What draft angle do injection molded parts need?

The short answer

What draft actually does during ejection

A cooling part shrinks. On the male side of the tool, the core, it shrinks onto the steel and grips it; on the female side, the cavity, it pulls away. That asymmetry is the whole reason draft is not a cosmetic detail. With a vertical wall the part stays in contact with the core for the entire ejection stroke, so the ejector pins have to overcome friction over the full depth of the part. With 1 to 2 degrees of taper the wall separates from the steel within roughly the first tenth of a millimetre of travel, and the rest of the stroke runs with clearance.

The consequences of getting it wrong are visible before they are dimensional. Drag marks and scuffing appear on the wall, the surface stress-whitens where the plastic was stretched, ejector pins leave a witness ring or punch through a thin floor, and the part distorts as it leaves. On a textured face the damage is worse, because the texture acts as a field of micro-undercuts and a dragging part shears the grain off the tool. The repair is not a process tweak: it means re-machining or re-texturing steel.

Draft is measured from the direction of pull, not from the parting line, and it is always quoted per side. That convention matters when a wall has draft on both faces: a 1 degree per side taper on a 4 mm wall closes the section by about 0.14 mm over 4 mm of depth, and a supplier quoting "1 degree total" is describing half of what the design needs.

The baseline by surface condition

Start from the finish, not from the resin. A polished cavity releases easily and 1 degree per side is a workable minimum for shallow parts in stable engineering resins, with 2 degrees the safer default for anything with depth. A fine matte or light etch needs 1.5 to 2 degrees. A medium leather or sand grain needs 2 to 3 degrees. A heavy grain or deep chemical etch needs 3 to 5 degrees, and the deepest patterns run beyond that. Ribs and bosses are the exception in the other direction: they are narrow, they grip the core hard, and 0.5 to 1 degree per side is the accepted minimum, with the taper running from the base toward the tip on core-side features.

The table is the number most designers never calculate: the side offset the draft consumes at the far end of the feature. It is plain trigonometry, offset equals depth multiplied by the tangent of the angle, and it explains why deep ribs and tall bosses run out of material at the tip. A cosmetic wall that is 2.4 mm at the parting line with 1.5 degrees of draft over 50 mm is 0.9 mm thinner at the other end, which is no longer the wall that was analysed. If a feature has to stay thick at the tip, either reduce its depth or accept less draft and pay for it in ejection.

Texture is the largest single adder

The industry rule is to add 1 to 1.5 degrees of draft for every 0.025 mm, or 0.001 inch, of texture depth. Typical moulded-in grains are 0.06 to 0.08 mm deep, so the adder works out at 2.5 to 3.75 degrees on top of whatever the smooth face needed. A face that would have run at 1 degree polished therefore lands at 3.5 to 4.75 degrees once it is grained. A deeper industrial pattern at 0.1 mm would add 4 to 6 degrees by the same arithmetic, which is why heavy textures and tight wall positions fight each other.

Two practical consequences follow. First, the texture specification has to be settled before the tool is cut, because the draft that the grain requires changes wall positions, rib tips and mating faces. Adding a grain after the tool exists usually means re-cutting walls or accepting a drag mark. Second, the texture supplier and the mould maker should see the same number: the depth in the texture standard, not the pattern name. A pattern quoted as "medium leather" by one supplier is not necessarily the same depth as another's.

Core side, ribs and shut-offs carry different numbers

Because the part shrinks onto the core, core-side faces need more draft than cavity-side faces at the same texture. The working adjustment is 0.5 to 1 degree extra on core-side features beyond the cavity baseline, and more on deep cores where cooling shrinks the part tighter. Cored holes deserve their own rule: a perfectly cylindrical core will grip the part, so 0.5 degree per side is the practical minimum even when the surrounding wall has 2 degrees.

Shut-off faces are a separate case again. Where cavity and core steel meet metal-on-metal to blank off a hole or an opening, the faces slide against each other under clamp pressure. A 1 degree angle is too shallow here and will gall, wear and eventually flash, so 3 degrees is the usual minimum. Ribs and bosses take 0.5 to 1 degree per side, with the draft measured base to tip on core-side features and tip to base on cavity-side ones; getting that direction wrong creates an undercut that a slide then has to solve.

Depth changes the answer more than material does

Resin choice matters less than most design guides imply. Soft unfilled grades such as PP and PE release more easily and tolerate the low end of each band; rigid and filled grades such as PC, ABS and glass-filled nylon grip harder and need the middle or top. But a 5 mm deep feature in the easiest resin still needs less draft than a 100 mm deep one in the most difficult, because the contact area and the shrink grip both scale with depth. Depth is the variable to check first.

The usual correction for a deep draw is not more draft on the whole part, which would move every wall, but a local increase: steeper taper on the deep feature only, a polish in the draw direction to cut friction, or a redesign that splits the depth. On cores forming deep pockets, additional draft plus better core cooling, which reduces shrink grip, does more than another half degree of taper alone.

When a face has to stay vertical

Some faces genuinely cannot be tapered: a sealing land, a mating face that must sit square against another part, an optical window, a bore that takes a bearing. Moulding them at zero draft is possible and it is not free. The tool then needs draw-direction polishing, tighter steel tolerances, often a sleeve ejector rather than pins, air poppet valves to break the vacuum, or extra wall thickness so the shrink grip is lower. Every one of those is a line in the tooling quote, and a face marked "must stay vertical" without a reason will be priced conservatively because the supplier has to assume the worst.

There is one more option worth knowing: stripping. A small undercut or a zero-draft lip can sometimes be forced off the core by the flexibility of the resin itself, which avoids a slide. That works on unfilled, ductile grades for features up to roughly 2 to 3 percent of the part diameter, provided the edge is rounded. It does not work on polycarbonate or glass-filled nylon, which are too stiff and will crack or whitening instead.

How to put it on the drawing

Write the default, then write the exceptions. A single note such as "all vertical faces 1.5 degrees per side unless dimensioned otherwise" gives the toolmaker a baseline, and marking the faces that must stay vertical, with the functional reason beside them, prevents a late argument. Give the texture standard and its depth on the same drawing rather than in a separate cosmetic document, because the draft requirement depends on it.

Two habits avoid the common failures. Do not dimension across a drafted face as though it were parallel; give the dimension at a stated plane, usually the parting line. And check both halves of the tool: a wall drafted correctly on the cavity side but left vertical on the core side will still drag, and it is the core side that the part is gripping.

This answer covers the number to put on a drawing. The cost side of the same decisions, which design changes actually move the piece price, is set out in injection moulding, and the parts that come out of those tools are listed under plastic injection moulding. Where a wall or a feature cannot be moulded as drawn, CNC machining is the usual bridge for the first articles.