Guide
What draft angle does a die casting need on walls, holes and ribs?
In die casting, the draft angle is the taper built into every surface that runs parallel to the direction the die opens, so the solidified part can be pulled off the die steel without dragging, galling or sticking. How much draft a surface needs is not one number: it depends on whether the surface is an outside wall, an inside wall or a cored hole, how deep it is, and which alloy is cast.
By Saola Manufacturing engineering team · Published · Updated
This guide is for design engineers and sourcing managers who have to put a draft callout on a casting drawing, or who have received a design-for-manufacturing comment asking for more of it. It explains why different surfaces need different amounts, what the published guidance says for zinc, how aluminum differs, how much a given angle moves a dimension, and how to write draft on the drawing so a die caster anywhere reads it the same way. Paid standards are named, not quoted. Where no free primary source gives a number, the page says so instead of repeating figures that circulate without a basis.
On this page
Which surfaces of a die casting need draft?
Every cast surface parallel to the die-opening direction needs draft, including outside walls, inside walls, cored holes, ribs and bosses. Surfaces square to the opening direction, such as a flat face on the parting plane, do not.
NADCA’s design guidance defines draft as the taper given to cores and other parts of the die cavity so the casting can be ejected, and states that the required angle varies with the type of wall, the depth of the surface and the alloy (NADCA, draft). That definition has a practical consequence for the drawing: draft is tied to a direction, so nobody can judge whether a surface has enough of it until the parting line and the pull direction are known.
Side cores and slides change the picture. A hole or pocket formed by a slide that moves sideways is drafted along the slide’s own direction of travel, not the main die opening. If the part has undercuts, settle with the die caster which features come from slides before the drawing is frozen, because moving a feature from the fixed steel to a slide changes both its draft and the cost of the die.
Surfaces that the design does not care about are the easy ones. Give them generous draft and leave the die caster room to add more where ejection is marginal. The work goes into the few surfaces that locate, seal or mate with something, because those are where draft and function collide.
Why do holes and inside walls need more draft than outside walls?
Because the casting shrinks as it cools. Metal shrinks away from the steel that forms an outside wall, but it shrinks onto the core pins and die inserts that form holes and inside walls, gripping them tightly.
NADCA ranks the three cases in that order: holes need the most draft, inside walls need less, and outside walls need the least (NADCA, draft). Its guidance on holes and windows adds that the perimeter of a window grips the die steel in the same way, and that these features need more draft than any other die-cast feature (NADCA, holes and windows).
The same logic explains two things engineers often find surprising. First, a hole deep in a heavy section is harder to eject than the same hole in a thin wall, because more metal is shrinking around the pin. Second, adding a hole to a part can make the whole casting harder to release, since every cored feature adds grip. When a draft comment comes back from a die caster, it almost always concerns holes, windows and deep inside pockets rather than the outer skin.
Depth matters too. The deeper the surface, the longer the stroke over which the casting is dragged along the steel, which is why NADCA treats depth as one of the inputs to the draft a surface needs. The NADCA Product Specification Standards give the calculation itself; they are a paid manual and this page does not reproduce its constants.
How much draft does zinc need compared with aluminum?
Zinc needs less draft than aluminum. The International Zinc Association gives a normal minimum of 1° on internal walls and 0.5° on external walls for zinc die castings, while NADCA’s alloy guidance lists zinc, not aluminum, among the alloys that can often be cast with zero draft.
