Answers › Draft angle

What is draft angle, and how much does my molded part need?

Draft is a slight taper on the walls that run in the mold's pull direction, so the part releases cleanly instead of gripping the tool. Nearly every injection-molded part needs some. A common rule of thumb is about 1–2° per side — more on deep or textured walls, less on shallow smooth ones.

Why parts need draft

As the plastic cools it shrinks tightly onto the steel of the mold. If the walls are perfectly straight up and down, the part grips the tool and resists ejection — which can scratch surfaces, deform the part, or stall the cycle. A small taper (the draft) breaks that grip so the part slides off cleanly every time. It's one of the most common things missed in a first design, and one of the cheapest to fix in CAD before the tool is cut.

How much draft (rules of thumb — confirm for your part)

How little you actually give up: draft costs almost no geometry. One degree over a 50 mm-tall wall only tapers it by roughly 0.9 mm top to bottom — a change most parts never notice, in exchange for clean release every cycle. These are starting points, not specifications — the right number depends on depth, finish, and resin. (The DFM checklist covers draft alongside wall thickness and undercuts.)

Which surfaces need it

The faces that run along the pull direction — the vertical walls as the mold opens — need draft. Surfaces perpendicular to the pull (the top and bottom) don't. One nuance worth knowing: as the part shrinks it grips the core (the inside walls) hardest, so inside walls often need more draft than the outside ones. Ribs and bosses that run in the pull direction need it too. The quickest check is a draft analysis in CAD run against the pull direction: any face with zero or negative draft lights up.

What too little draft looks like — and what to do when you can't add it

The symptom is drag or scuff marks down the pull-direction faces, harder ejection that can mark or deform the part, and a slower or stalling cycle. If a feature genuinely can't take draft (a straight-sided or undercut detail), it can still be molded — but it needs a tooling solution that costs more: a shut-off or sliding core where the steel meets to form the face, or an extra moving piece (a side-action or lifter), or a redesign that removes the need. Adding draft in CAD is free; discovering you need a side-action after the tool is cut is not — so add draft wherever you can first.

Draft and texture: the trade nobody warns you about

The single biggest surprise on draft is that a textured surface needs far more of it than a smooth one. A polished wall releases with about half a degree to a degree of draft; the moment you add a grain or a bead-blast finish, the texture bites into the steel like tiny barbs and the part cannot slide off until the draft clears the depth of that texture. The working rule in texture-supplier guides is roughly 1 to 1.5 degrees of extra draft for every 0.001 inch (about 0.025 mm) of texture depth, on top of the base draft. A leather grain 0.004 in (0.1 mm) deep therefore asks for roughly 5 to 7 degrees where a smooth face would have needed one; Protolabs asks for 5 degrees or more even on a medium bead-blast texture (PM-T2). Decide the texture before you freeze the draft, because discovering it after the tool is cut means drag marks, scuffing, or a part that will not eject cleanly.

How draft actually interacts with shrinkage

Draft works with you on the cavity side and against you on the core side, and knowing which is which explains a lot of ejection trouble. As the part cools it shrinks ONTO the core (the male side) and AWAY from the cavity (the female side). So the core is where the grip is, and the core is where draft matters most — too little core draft and the part clamps on and needs high ejection force, leaving push marks or stress whitening. Cavity draft is more forgiving because shrinkage is already pulling the part loose there. If you have to be generous with draft somewhere and stingy somewhere else, be generous on the core.

The geometry: how much a degree costs you

Draft is not free dimensionally — it tapers the wall, so a tall feature with a lot of draft is thicker at the base than the tip. The offset is simple trigonometry: the wall moves in (or out) by depth times the tangent of the draft angle, so a 40 mm tall rib at 2 degrees tapers about 1.4 mm across its height. On a deep, thin feature that taper can eat your wall or your clearance, which is the real reason draft is a balancing act rather than "more is always better". Our draft angle calculator does this offset for you so you can see the dimensional cost before you commit, and the ejection force estimator shows how draft cuts the force needed to push the part off the core.

When you genuinely cannot add draft

Some features have to be straight — a sealing face, a press-fit bore, a sliding interface. When the function forbids draft, the answer is a tool mechanism, not a prayer. A straight internal feature usually needs the core built as a separate insert with its own fine finish and sometimes its own ejection; a straight external feature may need a side-action, a lifter or a collapsible core. These add tool cost and cycle time, so the honest design move is to ask early whether the zero-draft feature truly has to be zero-draft, or whether a half-degree that the function can tolerate would let you avoid the mechanism entirely. That conversation, held before the tool is designed, is where the money is saved.

From the mould review

The quickest draft check on a model is to colour the faces by pull direction and look for anything red that is vertical or undercut — those are the faces that will drag. We run that check as part of the design-for-manufacture review and flag the texture-versus-draft conflicts before steel is cut, because a draft problem found on a CAD screen costs nothing and the same problem found on a T1 sample costs a tool rework. The numbers here are rules of thumb; the final draft is set against your exact resin, texture spec and feature depth in the mould review.

Common questions

What is draft angle? A slight taper on pull-direction walls so a molded part releases cleanly from the tool.

How much does a part need? ~1–2° per side typical (ribs/bosses ~0.5–1°), ~0.5° minimum on shallow smooth walls, ~1–1.5° extra per 0.001″ of texture depth — and it costs little geometry: 1° over a 50 mm wall tapers it only ~0.9 mm (rules of thumb).

Which surfaces? The faces running along the pull direction (vertical walls, ribs, bosses) — not the top/bottom; inside/core walls grip hardest and often need more draft than outside walls.

What if there's too little? Drag marks, hard ejection, slow cycle — fix it in CAD before tooling.

Can't add draft to a feature? It needs a side-action/lifter (extra tooling cost) or a redesign; add draft where you can first.

JCH Design & Manufacturing can review your part for draft along with wall thickness, radii, and undercuts, and propose the right taper in the right places before any steel is cut. Send your part or drawing; NDA first.

Book a 30-minute call