Injection Molding Draft Angle Guide: How Much Draft Do You Need?
Draft angle is one of the least glamorous decisions in part design and one of the most consequential. Get it right and your parts release cleanly, cycle times stay short, and the tool runs for its full rated life. Get it wrong and you inherit drag marks, sticking, distorted parts, and a mold that needs constant intervention — problems that only get more expensive the longer they go undiagnosed.
In this guide
- What Draft Angle Actually Does
- The Baseline Numbers
- Texture Changes Everything
- Depth, and Why Cavity and Core Differ
- Ribs, Bosses, and Other Features
- What Insufficient Draft Actually Costs You
The frustrating part is that draft costs nothing to add at the design stage and a great deal to add later. Once steel is cut, adding draft means welding and re-machining cavities, or in the worst cases rebuilding inserts. This guide covers how much draft you actually need, why material and texture change the answer, and how to catch draft problems before tooling begins.
What Draft Angle Actually Does
Draft is a slight taper applied to any surface that runs parallel to the direction the mold opens. Instead of a perfectly vertical wall, the wall leans by half a degree, one degree, or more. The taper means that the moment the mold begins to open, the part breaks free of the steel rather than sliding against it for the full depth of the draw.
The physics is straightforward. Molten plastic shrinks as it cools, and it shrinks onto the core. That shrinkage grips the steel. Without draft, the part must slide the entire depth of the wall against a surface it is actively squeezing — friction, vacuum, and adhesion all working against ejection. With adequate draft, contact is broken within the first fraction of a millimetre of mold travel, and the part is free.
Every vertical surface needs it: outer walls, inner walls, ribs, bosses, the sides of holes, and shut-off faces. The only surfaces that do not need draft are those perpendicular to the pull direction — the flat top of a boss, for example, or a parting-line face.
The Baseline Numbers
There is no single correct answer, but there are reliable starting points. These assume a smooth, untextured surface and a wall depth under about 25 mm:
0.5 to 1 degree per side — shallow parts, smooth finish, unfilled materials, and situations where the part is short and stiff enough to resist distortion. Common on small housings and cosmetic covers.
1 to 2 degrees per side — the safe general-purpose range for unfilled engineering plastics. If you have no reason to choose otherwise, specify 1.5 degrees and you will rarely be wrong.
2 to 3 degrees per side — glass-filled and mineral-filled materials. Fillers make the melt more abrasive and the part stiffer, so it grips harder and flexes less to release. PA66 with 30% glass fibre, for example, typically wants 2 to 3 degrees where unfilled PA66 is comfortable at 1.5.
0 degrees or even slight undercut — flexible materials such as TPE and soft TPU can sometimes be stripped off a core with no draft at all, because the part deforms elastically rather than the steel having to release it. This is a special case and should be confirmed with your moulder rather than assumed.
Material matters as much as geometry. ABS and PP are forgiving at around 1 degree. Polycarbonate, with its high melt viscosity and tendency to grip, prefers 1.5 to 2. POM shrinks significantly and wants 1.5 to 2. Anything reinforced wants more.
Texture Changes Everything
This is where most draft calculations go wrong. A part that moulds beautifully with 1 degree in a polished cavity can stick badly with the same 1 degree once it is textured, because texture is not a surface treatment — it is a field of microscopic undercuts.
The working rule used across the industry is roughly 1 degree of draft per 0.025 mm (0.001 inch) of texture depth, added on top of your base requirement. A light matte finish may add only half a degree. A medium grain may demand 2 to 3 degrees. A heavy leather or stipple texture can require 5 degrees or more before the part releases reliably.
Practically, that means:
A mirror or high-gloss finish is the most forgiving — 0.5 to 1 degree often suffices. A fine bead-blast or 600-grit stone finish typically wants 1.5 to 2 degrees. A visible decorative texture generally needs 3 degrees or more, and deep textures on deep draws can need beyond 5.
Decide your finish before you finalise draft, not after. We regularly see parts designed for 1 degree and then specified with a texture that needs 3, which forces either a tooling change or a compromise on appearance. If you are weighing cosmetic requirements against manufacturability, a DFM review will resolve it in a day rather than a week of email.
Depth, and Why Cavity and Core Differ
Draft requirement scales with draw depth. A 5 mm deep wall can get away with very little; a 60 mm deep box cannot. As a rough guide, once a wall exceeds 25 mm of depth, add roughly 0.5 degrees for every additional 25 mm.
It also matters which half of the tool forms the surface. As the part cools it shrinks onto the core and away from the cavity. That means core-side surfaces grip harder and need more draft than cavity-side surfaces. Outer walls formed in the cavity are comparatively forgiving; inner walls formed on the core are where sticking begins. When in doubt, add the draft on the inside.
