Design aluminum die castings with 2-3 mm walls, a typical minimum of 1.5 mm and 1.0 mm only on small parts, keeping wall variation under 2:1. Use 1-2° draft on external surfaces and 2-3° on internal surfaces and cored holes, because aluminum shrinks roughly 0.6% and grips internal cores. Fillet every internal corner at 0.5 times wall thickness and never below 1 mm, size ribs at 60-80% of the adjoining wall, and keep boss diameter under twice the wall at the base. As-cast features hold ±0.1 mm for the first 25 mm plus ±0.025 mm per additional 25 mm; leave 0.5-1.0 mm of machining allowance wherever you need ±0.02 mm.
The most expensive drawing we ever reviewed had a 6 mm boss standing on a 2 mm wall, with a sharp internal corner at its base, on a sealing face that crossed the parting line. Fixing those four decisions at DFM took two days; fixing them after the die was cut would have cost $6,000 and three weeks.
This is the reference we work from during that review. Each rule carries a target value and the physical reason it exists, because a rule you understand is one you can bend correctly.
Design rule quick reference
| Feature | Target | Practical limit | Governing reason |
|---|---|---|---|
| Wall thickness | 2.0-3.0 mm | 1.5 mm typical, 1.0 mm on small parts | Fill before freeze |
| Wall variation | Under 1.5:1 | 2:1 | Isolated liquid pockets void |
| Flow length per gate | 60 × wall | 100 × wall | Front stiffens at 20-30% solid |
| External draft | 1.5° | 1° | Ejection without drag |
| Internal draft and cored holes | 2.5° | 2° | 0.6% shrink grips the core |
| Internal fillet radius | 0.5 × wall | 1.0 mm | Heat checking and hot spots |
| External radius | Internal R + wall | 0.5 mm | Uniform wall through the corner |
| Rib thickness | 60-80% of adjoining wall | 1.0 mm | A thick rib is thermal mass |
| Rib height | ≤ 5 × rib thickness | 8 × with draft relief | Fill and ejection |
| Rib spacing | ≥ 2 × wall | 3 mm | Thin die steel runs hot |
| Boss diameter at base | ≤ 2 × wall | 2.5 × wall with relief | Shrink porosity and sink marks |
| Cored hole diameter | ≥ 4 mm | 2.5 mm | Core pin strength |
| Cored hole depth | ≤ 3:1 blind under 5 mm dia. | 5:1 above 5 mm, 8:1 through | Pin deflection and heat |
| Machining allowance | 0.5-1.0 mm | 0.3 mm | Clear draft and distortion |
| Cast datum pads | Three, 8-12 mm dia. | — | Repeatable fixturing |
| Raised text height | 0.3-0.5 mm | — | Recessed text traps dirt |
Wall thickness
| Part size, largest dimension | Minimum wall | Recommended wall |
|---|---|---|
| Under 50 mm | 1.0 mm | 1.5-2.0 mm |
| 50-150 mm | 1.5 mm | 2.0-2.5 mm |
| 150-300 mm | 2.0 mm | 2.5-3.0 mm |
| Over 300 mm | 2.5 mm | 3.0-4.0 mm |
Reaching 1.0 mm usually means ADC12, whose near-eutectic silicon keeps metal fluid longer in a thin section.
Why thin and uniform beats thick
Solidification time scales with the square of section thickness, so a 4 mm wall freezes four times slower than a 2 mm wall. That stretches the dwell portion of the 30 to 90 second cycle and shows up in piece price. Above about 6 mm the thermal centre freezes so late that no liquid reaches it, giving shrinkage porosity and a sink mark opposite. The instinct to add thickness for strength is backwards here. Add a rib.
Uniformity matters even more than the absolute number. Aluminum freezes from the die wall inward, so a thick region separated from the gate by a thin one gets cut off when that thin section solidifies, left shrinking with nothing to draw on. This is the mechanism behind almost every internal void we find, described further in how aluminum die casting works. Keep thickest-to-thinnest under 1.5:1 where you can, 2:1 as a hard target, and blend any change over at least three times the thickness difference.
