Design for Manufacturability (DFM): An Injection Moulding Checklist

Most injection moulding problems aren’t moulding problems at all — they’re design decisions made months earlier, baked into the geometry long before anyone cuts steel. A wall that’s too thick sinks. A corner that’s too sharp cracks. An undercut that no one flagged turns a simple two-plate tool into an expensive one with side-actions. By the time these show up in a moulding trial, the tool exists, and fixing them means re-cutting steel.

Design for Manufacturability (DFM) is the discipline of catching all of that up front. It’s a structured review of a part’s geometry against how injection moulding actually behaves — how molten polymer flows, packs and cools inside a steel cavity — so the part is easy to mould, cheap to tool, and consistent in production. Do it well and you avoid the two most expensive words in this industry: tool modification.

This is a working checklist, written for the design engineers and procurement managers who have to sign off a part before it goes to tooling. Run your part against every section below. Where you can’t tick the box, that’s a conversation to have with your toolmaker now — not after the tool is cut. It’s the same design discipline that quietly drives injection mould tooling cost, so every box you tick here usually takes money off the quote as well.

Wall thickness and uniformity

This is the single most important thing to get right. Injection moulded parts should be shelled out to a thin, uniform wall — not designed as solid chunks of plastic. Thick sections cool slowly and unevenly, which causes sink marks, internal voids, warp and long cycle times. Uneven walls cause the material to cool at different rates, which pulls the part out of shape.

• Nominal wall thickness is uniform across the part. Aim to hold a single nominal wall everywhere you can.
• Wall thickness sits in the sensible range for your material — roughly 1.0–3.5 mm for most thermoplastics (typically 1.5–2.5 mm for ABS/PC/PP). Check the specific grade with your material selection.
• No thick solid sections. Core out anything chunky so the wall stays consistent.
• Wall transitions are gradual, not abrupt. Where thickness must change, blend it over a distance of at least 3× the wall, never as a sudden step.
• Thickness changes stay within ~15% of nominal wherever possible.

Draft angles

Every surface that runs in the direction the part is pulled from the tool needs draft — a slight taper — so the part releases cleanly instead of dragging, scuffing or sticking. Zero-draft vertical walls are one of the most common rookie mistakes, and they cause ejection problems, drag marks and stress on the part.

• Every vertical face has at least 1° of draft per side as a working minimum; 1.5–2° is safer and releases more reliably.
• Textured surfaces have extra draft — add roughly 1–1.5° for every 0.025 mm (0.001″) of texture depth. Heavy grains can need 3–5°.
• Deep ribs, bosses and tall walls have generous draft — the deeper the feature, the more draft it needs to eject.
• Draft direction is consistent with the direction of tool opening.
• No zero-draft or “negative” faces unless you’ve accepted the side-action or lifter they require (see undercuts, below).

Ribs and bosses

Ribs add stiffness without adding wall thickness; bosses accept screws, pins and fasteners. Both are essential — and both cause sink marks and warp if they’re too thick where they meet the main wall.

• Rib base thickness is 40–60% of the nominal wall. Thicker than that and you’ll see a sink mark on the opposite (show) surface.
• Rib height is no more than about 3× the wall thickness. Taller ribs are hard to fill and eject.
• Ribs have at least 0.5° of draft per side.
• Space multiple ribs at least 2× the wall thickness apart to allow cooling and avoid a thick heat-trapped zone.
• Boss wall thickness is 40–60% of nominal, not a solid stub.
• Boss outside diameter is roughly 2× the screw hole diameter.
• Bosses are tied in with ribs or gussets rather than joined to the wall by a thick, sink-prone section, and are not standing alone in open space unsupported.

Radii and fillets

Sharp internal corners are stress concentrators — they crack in service, and they restrict and disrupt polymer flow during filling. Rounding them improves both strength and mouldability. The rule is simple: no sharp internal corners anywhere the design allows a radius.

• Internal corners have a radius of at least 0.5× the wall thickness (0.25× is the absolute minimum).
• External radius = internal radius + wall thickness, so the wall stays uniform around the corner.
• No sharp (zero-radius) internal corners on load-bearing or high-stress features.
• Radii are kept moderate — over-large radii can create a thick section of their own, so don’t over-correct.

Gate and parting-line placement

The gate is where molten plastic enters the cavity; the parting line is where the two tool halves meet. Both leave a mark on the part and both affect how it fills, so they need to be agreed at the design stage — not discovered on the first shot.

• The gate feeds into the thickest section so the part fills from thick to thin and packs out properly.
• The gate is away from cosmetic and critical surfaces — it always leaves a small witness mark.
• Flow length is achievable for the material and wall thickness; long, thin flow paths risk short shots and may need a second gate.
• Weld/knit lines (where flow fronts meet) fall in low-stress, non-cosmetic areas. These are a common defect origin — see our guide to injection moulding defects.
• The parting line sits on a natural edge of the part, where the small witness line won’t matter functionally or cosmetically.
• The parting line keeps the tool simple — a flat, straight parting line is far cheaper than a stepped or contoured one.