The table sets the ranking from NADCA beside the zinc figures published by the International Zinc Association (IZA). No aluminum column is shown, because no free primary source we have read publishes aluminum draft values in a form that can be quoted.
| Surface | Why it grips or releases | NADCA ranking | Zinc minimum (IZA) |
|---|---|---|---|
| Outside wall | Casting shrinks away from the steel | Least draft | 0.5° |
| Inside wall | Casting shrinks onto the steel | More than outside walls | 1° |
| Cored hole or window | Casting shrinks around the core pin | Most draft | 0.1° listed for round holes (see note) |
| Shallow rib | Short, thin feature that sticks in the die | Not ranked separately | 5–10° |
| Critical feature | Function needs a straight surface | Zero draft often possible in zinc | 0° in some cases, from the moving die half |
Read the hole row with care. The IZA design rules list 0.1° for round holes, which looks at odds with NADCA’s point that holes need the most draft (IZA, design rules). The two statements measure different things: one is a floor for small round cores in zinc, the other is a ranking of how hard each feature grips. Do not design a hole to the lowest number in the table without the die caster’s agreement, and treat any single figure as a starting point for that conversation.
On aluminum, NADCA’s alloy selection guidance notes that zinc, ZA and magnesium alloys can often hold precision features such as zero draft as cast, which would otherwise need finish machining (NADCA, alloy selection). Aluminum is not on that list, so do not carry the zinc figures over to an aluminum part; take the values from the NADCA standards or from the die caster’s review. The ADC12 vs A380 guide covers the aluminum grades most often quoted from Asia.
How much does a draft angle change a dimension over the depth of a wall?
The offset on each side is the wall depth multiplied by the tangent of the draft angle. A wall drafted at one degree moves sideways by a little under one-fiftieth of its depth, and the table below works this out for common depths and angles.
| Wall depth | 0.5° | 1° | 2° | 3° |
|---|---|---|---|---|
| 10 mm | 0.087 | 0.175 | 0.349 | 0.524 |
| 25 mm | 0.218 | 0.436 | 0.873 | 1.310 |
| 50 mm | 0.436 | 0.873 | 1.746 | 2.620 |
A diameter changes by twice the per-side figure, because both sides of a bore or boss are drafted. That is the number to compare with the tolerance. Per ISO 2768-1 Table 1, the medium-class band for a size over 6 up to 30 mm is 0.4 mm wide in total, yet a 20 mm bore cored 25 mm deep at 1° changes diameter by about 0.87 mm from one end to the other, more than twice that whole general tolerance band. The drawing therefore has to say where the size applies, or the part cannot be accepted or rejected consistently.
For inch drawings, the same factors apply: tan 1° is about 0.0175, so a surface one inch deep at 1° typically moves a little under 0.018 in per side. The tolerance guide explains how the ISO and NADCA tolerance systems are called out alongside it.
How should draft be shown on a casting drawing?
State the draft once in a general note, override it only on the surfaces that need something different, and say for every toleranced drafted feature whether the size applies at the large end, the small end or the midpoint of the taper.
In the US, the companion standard for these drawings is ASME Y14.8-2022, Castings, Forgings, and Molded Parts, which builds on ASME Y14.5 for the conventions cast parts need. Whichever edition your drawings follow, a draft callout that a die caster abroad can price without questions answers four things:
- The pull direction. Show the parting line and the die-opening direction, or at least an arrow for it, so “draft” has a reference.
- Add or remove material. Say whether draft is added to the nominal geometry (walls get thicker toward the base) or taken from it (walls get thinner). The two readings move the part in opposite directions.
- Where the size applies. For a bore, a boss or a slot, name the end of the taper at which the dimension is measured. A mating pin usually cares about the small end of a cored hole.
- Exceptions by feature. Mark any zero-draft or reduced-draft surface individually, instead of lowering the general note for the whole part.
If the 3D model is the master, build the draft into the model and say so in a note. A model drawn with straight walls, sent with a note asking the die caster to add draft, forces a second model and a second round of approval. For datum targets that land on drafted surfaces, refer to ASME Y14.8, the drawing standard for castings and forgings. The RFQ preparation guide covers the rest of the package to send before quoting.
When is zero draft worth it, and when should you cast with draft and machine straight?
Zero draft is worth asking for on a few critical zinc features where it removes a machining step. For aluminum, and for any feature that needs a true cylinder or a tight fit over its full depth, casting with draft and machining the surface straight is usually the more predictable route.