Flow length
Thickness alone does not tell you whether a part will fill. Divide the longest path from gate to last-fill point by the local wall thickness there: under 60 is comfortable, up to 100 workable with good gating and a high-silicon alloy, above 100 designs in cold shuts. A 1.5 mm wall reaches roughly 90 to 150 mm per gate, a 3 mm wall 180 to 300 mm.
Draft angle
| Surface | Draft | Note |
|---|---|---|
| External walls | 1-2°, use 1.5° | Below 1° expect drag marks |
| Internal walls and pockets | 2-3°, use 2.5° | Shrink grip on the core |
| Cored holes | 2-3° | Remember the hole is tapered |
| Deep features over 25 mm | Add 0.5° per additional 25 mm | Ejection force grows with contact area |
| Rib sides | 1-2° per side | Never zero |
| Raised text sidewalls | 10-15° | Small features need heavy draft |
The asymmetry between internal and external draft comes down to shrink direction. Aluminum contracts roughly 0.6% linearly between solidification and ejection, so an external wall shrinks away from the die surface that formed it, opening a gap, while an internal wall shrinks onto the core inside it. A 60 mm bore closes about 0.35 mm onto its core, and that grip has to be broken by ejector force.
Two consequences get missed. Draft consumes wall thickness: 2.5° over a 40 mm pocket is 1.75 mm of taper, so a nominal 2.5 mm wall drafted from the top is 0.75 mm at the bottom unless you draft from the middle. And a cored hole is a cone, so machine the bore afterwards if a bearing presses into it.
Fillets and radii
Every internal corner gets a fillet, at 0.5 times the local wall with 1.0 mm as the floor: a 2.5 mm wall gets R1.25 and a 3 mm wall R1.5. External corners take internal radius plus wall thickness, which keeps the wall uniform as it turns. A generous internal fillet with a sharp external corner creates a locally thin section, and the reverse creates a thick one.
Four things go wrong without fillets:
- The die heat-checks there first. A sharp internal corner on the part is a sharp external corner in steel, a thin edge cycling between 180-280 °C and 700 °C. It cracks by thermal fatigue and prints crack lines onto every part, which is what limits a die to 80,000 to 150,000 shots.
- Mass concentrates. A sharp junction holds more metal than the walls it joins, so it freezes last and develops shrinkage porosity.
- Flow turns abruptly. A front hitting a sharp corner at 30 to 50 m/s separates and folds oxide into the casting.
- Stress concentrates. A380 gives 3.5% elongation and little capacity to yield around a stress riser.
Ribs
Ribs are how a casting gets stiff without getting thick. Bending stiffness scales with the cube of depth, so a rib standing 8 mm off a 2.5 mm wall beats thickening that wall to 4 mm, at no cost in cycle time.
| Parameter | Target | Reason |
|---|---|---|
| Thickness | 60-80% of adjoining wall, min 1.0 mm | A thicker rib is thermal mass and prints a sink mark opposite |
| Height | ≤ 5 × rib thickness | More draft and higher ejection force |
| Draft | 1-2° per side | Deepest thin features in the die |
| Spacing | ≥ 2 × wall, min 3 mm | Die steel between close ribs runs hot and cracks |
| Base fillet | ≥ 0.5 × rib thickness | Junction mass and heat checking |
| Top radius | ≥ 0.5 mm | Fill of the rib tip |
A 2 mm rib grid on 20 mm centres over a 2.5 mm wall behaves well. At 3 mm thickness on 8 mm centres it becomes a die maintenance problem with sink marks on the show face.
Bosses
A boss is a rib rolled into a cylinder, with the same failure mode: concentrated mass.
- Base outside diameter no more than 2 times the local wall.
- Core it. A solid 10 mm cast pillar has a thermal centre that holds porosity and prints a sink mark behind it.
- Unsupported height under 2 times base diameter; above that, tie the boss into nearby walls with gussets, which stiffens it and creates a feed path.
- Behind a cosmetic surface, add a relief pocket to balance local mass.
