Design is where aluminum die casting projects succeed or fail. A clean 3D model that follows basic die casting rules will fill better, crack less, and need less machining and rework. A “pretty but unfriendly” design will fight the process at every step.
This guide focuses on design for aluminum die casting (DFM) – things like wall thickness, fillet radius, ribs, draft angle, parting line, and machining allowance – so mechanical engineers and product designers can avoid the most common traps.
What matters most in aluminum die casting design?
If you remember only a few rules, make them these:
- Keep walls as uniform as possible – most structural housings work well around 2.5–4.5 mm wall thickness.
- Add draft everywhere the steel slides off the casting – typically 1–3° on most faces, sometimes more on deep or textured walls.
- Replace sharp corners with fillets and radii – at least 0.5–1.0 mm, larger if you can.
- Use ribs and gussets instead of thick blocks – stiffness without heavy sections and shrinkage.
- Plan the parting line, ejector marks and overflow early – don’t treat them as an afterthought.
- Decide which features are cast and which are machined – and mark them clearly on the drawing.
Done well, these choices lower tooling risk, scrap rate, cycle time and machining cost – without changing your functional design.
| Design factor | Good starting guideline (aluminum HPDC) | If you ignore it… |
|---|---|---|
| Wall thickness | 2.5–4.5 mm, keep changes gradual | Short shots, porosity, distortion |
| Draft angle | 1–3° on most faces, more for deep / textured walls | Sticking, drag marks, die damage |
| Fillets & radii | ≥ 0.5–1.0 mm, larger where possible | Cracks, hot spots, stress concentrations |
| Ribs & gussets | Rib thickness ≈ 0.5–0.7 × adjoining wall | Shrink sinks, warping, excess weight |
| Bosses | Hollow with core; base thickness ≈ 1.5 × wall | Porosity in bases, fill problems |
| Holes & windows | Add draft, keep edge distances ≥ 1.5× wall thickness | Cracking, poor fill, ejection problems |
| Machining allowance | 0.3–0.6 mm on critical faces/bores | Missed tolerances or unnecessary metal |
Numbers above are typical starting points – the best values still depend on alloy, part size and casting machine.
Aluminum Die Casting Design Basics: Process Before CAD
Aluminum die casting injects metal into a hardened steel die at high speed and pressure. That means:
- Metal must flow quickly through thin sections without freezing.
- The die must open in a single direction (plus any slides).
- The part must shrink away from one half and then be pushed off by ejector pins.
So the core question is:
“Can this 3D model be filled, solidified and ejected consistently and economically?”
Everything else in this guide is just a more detailed version of that question.
Parting Line Design for Aluminum Die Casting Parts
The parting line is where the two main die halves meet. It decides:
- Which side of the part gets ejector pins.
- Where flash and potential mismatch will appear.
- How many slides or lifters are needed for side features.
Good design practices
- Try to place the main parting line where:
- It follows natural edges or steps in your geometry.
- Any small mismatch or flash can be hidden or easily trimmed.
- Avoid parting lines:
- Across sealing faces or critical cosmetic areas.
- Through small holes or thin features that are hard to clean.
Designer’s tip
When you send out your model, you don’t have to specify the exact parting line – but you can mark preferred cosmetic “A-surfaces” and sealing faces. A good die designer will then propose parting line options that protect those regions.
Recommended Wall Thickness in Aluminum Die Casting Design
Wall thickness drives:
- Fill behavior and risk of short shots
- Porosity and shrinkage
- Cooling rate and dimensional stability
- Part weight and cycle time
For many aluminum die cast housings and brackets, a baseline wall around 2.5–4.5 mm works well.
Guidelines
- Pick a target wall range early and stick close to it.
- Keep transitions between thin and thick areas gradual: taper or step over distance, don’t jump from 2 mm to 8 mm in one step.
- Where you need stiffness, use ribs and gussets instead of solid masses.
What to avoid
- Isolated “lumps” of metal: heavy pads or bosses sitting on thin walls.
- Large areas of very thick sections – better to split them or hollow them out with cores.
These regions cool slowly, creating shrinkage porosity and sink marks that later show up under machining or finishing.
Draft Angle Guidelines for High-Pressure Die Casting
Draft is the slight taper that allows the part to slide off the steel cavity and core.
Typical starting values
- Most walls: 1–3° draft
- Deep ribs, textured surfaces or heavily polished areas: 2–5°
- Inside walls may tolerate slightly less; outside walls often need more
Design tips
- Add draft in the direction of die opening.
- Apply draft consistently along the whole depth of a feature.
- Don’t forget: ribs, bosses, pockets, and windows need draft too, not just outside walls.
What happens without enough draft?
