Die casting offers productivity, precision and surface quality for high-volume metal components, but success depends heavily on part design that respects the physics of rapid filling and solidification under pressure. Poorly conceived features like uneven wall thickness, sharp corners, excessive mass concentration, or overly tight tolerances will lead to filling defects, porosity, shrinkage, distortion, cracking, and premature die wear, driving up cost and scrap. Following these recommendations from the earliest design stage ensures defect-free castings, maximum mechanical performance, and delivers the most cost-effective balance between functionality and manufacturability.
Wall Thickness
If the wall thickness of a die-cast part is too thin, it is difficult to fill during die casting, easily leading to poor filling. If the wall thickness is too thick, coarse internal grains are likely to form, resulting in defects such as shrinkage cavities and porosity. Additionally, surface sink marks may appear, reducing the mechanical properties of the die-cast part. Thin-walled parts offer good density, relatively improving strength and pressure resistance. Excessively thick walls also increase part weight and consume excessive metal, raising costs. In general, the wall thickness of die-cast parts should not exceed 5 mm.
Wall Thickness for Aluminum, Magnesium, and Zinc Alloys (unit: mm)
| Wall area (cm²) | Aluminum & Magnesium Alloys | Zinc Alloys |
| Minimum | Recommended | |
| ≤25 | 0.8 | 2.0 |
| 25–100 | 1.2 | 2.5 |
| 100–500 | 1.8 | 3.0 |
| >500 | 2.5 | 3.5 |
If certain local areas of the part are excessively thick, a hollowed-out design should be used to achieve uniform wall thickness throughout. This approach prevents shrinkage defects in thick areas while reducing part weight.
Smooth transitions at thickness changes
The wall thickness of each cross-section of a die-cast part should be uniform or as close to uniform as possible. Where functional or other requirements prevent full uniformity, the thick-to-thin wall ratio should not exceed 3:1. Gradual transitions (taper or radius) should be introduced to avoid abrupt thickness changes; otherwise, molten metal flow may be impaired, leading to flow marks or cold shuts. Additionally, differing solidification times between thick and thin sections generate uneven internal stresses, which can cause cracking or distortion. In cases of sharp thickness transitions, adding a taper or radius to ensure a smooth transition is recommended.
In the above figure, design#a is the worst, design#d is the best design.
Minimum Holes
Minimum hole diameter and maximum hole depth for aluminum, magnesium, and zinc alloys (unit: mm)
If a hole is smaller or deeper than the values in the table, it can still be partially formed during die casting (as a pilot mark) and then finished by machining, though this increases part cost.
The distance between holes, between holes and grooves, and between holes and edges must also be considered to ensure the die has sufficient strength to withstand the impact and severe thermal stresses from high-temperature molten metal.
| / | Mimimum diameter of hole | Depth of hole: times diameter(d ) | ||||
| Material | Recommended | Feasible | Non-through hole | Non-through hole | Through hole | Through hole |
| / | / | / | d >5 | d <5 | d >5 | d <5 |
| Aluminum alloy | 2.5 | 2.0 | 4 | 3 | 8 | 6 |
| Magnesium alloy | 2.0 | 1.5 | 5 | 4 | 10 | 8 |
| Zinc alloy | 1.5 | 0.8 | 6 | 4 | 12 | 8 |
Avoid Too Thin Sections
Thin die sections have low strength and are prone to deformation, bending, or fracture under high temperatures.
Ribs
Ribs are primarily used to enhance part strength, prevent deformation, and secondarily to assist molten metal flow. Recommended rib dimensions are shown in the table below.
Recommended Rib Dimension Table (unit: mm)
| Item | Recommended dimension |
| Part wall thickness | – |
| Root thickness t | t = (0.6 ~ 1) × T |
| Height H | H ≤ 5T |
| Fillet radius R | t ≤ R ≤ 1.25t |
| Draft angle α | α = 1° ~ 3° |
- Avoid flat-plate designs; adding ribs improves part strength.
- Ribs can assist in the flow of molten metal; their orientation should align with the direction of the metal flow.
- Rib placement should be reasonable, symmetrical, and evenly distributed.
- Avoid excessive thickness buildup at rib junctions.
Draft Angles
Due to differing adhesion tendencies between the three common die-casting alloys and the die, typical draft angles are:
- Aluminum alloys: highest adhesion → internal draft generally 1°
- Magnesium alloys: slightly lower adhesion than aluminum → internal draft generally 0.75°
- Zinc alloys: lowest adhesion → internal draft generally 0.5°
External draft angles can be twice the internal draft to ensure the casting remains on the core side during ejection.
