Draft Angle Calculator
Standard-tolerance constants from NADCA table S-4A-7. Inside walls carry twice the draft of outside walls; hole draft is the total across the diameter.
Draft is calculated by multiplying the height of the wall above the parting line by the tangent of the draft angle: an 8 in. wall at 1° leans 0.14 in. over its height. That linear offset, not the angle, is what changes a dimension, and a drawing has to settle two things about it — which end of the wall the stated dimension applies to, and how the offset stacks with machining stock and casting tolerance.
Draft Angle Formula
The draft allowance is the height of the drafted surface, measured perpendicular to the parting line, times the tangent of the draft angle.
DA = L × tan θ
DA is the linear offset between the two ends of the drafted surface, L is its height from the parting line, and θ is the draft angle. The offset applies per wall: a pocket or a slot drafted on both sides changes by 2 × L × tan θ across its width. When the clearance a feature can give up is already known — a drafted wall that has to clear a bolt pattern, say — the same relation gives the steepest angle it can afford.
θ = arctan(DA / L)
At casting draft angles the tangent behaves as a flat rate, so it is easier to carry as an offset per unit of depth than as a trig function.
| Draft angle | Offset per 1 in. of depth (in.) | Offset per 100 mm of depth (mm) |
|---|---|---|
| 0.5° | 0.0087 | 0.87 |
| 1° | 0.0175 | 1.75 |
| 1.5° | 0.0262 | 2.62 |
| 2° | 0.0349 | 3.49 |
| 3° | 0.0524 | 5.24 |
| 5° | 0.0875 | 8.75 |
Take a ductile iron gearbox housing molded no-bake, with side walls standing 8 in. above the parting line at 1°, the usual no-bake figure for most features. Each wall leans 8 × 0.0175 = 0.14 in. over its height, and a pocket between two such walls is 0.28 in. narrower at its floor than at the parting line. Whether the drawing dimension applies at the floor or at the parting line is the next section's question.
Calculating the Required Dimensional Allowance
The raw casting dimension is the finished dimension plus the required machining allowance on each machined side plus half the casting tolerance, with the draft offset stacked on top of that — never inside it. Draft goes onto the surface first, the tolerance zone is referenced from the drafted surface, and the machining stock is superimposed on both.
| Machined feature | Raw casting dimension R |
|---|---|
| One face machined | R = F + RMA + CT/2 |
| External diameter or boss, machined all round | R = F + 2 RMA + CT/2 |
| Bore or internal pocket | R = F − 2 RMA − CT/2 |
F is the dimension after final machining, RMA the required machining allowance for the casting's size and molding method, and CT the casting tolerance for the tolerance grade on the drawing. R is the dimension at one end of the drafted wall; the other end differs from it by L × tan θ.
Which end holds R is a drawing convention, not a universal rule. Under taper plus, the drawn dimension is the minimum-metal end and the draft adds metal from there; under taper minus, the drawn dimension is the maximum-metal end and the draft is taken inside it. ISO 8062-3 applies taper plus unless the drawing says otherwise, switching to taper minus only for features that carry a maximum material requirement.
On the gearbox housing above, take a bearing boss 4 in. tall, machined all round to Ø6.000 in., on a machine-molded casting whose largest dimension falls in the 16–25 in. band — required machining allowance grade G, 0.160 in. per side. The minimum-metal end must be R = 6.000 + 2(0.160) + CT/2 = 6.320 in. + CT/2. At 1° the draft across the diameter over 4 in. is 2 × 4 × 0.0175 = 0.14 in., so under taper plus the boss measures 6.46 in. + CT/2 at the parting line.
Read as taper minus, the same 6.320 in. sits at the parting line and the small end comes out at 6.18 in., leaving 0.09 in. of stock per side against the 0.160 in. the grade calls for, and the cut may not clean up. On a wall this tall the draft offset is the same order as the machining stock, so an unstated convention is not a rounding error.
Pattern shrinkage is not part of this stack. The shrink rule is applied to the pattern by the foundry; drawing dimensions are always finished-casting dimensions.
Draft Angle in Die Casting
Die casting calculates draft as a distance first and an angle second: the draft distance grows with the square root of feature depth, so the angle on the same wall falls as the feature gets deeper.
D = √L / C
D is the draft in inches, L the depth of the feature from the parting line in inches, and C a constant NADCA tabulates by alloy and by wall type — inside wall, outside wall, or hole. The angle follows from arctan(D / L) as in the first section. For an aluminum inside wall C is 30, and NADCA's own three depths show what the square root does.
| Feature depth (in.) | Draft distance (in.) | Draft angle |
|---|---|---|
| 0.1 | 0.010 | 6° |
| 1.0 | 0.033 | 1.9° |
| 5.0 | 0.075 | 0.85° |
The reason is the die. The casting has to eject from steel, and as the alloy freezes it shrinks onto the die steel that forms inside walls and holes and away from the steel that forms outside walls. NADCA therefore gives inside walls twice the draft of outside walls (C is 60 for an aluminum outside wall) and holes the most, and the familiar general note "2° minimum inside, 1° minimum outside" is NADCA's example for aluminum features at least 1 in. deep, not a rule for every alloy or depth.
In sand casting the pattern withdraws from sand rather than the casting from steel, so the angle is set per molding process, at most stepped down for taller features, and the arithmetic is the linear one above. A die-cast part converted to a ferrous sand casting is redrafted from the first section's formula with the sand process's angle; its die-casting draft note does not carry over.