- Parts drag on the die, causing scratches, tears and sticking.
- Ejection forces rise, so pins leave deeper marks and the risk of part deformation increases.
- Tool wear and maintenance costs rise sharply.
Adding 1–2° more draft is almost always cheaper than fighting a “zero-draft” design in production.
Fillet Radius and Corner Design in Die Cast Aluminum Parts
Sharp internal corners are bad for both parts and tools:
- They create stress concentration and crack initiation points.
- They are hard to fill and cool uniformly, leading to hot spots and porosity.
- They cause thermal fatigue in the die steel.
Practical rules of thumb
- Avoid 0 mm radii almost everywhere.
- Use at least 0.5–1.0 mm radius as a minimum.
- Between thick sections and walls, aim for larger fillets when possible (e.g. 1.5–3.0 mm).
- Blend wall intersections smoothly rather than using sharp “T” joints.
Corner design
- External corners can often accept larger radii without affecting assembly.
- If a very sharp outside corner is needed for fit, consider:
- Cast with a radius, then machine the sharp edge only where required.
Ribs and Gussets in Aluminum Casting Design for Stiffness
Ribs and gussets are your main tools to improve stiffness without making walls too thick.
Rib sizing
- Rib thickness ≈ 0.5–0.7 × the adjoining wall thickness.
- Rib height ≈ 2–3 × wall thickness as a starting point.
- Add fillets where ribs meet walls, both for flow and strength.
Layout tips
- Use several smaller ribs instead of one massive rib.
- Align rib direction with metal flow if possible, to reduce trapped air.
- Avoid crossing too many ribs in one point, which creates heavy intersections and shrinkage risk.
Done well, ribs let you reduce global wall thickness (saving weight and cost) while maintaining stiffness.
Bosses, Mounting Feet and Fastener Design in Die Casting
Bosses are common for screws, inserts and stand-offs, but solid bosses can easily become porosity hotspots.
Better boss design
- Make bosses hollow where possible, with a core defining the inner hole.
- Boss outer diameter and base thickness should not exceed about 1.5–2 × wall thickness unless supported by ribs.
- Add ribs from the boss to nearby walls to support load and help flow.
- Fillet the transition between boss and wall generously.
Threaded inserts and tapping
- If you need strong threads in aluminum die castings:
- Consider threaded inserts installed after casting, or
- Specify post-machined threads and leave enough machining allowance.
This avoids relying on as-cast fine threads that are difficult to control.
Holes, Windows, Undercuts and Cores in Die Casting Design
Through holes and pockets
- Add draft to any hole or pocket formed by a core – just like walls.
- Keep distance from edge to hole at least 1.5 × wall thickness to avoid cracking and fill problems.
- For deep holes, follow a reasonable depth/diameter ratio; extremely deep, narrow holes are better drilled after casting.
Windows and slots
- Large openings can disrupt metal flow. Use flow guides or adjust gate position in cooperation with your supplier.
- Avoid thin “fingers” of metal between windows; support them with ribs or thicken them slightly.
Undercuts and side cores
Every undercut that cannot be formed by the main die requires:
- A slide (moving core), or
- A loose insert, or
- Secondary machining
Slides and loose cores:
- Increase tool cost and complexity
- Add wear items that need maintenance
- Can limit cycle time
Whenever you sketch an undercut, ask yourself:
“Can I redesign this feature so that it opens in the main die direction, or can I replace it with machining on a small area only?”
Often a small design compromise drastically simplifies tooling.
Machining Allowances, Datums and Tolerances in Die Cast Parts
No matter how good the casting, some features are best machined:
- Critical bores and bearing seats
- Sealing surfaces and precision gasket grooves
- Tight hole patterns for assembly
As-cast vs machined drawing
- Clearly mark which dimensions are “as-cast” and which are “machined after casting”.
- For machined features, allow 0.3–0.6 mm stock for cleanup, depending on part size and process capability.
- Define a logical datum structure:
- Start from cast features that are well controlled and easy to fixture.
- Reference machined features from those datums consistently.
Tolerance realism
- Expect general as-cast dimensions around ±0.10–0.30 mm for small features, increasing with size.
- Reserve ±0.01–0.02 mm for machined bores or critical dimensions only – and be prepared to pay for the extra process control.
The fewer ultra-tight dimensions you specify, the easier it is to keep both cost and quality under control.
Surface Finish, Cosmetic Areas and Die Casting Defects
Aluminum die castings can be supplied:
- As-cast with shot-blast texture
- Machined plus shot-blast
- Powder coated, painted, anodized, plated, etc.
Design tips for appearance
- Identify cosmetic “A-surfaces” on the 3D model.
- Avoid placing ejector pins, parting lines and overflows on those surfaces if possible.