Holes: cored versus drilled
| Situation | Cast it | Drill it after casting |
|---|---|---|
| Diameter 4 mm and above | Yes | If tolerance demands |
| Diameter 2.5-4 mm | Possible, short depth only | Usually better |
| Diameter under 2.5 mm | No | Yes |
| Blind depth over 3× diameter (pins under 5 mm) | No | Yes |
| Position tighter than ±0.15 mm | No | Yes |
| Needs straight, untapered wall | No | Yes |
| Crosses the parting line | Avoid | Yes |
| Fastener clearance only | Yes | No |
Core pins are thin steel columns surrounded by aluminum at 700 °C, unsupported at one end for a blind hole. They run hot, deflect under the metal front, and are the most frequently replaced item in any die. That is the entire reason for the diameter and depth limits.
For a hole needing precision, cast a pilot 0.5 to 1.0 mm undersize and finish it in the machining operation, which gives location from the casting and holds ±0.02 mm where it matters.
Threads
Recommendation: do not cast threads. Cast a cored pilot and tap after casting.
Cast-in internal threads need an unscrewing mechanism in the die, adding tool cost, cycle time and a maintenance item, and the thread carries 2 to 3° of draft so the fit is compromised over its depth. External cast-in threads above M6 are feasible if the axis lies along the draw, but they still carry draft.
Tapping practice for cast aluminum:
- Range. M3 through M12. Below M3, use a thread-forming screw into a cored hole.
- Depth. 1.5 to 2 times nominal diameter of full thread. Aluminum threads strip well before steel.
- Cored pilot. 0.4 to 0.6 mm under tap drill size with 2° draft, so the drill cleans up the taper. For M5 × 0.8 the tap drill is 4.2 mm, so core at about 3.7 mm.
- Surrounding material. At least 0.6 times screw diameter of wall around the hole.
- Repeated assembly. Specify a press-in steel insert. Cast threads tolerate a handful of removal cycles, not a hundred.
Parting line placement
The parting line is the most consequential decision in the tool layout. Have an opinion before the toolmaker chooses for you.
- Place it at the largest projected cross section so both halves can draw.
- Put it on an edge or step where a 0.1 to 0.3 mm witness line is acceptable, never across a sealing or cosmetic face. Expect 0.05 to 0.15 mm of flash there.
- Keep every accurate dimension inside one die half. Measuring across halves adds ±0.10 to ±0.15 mm, because they close with small variability and flash thickness varies shot to shot.
- Keep a sealing face, its gasket groove and its mating bolt pattern in the same half.
Undercuts and slides
Any feature that cannot draw in the open and close direction needs a slide, a lifter or a loose insert. Each one costs:
- $2,000 to $5,000 in additional tool cost.
- 2 to 4 seconds of cycle time.
- ±0.15 mm added to any dimension across the slide.
- An additional witness line and flash path.
- A recurring maintenance item, as slide faces wear and gall.
Before accepting a slide, try rotating the feature into the draw direction, reaching it from the opposite side as a through hole, machining it after casting, or splitting the part. Slides are worth paying for when they delete a machining setup, not to preserve a styling detail. Tool cost drivers are on our die casting tooling page.
Ejector pins
Ejector pins push hard. Plan one pin per 20 to 40 cm² of die contact area, typically 6 to 12 mm diameter, landing on structure that takes the load: rib intersections, boss tops, wall junctions, thickened pads. A pin bearing on an unsupported 1.5 mm wall leaves a dimple or bends the part, and every pin leaves a 0.05 to 0.15 mm witness.
Mark cosmetic and sealing faces as no-pin zones on the drawing. Otherwise the toolmaker places pins wherever ejection is easiest, which is exactly where the flat open faces are.
Machining allowance and cast datums
Leave 0.5 to 1.0 mm of stock on faces you intend to machine, and 0.3 mm as the minimum for a light facing pass.
Resist leaving more. The as-cast skin is the densest, finest-grained material on the part, formed against chilled steel under 40 to 100 MPa, so cutting deeper moves into the region where porosity lives. Excessive allowance is a common cause of porosity that appeared during machining when it was there all along. Check the draft arithmetic first: a wall drafted at 1.5° over 40 mm has 1.05 mm of taper.