The IZA design rules state that 0° can be reliably achieved on some critical features, at some increase in cost that is usually outweighed by the machining it saves, and that such features must be formed in the moving die half or by moving die members, with square ejection so the casting does not stick (IZA, design rules). For through holes in zinc, the IZA also describes ballizing, forcing a polished carbide ball through the hole to remove slight taper without cutting, while noting that it cannot correct straightness or alignment the way reaming can (IZA, ballizing).
Casting with draft and machining straight is the default for bearing bores, seal bores, dowel holes and any face that locates the part in an assembly. The cast surface keeps its normal draft, so the die releases cleanly, and a milling or turning operation brings the feature to size. Leave stock for the draft offset from the table above plus the usual clean-up allowance, and remember that the IZA warns against removing so much material that any porosity in the casting is exposed.
A simple test helps decide. If the feature would be machined anyway for size or finish, give it normal draft and let the machining do the rest. If the feature could be used as cast apart from its taper, and the alloy is zinc, zero draft may remove an operation, and it is worth asking the die caster to confirm it on that specific feature.
What should you ask a die caster about draft before tooling?
Ask for a draft review marked on your model, feature by feature, before the die design is released. It is the cheapest point to change draft, since after the steel is cut every change means reworking the die.
This matters more when the die caster is overseas, in Vietnam or elsewhere, and the conversation runs by email across time zones. A few items keep the review short:
- Send the parting line and pull direction you assumed, even as a sketch, so the review starts from your intent.
- List the surfaces where draft is not acceptable and why: a seal, a press fit, a cosmetic face.
- Say which faces will be machined after casting, since those can carry normal draft.
- Name the alloy by standard, because the draft that works in Zamak 3 will not work in an aluminum grade such as ADC12.
The alloys Saola sources from its partner foundries are ADC12 aluminum and Zamak 3 zinc, and the die casting page describes the part families. To have a drawing reviewed for draft along with the price, send it for a quote with the critical surfaces marked; draft comments come back as part of the reply.
Frequently asked
Is there one standard draft angle for die casting?
No. NADCA’s guidance states that the required draft varies with the type of surface, its depth and the alloy. A single blanket figure on a drawing is either wasteful on outside walls or too little on holes.
Do textured surfaces need more draft?
Yes. A texture on a wall parallel to the pull direction acts like a series of small undercuts and drags on ejection, so textured walls need more draft than smooth ones. Ask the die caster or the texture supplier for the value that matches the texture depth you specify.
Can draft be added after the die is built?
Adding draft to a surface means removing steel from a cavity or grinding a core, which is sometimes possible and sometimes not. Removing draft means adding steel, which is much harder. Settle draft on the model before the die design is approved.
Does draft affect the weight of the part?
It can. If draft is added to the nominal walls, the part gets slightly heavier and deep walls get thicker at the base, which can create heavy sections prone to shrinkage porosity. Say on the drawing whether draft adds or removes material.
Should the draft angle be on a drawing sent for a quote?
Yes, as a general note plus any exceptions. A drawing with no draft note gets a quote based on assumptions, and the differences only surface in the first-article inspection.
Sources
- Draft design guidance, NADCA Design, North American Die Casting Association, accessed September 2026
- Holes and windows design guidance, NADCA Design, accessed September 2026
- Alloy selection, NADCA Design, accessed September 2026
- Product Specification Standards for Die Castings, NADCA, accessed September 2026 (paid manual, not quoted)
- Zinc die casting design rules, International Zinc Association, 2019 web edition
- Bore sizing (ballizing), International Zinc Association, 2019 web edition
- ASME Y14.8-2022, Castings, Forgings, and Molded Parts, ASME, 2022
- ISO 2768-1:1989, General tolerances for linear and angular dimensions, ISO, 1989 (reviewed and confirmed 2022)