- For high-end cosmetic finishes, specify realistic surface roughness (Ra) and discuss with your supplier how it will be achieved (polish, blasting, coatings).
Remember: finishing can hide some casting defects but also reveal others. For example, anodizing shows every tiny flow line and porosity much more than paint.
Aluminum Die Casting DFM Checklist Before Tooling Release
Before you send your aluminum part for die casting quotes, go through this quick checklist:
- Wall thickness
- Have I chosen a practical baseline wall and avoided extreme thick/thin jumps?
- Draft
- Does every wall, rib, boss and pocket have enough draft in the opening direction?
- Fillets & radii
- Have I removed all unnecessary sharp internal corners?
- Ribs & bosses
- Am I using ribs instead of heavy sections, and are bosses hollow and supported?
- Parting line & cosmetic zones
- Are my critical sealing faces and visible surfaces marked, so parting line and ejectors can be planned away from them?
- Machined vs as-cast features
- Which dimensions must be machined, and do I allow sufficient machining stock?
- RFQ information
- Do my drawings and RFQ clearly state alloy, annual volume, finish, and any pressure or mechanical test requirements?
If you can answer “yes” to most of these, you’re already far ahead of many first-time die casting designs.
Working with an Aluminum Die Casting Design Manufacturer
At Yongzhu Casting, we don’t just pour metal into a die; we start with design for manufacturability:
- Reviewing your 3D model for wall thickness, draft, ribs and undercuts
- Proposing parting line and gate locations that protect cosmetic and functional areas
- Planning CNC machining only where it adds real value
- Balancing tooling cost, part price and quality for your target volume
If you are developing a new aluminum part or considering converting a machined part to die casting, you’re welcome to send us your models and drawings. Our engineers can give you design-for-die-casting feedback and a quotation, so you can see how design changes might reduce tooling risk and piece price before you commit.
FAQ
Q1. What is a realistic minimum wall thickness for aluminum die casting?
A: In high-pressure aluminum die casting, many suppliers can fill local sections down to about 1.5–2.0 mm, but this is only safe for short distances and with very good gating. For general structural walls, a more reliable range is 2.5–4.0 mm, especially on larger housings. Thinner walls increase the risk of short shots, cold shuts and warpage, and often require larger machines and tighter process windows, which can raise cost instead of lowering it.
Q2. How should I choose draft angles for different surfaces on an aluminum die cast part?
A: As a starting point, you can use about 1° draft per 25 mm of depth on smooth internal walls and 1.5–2° on external walls. Deep ribs, textured surfaces, and areas around heavy bosses typically need 2–3° or more to eject cleanly. Core pins forming small holes can sometimes use slightly less draft, but then require stricter die temperature control and maintenance. It is usually better to add an extra degree of draft than to fight sticking and die wear in production.
Q3. Can I reuse a sand casting or machining design directly for aluminum die casting?
A: It is rare that a sand casting or fully machined design can be copied 1:1 for high-pressure die casting. Sand castings usually have much thicker walls and fewer restrictions on undercuts, while machined-from-solid parts often ignore draft angles and ejection directions. When converting, expect to adjust wall thickness, draft, fillets, parting line and rib layouts. A short DFM review with the die caster typically reveals several features that should be simplified or hollowed out to avoid expensive slides and heavy sections.
Q4. When is it worth using slides or lifters instead of redesigning the part to avoid undercuts?
A: Slides and lifters are justified when an undercut feature is essential for product function or assembly and cannot be realistically achieved by machining after casting. Typical examples include locking details, complex clip features, or internal grooves that must be formed during casting. However, each slide adds cost, maintenance and potential cycle time. As a rule of thumb, if a local undercut could be replaced by a simple secondary machining operation on a small area, that is usually cheaper and more robust than adding another slide to the die.
Q5. How early should I involve the die casting supplier in my aluminum part design?
A: Ideally, you should involve the die caster once the basic geometry is 60–80% defined, before you freeze wall thicknesses, ribs and cosmetic surfaces. At that stage, changing draft angles, parting line candidates or rib layouts is still relatively cheap. If you only invite feedback after the design is fully released and all marketing images are built, even small changes to improve castability can become politically difficult inside your organization.
Q6. How do I balance design freedom with tool cost when creating an aluminum die cast part?
A: Start by listing which features truly drive function and brand value—for example, sealing surfaces, connector zones, or key visual elements. Treat these as fixed. Then look for areas where geometry is mainly aesthetic or oversized for strength; these zones are good candidates to simplify walls, reduce slides, or add draft and fillets. A good rule is that every special feature should either support function or save cost. If a detail makes the die significantly more complex without clear functional benefit, it is usually better to remove or simplify it.