Deep ribs are the classic offender. A 40 mm deep rib with 0.5 degrees will drag, and because ribs are thin they also cool fast and grip early. Deep ribs want 1 degree per side minimum, often more if the material is filled.
Ribs, Bosses, and Other Features
Draft applies to every feature, not just the outer walls, and these are the ones most often missed:
Ribs — 0.5 to 1 degree per side, with rib thickness kept to 50 to 60 percent of the nominal wall to avoid sink marks, and a base radius of roughly 0.25 to 0.5 times the wall thickness.
Bosses — 0.5 to 1 degree per side on the outer wall, and the same on the inner bore if it is formed by a core pin. Boss walls should be about 60 percent of the nominal wall.
Through-holes and slots — 0.5 degree minimum on the hole wall. Blind holes need it too, or the core pin will fight the part on every cycle.
Threads — avoid moulded threads where a self-tapping screw or insert will do. If threads are necessary, allow 1 to 2 degrees and expect either an unscrewing mechanism or a collapsible core, both of which add cost and maintenance.
Shut-off faces — where steel meets steel at an angle, the shutoff needs draft on both sides or the shut-off will wear and flash quickly.
The parts that get into trouble are usually not the ones with no draft at all — those are obvious in CAD. They are the ones with almost enough: 0.5 degrees where 1.5 was needed, or 1 degree on a textured core. That is enough to mould, barely, and not enough to mould reliably for a hundred thousand cycles.
What Insufficient Draft Actually Costs You
The symptoms are progressive, and they are all expensive in different ways.
First, drag marks and scuffing on the sidewalls, where the part scrapes against the steel during ejection. On a cosmetic surface this is immediate scrap.
Second, sticking and ejection force. The part stays on the core, ejection pins have to push harder, and cycle time stretches because the moulder adds cooling time or ejection dwell to compensate. A two-second penalty per cycle on a 30-second cycle is a 6 percent throughput loss, permanently.
Third, distortion. Parts ejected under excessive force warp, bow, or crack around ejector pin locations. This is often misdiagnosed as a material or cooling problem, and teams spend weeks chasing a process fix for what is fundamentally a geometry problem.
Fourth, tool wear. Repeated dragging polishes the texture off cavity walls and rounds off shut-off edges. Once texture is polished away, the cosmetic finish is gone and the insert has to be re-textured — which means the tool is out of production.
There is a common and costly mistake here: when parts stick, the instinct is to polish the cavity. Polishing in the direction of draw reduces friction temporarily but also reduces effective draft, because you are removing steel from the wall. It frequently makes the underlying problem worse over time. The correct fix is more draft, not a smoother wall.
Finding and Fixing Draft Problems Early
Every mainstream CAD package includes a draft analysis tool. Set the pull direction, set your target angle, and the software colour-maps the model — surfaces meeting the target in one colour, insufficient in another, and negative draft in a warning colour. Run it on the final model, not an early revision, and run it with the actual texture requirement in mind rather than the base angle.
Pay particular attention to surfaces you may not have considered: the inside faces of deep pockets, the flanks of snap-fits and living hinges, and any surface created by a slider or lifter. Negative draft on a slider face is a frequent late-stage surprise.
If analysis reveals insufficient draft and the design is not yet frozen, the options in order of preference are: increase the draft, reduce the texture depth, relocate the parting line, or — last and most expensive — add a side action. Slides and lifters solve the geometry but add tooling cost, maintenance burden, and a potential flash location. They are a legitimate solution, but they are not the cheap one.
This is exactly the class of issue a mold design review and mold flow analysis exist to catch, while the fix is still a CAD edit rather than a welding job.
A Practical Draft Checklist
Before you release a model for tooling, confirm the following:
You have set an explicit pull direction and run draft analysis against it. Your base draft is at least 1 degree per side on unfilled materials and 2 degrees or more on filled grades. You have added draft for texture at roughly 1 degree per 0.025 mm of texture depth. Core-side and inner surfaces have at least as much draft as cavity-side surfaces. Ribs, bosses, holes, and shut-offs all carry draft. Deep draws have been increased beyond the baseline. And your moulder has confirmed the numbers against the actual material and finish specification.
Draft is unusual among design rules in that being generous costs you almost nothing. A part with 3 degrees of draft looks and functions identically to one with 1 degree in most applications — it simply moulds better, faster, and for longer.
If you have a part you are preparing for tooling, or an existing tool that is giving you ejection trouble, send us the 3D model. We will run a draft and DFM review and tell you plainly whether your angles will hold up in production. Contact us to get started, or read more about our injection molding capabilities.
Related guides in this series
This article is part of our Mold Design & DFM Guide — a full walkthrough of the topic with the numbers and checklists behind each decision.