massRib base about equal to nominal wall; height up to about 4× wall; 1–2° draft per side; root fillet at least 0.040 in (1 mm)	Rib base about equal to nominal wall; height up to about 4× wall; 1–2° draft per side; root fillet at least 0.040 in (1 mm)
06	Core bosses and tie them to wallsBoss wall about equal to nominal wall; core the center; connect to adjacent walls with ribs	Boss wall about equal to nominal wall; core the center; connect to adjacent walls with ribs
07	Size cored holes to the alloyZinc at least 0.040 in (1 mm) diameter; aluminum at least 0.100 in (2.5 mm); depth no more than about 4× diameter; draft the pin	Zinc at least 0.040 in (1 mm) diameter; aluminum at least 0.100 in (2.5 mm); depth no more than about 4× diameter; draft the pin
08	Avoid undercuts where you canTarget zero slides; small zinc parts can run in multi-slide dies with up to 4 slides	Target zero slides; small zinc parts can run in multi-slide dies with up to 4 slides
09	Keep critical dimensions in one die halfPut the parting line on one flat plane off sealing and cosmetic faces; add about ±0.004 in (±0.10 mm) or more across it	Put the parting line on one flat plane off sealing and cosmetic faces; add about ±0.004 in (±0.10 mm) or more across it
10	Minimize machining stockLeave 0.010–0.030 in (0.25–0.75 mm) on machined faces; mark machined features on the casting drawing	Leave 0.010–0.030 in (0.25–0.75 mm) on machined faces; mark machined features on the casting drawing
11	Plan ejector pin locationsFlat, non-cosmetic pads, typically 0.25–0.50 in (6–13 mm) across, near deep features and bosses	Flat, non-cosmetic pads, typically 0.25–0.50 in (6–13 mm) across, near deep features and bosses
12	Specify pressure tightness explicitlyCall out leak test pressure, rate and impregnation per MIL-STD-276 if required	Call out leak test pressure, rate and impregnation per MIL-STD-276 if required

These build on the short list on the die casting process page, with the failure each rule prevents and a drawing for each.

How much draft does a part need to release?

Change the draft angle and the depth of a wall to see how drag on ejection grows as draft shrinks and walls get deeper. An aluminum core needs about twice the draft of the same core in zinc because aluminum shrinks onto the steel harder at ejection temperature.

DRAFT 2° · DEPTH 1.50 IN · ALUMINUM, INSIDE WALL

angle drawn 4× for legibility

Typical minimum here: 2°
Taper per side, H × tan θ: 0.052 in(1.33 mm)
Width change top to bottom: 0.105 in(2.66 mm)

Works: releases cleanly

2° meets the typical 2° for an inside wall in aluminum. The wall tapers 0.052 in per side over 1.50 in; put that on the model, not as a note.

Typical values per NADCA guidance: aluminum about 1° outside and 2° inside, zinc about half that. Deeper walls need the same angle but move more metal.

Why does each rule matter?

Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.

Rule 01

Keep walls uniform

Aluminum 0.060–0.150 in (1.5–3.8 mm); zinc 0.040–0.100 in (1.0–2.5 mm); minimum about 0.040 in (1.0 mm) aluminum, 0.020 in (0.5 mm) zinc

Why: Metal freezes in milliseconds, so thin walls must fill fast and thick walls must feed shrinkage from the gate.
If you ignore it: Thick sections trap shrinkage porosity that opens up when machined, and thin sections cold shut or fail to fill.

Standard: NADCA Product Specification Standards

Fig. 1Uniform wall

Do. Every wall within about 15% of nominal T, so the whole part cools and shrinks at one rate.

Avoid. A section twice as thick cools last: it pulls a sink mark into the face above it and can leave a void inside.

Rule 02

Core out heavy sections

Pocket any section more than about 1.5× nominal wall from the back side, leaving ribs

Why: Heavy sections are the last to freeze and draw liquid metal from the walls around them.
If you ignore it: Porosity and sink concentrate under bosses and pads, leak paths open on sealing faces, and part weight and metal cost climb.

Fig. 2Core out thick sections

Do. Hollow the section from the back into walls and ribs at T: same stiffness at the face, a fraction of the cooling time.

Avoid. A solid thick section takes several times longer to cool and still sinks at the surface and voids in the middle.