Fillet Radius Design
Avoid external sharp corners. Sharp external corners not only cause underfilling, poor density, and low strength, but also pose safety risks due to sharp edges.
- Internal fillets – avoid internal sharp corners. Fillet radii at wall-to-wall junctions significantly affect part performance, quality, and die life.
- Improve molten metal flow, reduce turbulence, enhance fill ability, and facilitate gas escape.
- Sharp corners cause stress concentration, leading to cracking or premature failure under load.
When plating is required, fillets ensure uniform coating and prevent buildup at sharp corners.
Internal fillet radius is typically equal to the wall thickness. Fillet radii must not be excessively large, as this creates locally thick sections prone to shrinkage, porosity, and surface sink marks.
Boss
- Avoid placing bosses too close to walls or to each other. Boss design must follow uniform wall thickness principles and avoid localized excessive thickness.
- Minimize boss height. Excessive height reduces strength and hinders filling.
- Add ribs around bosses. Ribs increase boss strength and aid filling; isolated bosses should be avoided.
- Redesign inclined bosses to simplify the die structure. Proper optimization of inclined bosses can simplify the die and reduce cost.
Text/Characters
- Characters should be raised (proud) from the part surface. This reduces die machining and maintenance costs.
- Character dimensions must ensure proper filling. Minimum character width is 0.25 mm, height is about 0.25 to 0.5 mm, with a 10° draft. Characters should generally not be placed on sidewalls, as this creates undercuts that prevent ejection.
Threads
- Avoid full-thread external threads.
- Internal threads should not be directly cast.
Facilitate Flash and Gate Removal
- Avoid acute angles between part walls and the parting line.
- Simplify part geometry to avoid complex parting line shapes that complicate flash removal.
Tolerances
The parting line and core slides influence dimensional tolerance accuracy.
Under the premise of meeting functional requirements, relax tolerance requirements as much as possible:
- Tighter tolerances require tighter die tolerances → higher die cost
- The lifespan of the die is shortened
- Frequent die maintenance and replacement are needed
- More frequent dimensional checks and higher scrap rates → increased part cost
To avoid machining, tolerances should be as generous as possible. Avoiding machining reduces part cost.
Select the parting line rationally to improve critical dimensional accuracy:
- If concentricity between D1 and D2 is critical → choose C-C as parting line
- If concentricity between D1 and D3 is critical → choose B-B as parting line
- If the diameter consistency of D1 at the left or right end is critical → choose A-A as the parting line
Simplify Die Structure
(1) Avoid internal undercuts. Internal undercuts require side-action cores or secondary machining will lead to significantly higher die or part cost. Reasonable part design, eliminating internal undercuts, reduces cost.
(2) Avoid external undercuts where possible.
(3) Avoid obstructions to core slides.
(4) Avoid rounded parting lines. Rounded parting lines complicate die manufacture, reduce strength at the radius, and shorten die life.
(5) Choose the parting line wisely to simplify the die structure. The parting line should result in the simplest possible die construction, easiest machining, and lowest cost.
CNC Machining
Avoid CNC machining whenever possible because:
- Die castings already achieve high dimensional accuracy and surface finish; generous tolerances during design can eliminate machining.
- The surface skin of a die casting is dense and strong; machining destroys this layer.
- Internal porosity may be exposed after machining, affecting performance.
- Machining significantly increases part cost.
When machining is unavoidable, design the part to facilitate machining and minimize the machined area.
Keep the machining allowance as small as possible. The outer skin is dense, while the interior is relatively porous with possible gas holes or pinholes; therefore, machining allowance should be minimized to preserve the dense layer.
Surface Machining Allowance (single side, unit: mm)
| Max dimension of machined face | ≤50 | 50–120 | 120–260 | 260–400 | 400–630 |
| Allowance | 0.3–0.5 | 0.4–0.7 | 0.6–1.0 | 0.8–1.4 | 1.2–1.8 |
Hole Machining Allowance (single side, unit: mm)
| Hole diameter | ≤6 | 6–10 | 10–18 | 18–30 | 30–50 | 50–80 |
| Allowance | 0.05 | 0.10 | 0.15 | 0.20 | 0.25 | 0.30 |
Remember:
- Avoid surface machining wherever possible.
- Where machining is required, keep allowance as small as possible (generally less than 0.5–0.8 mm).
- After machining, no internal porosity or loose structure should be exposed, otherwise, strength and pressure tightness will be severely compromised.
