Injection molding is unforgiving about two things in particular: draft angles and undercuts. Get either wrong and your factory either cannot eject the part cleanly or cannot open the mold at all. Both problems are invisible in a CAD render, and neither shows up during 3D printing or CNC prototyping. They only appear when the steel tool is already cut.
This post explains what each issue is, why it happens, and which faces of your design to check before you send a STEP file for a quote.
What Is a Draft Angle?
Every wall in a straight-pull injection mold needs to taper slightly in the direction the mold opens. That taper is the draft angle, measured in degrees from vertical.
The reason is thermal. When molten plastic fills the mold and begins to cool, it shrinks. On the outside of the part, the plastic shrinks away from the cavity walls and releases naturally. On the inside — around cores, bosses, and ribs — the plastic shrinks tightly onto the steel, like a fist closing around a post. If those inner walls are perfectly vertical, the ejector pins have to drag the part straight off the steel under significant friction. The result is scratches and scuff marks called drag marks, visible on the surface of every part in the production run. In severe cases the part warps or cracks during ejection.
A slight taper — even half a degree — creates an immediate air gap the moment the mold begins to open, so the part breaks free cleanly.
The Numbers That Matter
The required draft angle depends on the surface finish of your design:
- Smooth or polished finish: The absolute minimum is 0.5 degrees per side. In practice, 1 to 2 degrees is the standard recommendation and what most moldmakers assume by default.
- Light texture (such as a fine grain pattern): At least 3 degrees per side.
- Heavy texture (deep grain or leather-like patterns): 5 degrees per side, or more.
For Mold-Tech textures and similar industry standards, the strict rule is to add 1.5 degrees of draft for every 0.001 inch (0.025 mm) of texture depth, on top of a 1-degree base. A medium grain at 0.003 inches deep would therefore require 1 + (3 × 1.5) = 5.5 degrees minimum. Miss this and the surface texture drags against the steel and scuffs during every ejection.
Which Faces Designers Commonly Miss
CAD tools make it natural to extrude walls at exactly 90 degrees. The draft gets added later — or forgotten. These are the faces most often missed:
Inner walls of bosses. Screw bosses are hollow cylinders that grip the steel core tightly during cooling. Inside surfaces require more draft than outside surfaces for exactly this reason: the shrinkage direction works against you. A common recommendation is to apply at least 1 degree inside versus 0.5 degrees outside.
Rib walls. Ribs project from the main wall in the mold-opening direction and are formed in blind holes in the steel. They need at least 0.5 degrees of draft per side. The complication: because draft tapers a rib's wall as it rises, tall ribs with too much draft become dangerously thin at the tip, which prevents the plastic from filling to the top. The standard guidance is to keep ribs no taller than approximately three times the rib-base thickness and to use the minimum draft needed for ejection.
Interior surfaces of deep pockets. Any deep interior wall grips the core harder than a shallow one. The deeper the feature, the more draft it needs to release cleanly.
Surfaces intended to carry texture. Designers sometimes add a texture specification late in the design process without revisiting the draft on those faces.
What Is an Undercut?
An undercut is any feature that sits perpendicular to the mold's opening direction — effectively a hook that wraps around the steel. In a standard straight-pull mold, two halves clamp together and then pull directly apart. If your design has a feature that goes sideways relative to that pull, the mold cannot open without physically tearing the feature off the part. This is called a die-lock.
Undercuts are not always obvious in CAD because the software has no concept of which direction a mold opens. You can model a beautiful, functional snap-fit hook in five minutes without realizing the mold cannot release it.
Features That Create Accidental Undercuts
Side holes and vent windows. Placing a hole through a vertical side wall — for a port, a speaker grille, or ventilation — creates an undercut. The mold steel forms one side of the hole, but it cannot pull straight back out. A side-action cam or bypass steel is required.
Snap-fit hooks and clips. A snap-fit hook projecting from a solid floor is a classic die-lock. The underside of the hook catches on the mold steel. The standard fix is to add a pass-through slot directly beneath the hook: this allows the two mold halves to meet through the wall and form the underside of the hook without any moving part in the mold.
Logo text and raised lettering on side walls. Every character in a logo placed on a vertical side wall protrudes horizontally. Each letter is effectively a tiny undercut. Unless a side-action pulls that wall away before ejection, the text locks the part in the mold or shears off.
O-ring grooves and threads. A groove that wraps around a cylindrical surface is a continuous undercut. External threads are the same. Releasing them requires one of the most complex mold mechanisms available — either a collapsible core that mechanically shrinks inward in segments, or a hydraulic unscrewing device that rotates a threaded core pin out of the plastic.
Lip rims and internal recesses on the inside of caps or shells. Any inward-facing ridge or dimple on the inside of a hollow part requires a lifter — an angled mechanism built inside the mold core that moves diagonally during ejection.
What Fixing Undercuts Costs
The only economical fix is to redesign the feature so it aligns with the mold's pull direction — or to add bypass steel, which requires careful geometry. When a redesign is not possible, the factory adds moving mechanisms to the mold:
- Side-action slide: Used for external undercuts like side holes. Adds tooling complexity and cost. Even the simplest core movement carries a meaningful cost premium, and machining time for the slide mechanism alone typically runs 50 to 80 hours of toolmaking.
- Internal lifter: Used for shallow internal undercuts. More difficult to build than a side-action — typically 100 to 200 hours of toolmaking.
- Unscrewing mechanism or collapsible core: Required for threads and continuous internal grooves. The most complex option, requiring 200 to 300 hours of additional toolmaking time.
All of these also increase long-term mold maintenance costs because moving parts wear and need servicing between production runs.
Why These Issues Are Hard to Catch Without a Face-by-Face Check
Both draft and undercut problems are geometry problems, not appearance problems. A part can look completely finished and functional in your CAD software and still have walls at zero degrees of draft and three die-lock features. Standard CAD tools do not highlight these conditions by default. A general review — looking at the model as a whole — tends to miss the inner wall of a boss, the base of a rib, or the underside of a clip, because those faces are not visible from the outside.
A face-by-face check examines each surface individually against the mold's pull direction, flags which specific face is below the draft threshold, and identifies which features create a locked condition and on which side of the geometry.
How Fabdose Checks Your Design
Fabdose reads your STEP file on your computer. The geometry is never uploaded to a server — your CAD files stay local. The analysis identifies which faces have insufficient draft and which features create undercuts, then generates descriptions of each issue that are processed by AI and synced to your account. For a typical product enclosure or consumer part, the check takes about a minute.
The current analysis covers injection molding with face-level specificity for draft and undercut conditions. It does not currently detect defects that require flow simulation — such as weld lines or sink marks — which depend on material, gate placement, and wall thickness ratios rather than geometry alone.
If you have a STEP file ready, you can drop it in and get a report before you send anything to a factory.