Rule 03

Add draft to every wall in the line of draw

Aluminum about 1° outside, 2° inside; zinc about 0.5° outside, 1° inside; deep cores need more

Why: Castings shrink onto cores and away from outside walls, so inside walls grip the die harder.
If you ignore it: Castings stick in the die, ejector pins punch through or distort the part, and the die galls and solders on the cores.

Standard: NADCA Product Specification Standards

Fig. 3Draft angle

Do. Walls taper by the draft angle in the line of draw; each side moves in by H × tan θ, and the part slides off the core.

Avoid. With zero draft the part grips the core as it shrinks: drag marks, scuffed texture, and ejector pins that dent or punch through.

Rule 04

Radius corners and fillets

Inside radius at least 0.040 in (1 mm); outside radius equals inside radius plus wall

Why: Radii keep metal flowing without turbulence and remove the sharp steel edges where die cracking starts.
If you ignore it: Hot spots and porosity form at sharp inside corners, and heat-check cracks grow in the die at every sharp edge and print onto the castings.

Fig. 4Inside and outside radii

Do. Inside radius at least half the wall and outside radius equal to inside plus T: the corner stays at thickness T and flow turns smoothly.

Avoid. A sharp inside corner concentrates stress about 3× and the corner runs thick: cracks start there, and it cools last.

Rule 05

Stiffen with ribs, not mass

Rib base about equal to nominal wall; height up to about 4× wall; 1–2° draft per side; root fillet at least 0.040 in (1 mm)

Why: Ribs add stiffness and act as flow paths to far corners without adding a thick section.
If you ignore it: Solid pads porosity-check and sink, and unribbed flat walls distort on ejection and trimming.

Fig. 5Rib proportions

Do. A rib 50–60% of the wall at its base, up to 3× the wall tall, with a small root radius: stiffness without a thick spot.

Avoid. A rib as thick as the wall doubles the mass where it joins, and the face behind it sinks.

Rule 06

Core bosses and tie them to walls

Boss wall about equal to nominal wall; core the center; connect to adjacent walls with ribs

Why: A solid boss is a heavy section. Coring it keeps the wall uniform and gives a hole for a thread-forming screw or tap.
If you ignore it: Solid bosses porosity-check when tapped, threads strip, and sink shows on the face behind.

Fig. 6Boss design

Do. Boss OD about 2× the hole, boss wall at most 60% of T, cored down to the wall and braced with gussets.

Avoid. A thick, solid boss is a heat sink in the middle of the part: sink on the show face and a void around the screw.

Rule 07

Size cored holes to the alloy

Zinc at least 0.040 in (1 mm) diameter; aluminum at least 0.100 in (2.5 mm); depth no more than about 4× diameter; draft the pin

Why: Core pins sit in the hottest metal. Small, deep pins overheat, bend and bond to the casting.
If you ignore it: Core pins bend, break or solder to the casting, holes come out tapered or off-position, and the die goes back for repair.

Standard: NADCA Product Specification Standards

Fig. 7Cored hole depth

Do. A drafted core pin no deeper than about 4× its diameter stays straight under injection pressure and releases cleanly.

Avoid. A long, thin pin deflects under metal pressure and heat checks; holes run off-position and pins break in production.

Rule 08

Avoid undercuts where you can

Target zero slides; small zinc parts can run in multi-slide dies with up to 4 slides

Why: Each slide adds die cost, build time and a moving joint that wears and flashes.
If you ignore it: Die cost and lead time grow, slide joints flash, and dimensions across the slide need extra allowance.

Fig. 8Undercuts and side actions

Do. Where an undercut is worth it, a slide pulls sideways before ejection. Better still, move the feature into the line of draw or use a pass-through core.

Avoid. A side hole with no side action locks the part in the steel; every slide or lifter added to fix it adds tool cost and cycle time.

Rule 09

Keep critical dimensions in one die half

Put the parting line on one flat plane off sealing and cosmetic faces; add about ±0.004 in (±0.10 mm) or more across it

Why: Die closure and slide movement add variation to any dimension that crosses them, and the parting line leaves flash.
If you ignore it: Mating features across the parting line drift out of tolerance, and trimmed flash leaves a ridge on the sealing face.