Cast datum features are the other half of this. A casting is drafted, radiused and slightly distorted, so clamping on those surfaces gives an unrepeatable setup and the position errors get blamed on the casting. Design three raised pads, 8 to 12 mm diameter and 0.5 to 1.0 mm proud, in the same die half, positioned for a 3-2-1 scheme and called out as datums A, B and C, plus two cast holes for locating pins. This costs nothing in the die and removes most of the dimensional argument between casting and machining.
Tolerances you can actually hold
As-cast linear tolerance is ±0.1 mm for the first 25 mm of dimension, plus roughly ±0.025 mm for each additional 25 mm, measured within one die half.
| Nominal dimension | As-cast, one die half | After machining |
|---|---|---|
| Up to 25 mm | ±0.10 mm (±0.004 in) | ±0.02 mm |
| 25-50 mm | ±0.13 mm | ±0.02 mm |
| 50-100 mm | ±0.18 mm | ±0.03 mm |
| 100-150 mm | ±0.23 mm | ±0.04 mm |
| 150-250 mm | ±0.33 mm | ±0.05 mm |
Adders and geometric limits:
| Condition | Allowance |
|---|---|
| Dimension crosses the parting line | Add ±0.10 to ±0.15 mm |
| Dimension crosses a slide or moving core | Add ±0.15 mm |
| Flatness, as-cast | 0.2-0.4 mm per 100 mm |
| Flatness, machined | 0.02-0.05 mm per 100 mm |
| Cored hole diameter | ±0.10 mm, plus draft taper |
| Concentricity across the parting line | 0.25 mm |
| Surface roughness | Ra 1.6-3.2 µm as-cast, Ra 0.8 µm machined |
| Wall thickness | ±0.15 mm |
Two habits save real money. Put general as-cast tolerances in the title block and call out only the features that need more, because a drawing tight everywhere gets quoted as if all of it needs machining. And state the datum scheme, since a tolerance without a datum is not a specification.
Part consolidation
The largest cost reduction in casting rarely comes from the casting. It comes from deleting the parts around it.
A bracket assembly we quoted recently was two stamped plates, a machined spacer, four screws and two assembly operations, at $11.40 assembled. As one A380 casting with the spacer integrated and the fastener bosses cast in, it came to $4.20 finished, with a tighter stack-up because the tolerance chain went from five contributors to one. Look for fastened sub-assemblies, welded brackets and parts that exist only as spacers.
Design checklist
Run this before releasing a model for quotation:
- Walls 1.5-3 mm, variation under 2:1, transitions blended.
- Longest flow path under 100 × local wall.
- Draft 1-2° external, 2-3° internal and cored, modelled not assumed.
- Wall thickness re-checked after draft.
- Internal corners filleted at 0.5 × wall, min 1 mm; external radii internal + wall.
- Ribs 60-80% of wall, height under 5 × rib, spacing over 2 × wall.
- Bosses cored, base under 2 × wall, gusseted not thickened.
- Cored holes 4 mm or larger, blind depth within 3:1, none across the parting line.
- Threads tapped, pilot cored, depth 1.5-2 × diameter.
- No undercuts, or each one justified against its slide cost.
- Parting line proposed by you, off cosmetic and sealing faces.
- Cosmetic and sealing faces marked as no-pin zones.
- 0.5-1.0 mm machining allowance, checked against draft taper.
- Three cast datum pads plus two locating features, one die half.
- General tolerances in the title block, datums declared.
- Raised text 0.3-0.5 mm, no recessed text.
- Adjacent parts reviewed for consolidation.
File preparation and what to send with a request for quotation are covered in preparing CAD files for die casting, and common aluminum die casting defects maps each defect back to the design decision that caused it.
Our engineers run this checklist against every model quoted through aluminum die casting services and return a written DFM report with marked-up geometry rather than generic advice. Send STEP or Parasolid files plus a 2D drawing through contact and you will have it within 48 hours, before anyone commits to steel.
