Key takeaways
- Wall thickness has to be thin enough to fill and thick enough to feed, so uniformity matters more than the nominal number.
- A rib should be thinner than the wall it meets, or it creates the sink it was added to prevent.
- Inside surfaces need more draft than outside surfaces because the casting shrinks onto the core.
- Texture, depth and machining stock all consume draft, so check the finished part, not just the model.
Wall thickness is a process number
A die casting wall has two jobs that pull in opposite directions. It has to fill before the metal freezes, which argues for a thin wall and a short flow length. It has to feed the section as it solidifies, which argues for enough thickness to avoid a shrink cavity. The design has to satisfy both at once, and the only way to do that is to keep the wall as uniform as the function allows.
A thin wall at the end of a long flow path is the classic cold shut: two flow fronts meet, lose heat and fail to weld. A thick section is the classic shrink defect: the skin forms, the centre pulls away and the surface sinks. Neither is a machining problem, and neither can be fixed by tightening the tolerance.
The nominal wall is therefore a starting point, not a specification. The drawing should show the nominal wall, the transitions and the features that are deliberately thicker, with a note on where porosity or sink is acceptable.
The working bands
For aluminium die casting, a nominal wall of 1.5 to 3 mm covers most electrical and structural parts. A small part in a well-controlled die can go to about 1 mm, and a large part with a long flow may need 3.5 mm or more to fill reliably. These are illustrative bands, and the foundry's own capability on the specific die is the real limit.
Thin walls are not automatically better. A 1 mm wall over a large area is harder to fill, harder to keep flat and harder to machine without distorting. A 2 mm wall with good ribs is often stiffer and cheaper than a 1.2 mm wall with none, because the ribs carry the stiffness and the wall only has to form the surface.
The features and their starting values
The table gathers the values that come up most often in a die casting review. Treat them as starting points, and confirm each one with the caster before the die design is released.
| Feature | Starting value | Reason | Risk if ignored |
|---|---|---|---|
| Nominal wall | 1.5 to 3 mm | Fills before freezing, feeds without a shrink cavity | Cold shut or sink |
| Rib thickness | 50 to 70% of the wall | Cools at a similar rate to the wall | Sink opposite the rib |
| Boss wall | About 50% of the wall | Avoids a local hot spot | Shrink cavity at the bore |
| Internal fillet | About half the wall | Spreads stress and flow | Stress riser and hesitation |
| Outside draft | 1 to 2 degrees | Releases the part from the cavity | Scuffing and drag marks |
| Inside draft | 1.5 to 3 degrees | Casting shrinks onto the core | Tearing and ejection force |
| Machining stock | 0.5 to 1 mm per face | Cleans up draft and distortion | Black skin or exposed porosity |
Values are typical starting points for aluminium. Deep cores, textured faces and large parts need more draft and more stock.
Transitions, ribs and the sink problem
A change of section is a change of cooling rate. A wall that steps from 2 mm to 6 mm in one face creates a hot spot at the step, a sink on the opposite face and a shrink cavity inside. The fix is a gradual transition, typically at a ratio of 3:1 or 4:1, with a fillet at the junction.
Ribs are the usual way to add stiffness without adding a thick section. A rib at 50 to 70 per cent of the wall thickness cools at a rate close to the wall, so it does not create a hot spot at the root. A rib as thick as the wall does the opposite: it feeds a shrink cavity and pulls a sink into the face it was meant to support.
Bosses follow the same logic. A solid boss is a thick section, so it sinks. A cored boss with a wall about half the nominal wall, a fillet at the base and a rib if it stands free will cool more evenly. If the boss is going to be tapped, leave enough wall for the thread and check the thread depth against the cored hole.
Draft, depth and texture
Draft is the taper that lets the casting leave the die. The minimum depends on the depth of the surface, the finish and whether the surface is on the cavity or the core. A shallow outside face can run at about 1 degree. A deep core needs more, because the casting shrinks onto it and the ejection force rises with the contact area.