Standard: NADCA Product Specification Standards

Fig. 9Parting line

Do. A flat parting line at the largest section, off sealing and cosmetic faces, with critical dimensions inside one die half.

Avoid. A dimension across the parting line carries die-half mismatch and flash thickness, typically another ±0.004 in (±0.10 mm) or more.

Rule 10

Minimize machining stock

Leave 0.010–0.030 in (0.25–0.75 mm) on machined faces; mark machined features on the casting drawing

Why: The densest metal is in the outer skin. Light cuts stay in it; heavy cuts expose porosity.
If you ignore it: Heavy cuts open porosity on sealing faces and threads, and parts fail leak test or cosmetic inspection after machining.

Fig. 10Machining stock

Do. A thin, even allowance on the faces that need it; the datum sits on a machined face, and as-cast or as-forged faces stay as they are.

Avoid. Too much stock cuts through the dense skin into porous core on a casting; too little leaves scale or draft on a forging.

Rule 11

Plan ejector pin locations

Flat, non-cosmetic pads, typically 0.25–0.50 in (6–13 mm) across, near deep features and bosses

Why: Ejector pins push where the casting grips hardest and leave a witness mark wherever they land.
If you ignore it: Pin marks land on cosmetic or sealing faces, and a lack of push points near deep cores bends the part on ejection.

Rule 12

Specify pressure tightness explicitly

Call out leak test pressure, rate and impregnation per MIL-STD-276 if required

Why: Every die casting holds some gas and shrinkage porosity, so leak-tight parts need a defined test and process.
If you ignore it: Parts pass dimensional inspection and then leak in the field or at your assembly leak test.

Standard: MIL-STD-276

What tolerances can die casting hold?

Typical values for aluminum die castings. Standard tolerances are the NADCA default; precision tolerances need extra die work and process control. Zinc typically holds tighter than aluminum at the same size. Shrink allowance, about 0.5–0.7%, is built into the die by the diecaster.

Typical and tight tolerances with the cost of going tight
Feature	Typical	Tight	Cost of tight
Linear, first inch (25 mm)Standard vs precision per NADCA.	±0.010 in (±0.25 mm)	±0.002 in (±0.05 mm)	Moderate
Linear, each added inch	±0.001 in (±0.025 mm)	±0.001 in (±0.025 mm)	Moderate
Across the parting lineGrows with projected area.	Add ±0.004 in (±0.10 mm) or more	Add ±0.003 in (±0.08 mm)	Moderate
Across a slide	Add ±0.004 in (±0.10 mm) or more	Add ±0.003 in (±0.08 mm)	Moderate
Flatness, up to 3 in (75 mm)Machine sealing faces that need less.	0.008 in (0.20 mm)	0.005 in (0.13 mm)	High
Cored hole diameter	±0.003 in (±0.08 mm)	±0.0005 in (±0.013 mm) machined	High
Machined bore or face	±0.001 in (±0.025 mm)	±0.0005 in (±0.013 mm)	Moderate

Basis: NADCA Product Specification Standards for Die Castings. Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.

How does the material change the rules?

The same die casting rules shift with the alloy or compound.

Aluminum A380 (die cast)
A380 needs about 1° outside and 2° inside draft, walls of 0.060 in (1.5 mm) or more, and cored holes of 0.100 in (2.5 mm) or larger. Dies typically last 100,000–150,000 shots because aluminum heat-checks H13 faster than zinc.
Zinc Zamak 3
Zamak 3 fills walls down to about 0.020–0.040 in (0.5–1.0 mm), needs about half the draft of aluminum, and plates well. It is about 2.4× denser than aluminum, so thin walls matter more for part weight and metal cost.
Zinc Zamak 5
Zamak 5 adds copper for higher strength and hardness than Zamak 3 at slightly lower ductility. Design rules match Zamak 3; choose it where a thin wall or boss carries load.

Die casting design questions

What is the minimum wall thickness for die casting?

Zinc die castings typically fill walls as thin as 0.020–0.040 in (0.5–1.0 mm), and multi-slide zinc can go thinner on small parts. Aluminum typically needs 0.040–0.080 in (1.0–2.0 mm) at minimum, with 0.060–0.150 in (1.5–3.8 mm) as the comfortable production range. Larger parts and longer flow paths push the minimum up.

How much draft does a die casting need?

Aluminum castings typically need about 1° on outside walls and 2° on inside walls and cores. Zinc needs about half that: 0.5° outside and 1° inside. NADCA publishes formulas that scale draft with wall depth and alloy, so deep cores need more than shallow ones. Inside walls need more because the casting shrinks onto them.

What is NADCA and why does it matter for tolerances?

NADCA, the North American Die Casting Association, publishes the Product Specification Standards for Die Castings. It gives standard and precision tolerance tables by alloy for linear dimensions, dimensions across the parting line and slides, flatness, draft and cored holes. Citing it on a drawing gives the diecaster and buyer the same baseline.

How much machining stock should I leave on a die casting?

Leave about 0.010–0.030 in (0.25–0.75 mm) on faces that will be machined. The outer skin of a die casting is the densest metal, and porosity sits deeper in the section. Light cuts stay in the skin; heavy cuts expose voids on sealing faces and threads. Mark every machined feature on the casting drawing.

Why do die castings have porosity?

Die casting injects metal so fast that some air and die lubricant gas is trapped, and thick sections shrink as they freeze. Both leave voids. Uniform walls, good venting and overflows, vacuum assist and radiused corners reduce it. Parts that must hold pressure are typically leak tested and vacuum impregnated after machining.

Can die castings have threads?

External threads can be cast along the parting line or with slides, though they usually carry flash that needs chasing. Internal threads are normally tapped or formed in a cored hole after casting, with the core sized to the tap drill. Zinc can cast fine threads more readily than aluminum.

Check your part against these rules.

Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run die casting every day.

Build a part Send a drawing

Die casting design guidelines

Rule

Keep walls uniformAluminum 0.060–0.150 in (1.5–3.8 mm); zinc 0.040–0.100 in (1.0–2.5 mm); minimum about 0.040 in (1.0 mm) aluminum, 0.020 in (0.5 mm) zinc

Core out heavy sectionsPocket any section more than about 1.5× nominal wall from the back side, leaving ribs

Add draft to every wall in the line of drawAluminum about 1° outside, 2° inside; zinc about 0.5° outside, 1° inside; deep cores need more

Radius corners and filletsInside radius at least 0.040 in (1 mm); outside radius equals inside radius plus wall

Stiffen with ribs, not massRib base about equal to nominal wall; height up to about 4× wall; 1–2° draft per side; root fillet at least 0.040 in (1 mm)

Core bosses and tie them to wallsBoss wall about equal to nominal wall; core the center; connect to adjacent walls with ribs

Size cored holes to the alloyZinc at least 0.040 in (1 mm) diameter; aluminum at least 0.100 in (2.5 mm); depth no more than about 4× diameter; draft the pin

Avoid undercuts where you canTarget zero slides; small zinc parts can run in multi-slide dies with up to 4 slides

Keep critical dimensions in one die halfPut the parting line on one flat plane off sealing and cosmetic faces; add about ±0.004 in (±0.10 mm) or more across it

Minimize machining stockLeave 0.010–0.030 in (0.25–0.75 mm) on machined faces; mark machined features on the casting drawing

Plan ejector pin locationsFlat, non-cosmetic pads, typically 0.25–0.50 in (6–13 mm) across, near deep features and bosses

Specify pressure tightness explicitlyCall out leak test pressure, rate and impregnation per MIL-STD-276 if required

Feature

Typical

Tight

Cost of tight

Linear, first inch (25 mm)Standard vs precision per NADCA.

±0.010 in (±0.25 mm)

±0.002 in (±0.05 mm)

Moderate

Linear, each added inch

±0.001 in (±0.025 mm)

Moderate

Across the parting lineGrows with projected area.

Add ±0.004 in (±0.10 mm) or more

Add ±0.003 in (±0.08 mm)

Moderate

Across a slide

Add ±0.004 in (±0.10 mm) or more

Add ±0.003 in (±0.08 mm)

Moderate

Flatness, up to 3 in (75 mm)Machine sealing faces that need less.

0.008 in (0.20 mm)

0.005 in (0.13 mm)

High

Cored hole diameter

±0.003 in (±0.08 mm)

±0.0005 in (±0.013 mm) machined

High

Machined bore or face

±0.001 in (±0.025 mm)

±0.0005 in (±0.013 mm)

Moderate

What are the die casting design rules?

How much draft does a part need to release?