Texture adds to the requirement. A textured surface is full of microscopic undercuts, and the draft has to clear them as well as the macro geometry. A common rule adds about 1 degree of draft for every 0.025 mm of texture depth, so a coarse texture can add several degrees.
The parting line and the shut-offs also need draft. A shut-off between two die faces is a metal-to-metal seal, and it needs enough angle to avoid galling. A side action or a slide adds its own draft and its own cost, so a feature that needs a slide should be challenged before it is accepted.
Draft is measured on the finished part
If the face is machined after casting, the draft has to sit in the stock. Check that the finished wall still has the thickness the design needs.
As-cast against machined
A die casting is usually a near-net shape, not a finished part. Faces that mate, seal, carry current or locate are machined. That means the as-cast surface carries draft and distortion, and the machining operation removes both. The stock must be enough to clean up the draft over the full face and the distortion over the full length.
The interaction is easy to miss. A 1.5 degree draft on a 60 mm deep wall moves the surface by about 1.6 mm from top to bottom. If the machined face runs the full depth, the stock at the bottom has to cover that movement plus the casting tolerance. A nominal 0.5 mm stock is not enough, and the machinist will either leave a black patch or take an extra pass that exposes porosity.
The drawing should distinguish the as-cast surfaces from the machined surfaces, show the stock on each machined face, and state the datum for the machining. A casting that is located on an as-cast surface for machining carries the casting tolerance into the machined part, so the locating surface often needs to be machined first.
How to check a drawing before the die is cut
Start with a section through the thickest part of the casting. Mark the nominal wall, the ribs, the bosses and the transitions. Look for any place where the section changes quickly, and check that the change is graded rather than stepped.
Then check every vertical face for draft. Include the small faces, the shut-offs and the cores. Add the texture allowance where the surface is textured, and add the machining stock where the face will be cut. Confirm that the finished part still has the wall and the draft the design needs.
Finally, check the marks. Ejector pins, gates, overflows and the parting line all need a home on a non-cosmetic, non-sealing face. If they do not have one, the drawing is asking for a second operation that has not been costed. A short review at this stage is much cheaper than a die correction after the first shot.
What to send with the model
Send the model with the parting line, the gate position if it is fixed, the ejector areas and the surfaces that must not carry a mark. Add the alloy, the annual volume and the machining plan. If the part will be machined, say which faces and how much stock is allowed.
State the wall and draft assumptions in the notes, even if the model already shows them. A supplier who can see the intent will flag the features that fall outside the process rather than quoting a correction later. If the part is still in design, ask for the wall and draft review before the tooling quote, not after.
Frequently asked questions
What is a typical wall thickness for an aluminium die casting?
Most parts run between 1.5 and 3 mm. A small part in a well-controlled die can reach about 1 mm, and a large part with a long flow may need more than 3 mm. The foundry's capability on the specific die is the real limit.
Why does an inside surface need more draft than an outside surface?
The casting shrinks onto the core as it cools, so an inside surface grips the die. More draft reduces the contact and the ejection force. An outside surface shrinks away from the cavity and needs less.
How does texture change the draft?
Texture creates microscopic undercuts, so the draft has to clear them. A common rule adds about 1 degree for every 0.025 mm of texture depth. A coarse texture can need several degrees more than a polished face.
Can a die casting be made with no draft?
Not practically. A zero-draft surface will drag, scuff or crack during ejection. Some features can be formed with a slide or a split, but the surfaces still need draft to release.
Sources and further reading
- ISO 8062-3, Geometrical product specifications for moulded parts, casting tolerances
- EN 1706, Aluminium and aluminium alloys, castings, chemical composition and mechanical properties
- Qumek engineering desk notes on die cast wall and draft reviews
Qumek Engineering Desk
Engineering team
The engineering team behind Qumek drawings, DFM notes, tolerances and inspection standards. Every guide is reviewed against the drawings and processes used on live programmes.
Want a wall and draft check before tooling?
Send the model and the machining plan. The engineering desk will reply with the sections, faces and marks that need attention before the die is cut.
Send a drawing