Tolerances

Tight tolerances cascade cost through the whole tool — more precise machining, more metrology, more validation. Some features genuinely need them; most don’t. Applying tight tolerances everywhere “to be safe” is one of the most expensive habits in part design.

• Only the features that must be precise carry tight tolerances — sealing faces, mating interfaces, bearing fits.
• General dimensions use standard moulding tolerances (a good default is DIN 16742 or the SPI/DME tolerance tables; roughly ±0.1 mm on smaller features is a typical general-purpose target).
• Tolerances account for material shrinkage, which varies by polymer and is much higher for semi-crystalline materials (e.g. PP, nylon) than amorphous ones.
• Critical-to-function dimensions are clearly flagged on the drawing so the toolmaker knows where to hold tight and where to open up.

Undercuts

An undercut is any feature that blocks the part from ejecting straight out of the tool — a side hole, a snap-fit lip, an external clip, an internal thread. Every undercut needs a mechanism (a side-action, lifter or collapsible core) to release it, and every mechanism adds cost, complexity and potential failure points to the tool.

• Undercuts are eliminated wherever the design allows. A relocated snap-fit or a “shut-off” through-hole can often remove an undercut entirely.
• Remaining undercuts are counted and understood — you know which need side-actions and lifters, and you’ve accepted that cost.
• Shallow undercuts in flexible materials are checked for “bump-off” (stripping the part off without a mechanism), which can avoid a side-action altogether.
• Internal undercuts and threads are reviewed carefully — they’re the most expensive kind to release, sometimes needing an unscrewing core or a metal insert instead. Where a threaded feature is involved, insert moulding a metal insert is often cheaper and stronger than moulding the thread.

Sink marks and warp avoidance

Sink marks (dimples on the surface over a thick section) and warp (the part twisting out of shape) are the two defects most directly caused by design rather than process. They almost always trace back to wall thickness and cooling — so most of the checklist above is really warp-and-sink prevention. A few final checks pull it together.

• No thick masses of material anywhere — the root cause of both sink and voids. Core them out.
• Walls are uniform, so the part cools evenly and doesn’t pull to one side.
• Ribs, bosses and features are proportioned to the 40–60% rule so they don’t telegraph a sink onto the show surface.
• The part is roughly symmetrical in its cooling, or the asymmetry is understood and compensated for.
• Glass-filled or reinforced materials get extra warp attention — fibre orientation causes directional shrinkage and can warp an otherwise sound design.

DFM quick-reference table

Keep this beside the CAD screen. The values are sound industry starting points — always confirm them against your specific material grade and part.

How Sino runs DFM

At Sino we treat DFM as the first hour of every tooling project, not a box-ticking formality. Because we design, cut steel, mould and measure under one roof at our UK-managed, ISO 9001:2015-certified factory in Shenzhen — with a mould repair and support facility in Querétaro, Mexico — the engineers reviewing your part are the same people who will tool and mould it. That means the DFM feedback you get is grounded in what our machines and toolmakers actually do, not a generic report.

We’ll walk your model against every item on this checklist, flag the features that will cause sink, warp, ejection or tooling-cost problems, and propose specific geometry changes — usually ones that improve the part and reduce the tool cost at the same time. Where a part needs a soft-touch grip or a second material, we’ll flag whether over-moulding is the right route; where it’s better realised as separate mouldings, we’ll say so.

Send us your part and we’ll run a free DFM review. Share a STEP file or a drawing, we’ll sign an NDA, and we’ll come back with an honest read on mouldability, the tooling implications, and the changes worth making before steel is cut. It’s the cheapest engineering hour in the whole programme.

Frequently asked questions

What is DFM in injection moulding?

DFM — Design for Manufacturability — is the process of reviewing a part’s geometry against how injection moulding behaves, so the part is easy to mould, cheap to tool and consistent in production. It covers wall thickness, draft angles, ribs and bosses, radii, gate and parting-line placement, tolerances, undercuts, and the sink and warp those choices cause. The goal is to catch problems in CAD, before the tool is cut.

What is the ideal wall thickness for an injection moulded part?

For most thermoplastics it’s roughly 1.0–3.5 mm, with 1.5–2.5 mm a common sweet spot for materials like ABS, PC and PP. The exact figure depends on the material grade and the part. Far more important than the absolute number is uniformity: keep the wall as consistent as possible across the whole part, because uneven walls cause sink, warp and voids.

How much draft angle does an injection moulded part need?

At least 1° of draft per side as a working minimum, with 1.5–2° safer for reliable ejection. Textured surfaces need more — add roughly 1–1.5° for every 0.025 mm (0.001″) of texture depth, and heavy grains can need 3–5°. Deeper features need more draft than shallow ones.

Why does my part have sink marks?

Sink marks are almost always a design issue: a section that’s too thick — often a rib or boss that’s too heavy where it meets the main wall — cools slowly and pulls the surface in. The fix is to core out thick sections, keep walls uniform, and size ribs and bosses to 40–60% of the nominal wall thickness. Process tweaks can reduce sink, but they can’t fully fix a geometry that causes it.

The bottom line

Good injection moulding starts on the CAD screen, not the shop floor. Almost every defect that shows up in a moulding trial — sink, warp, short shots, ejection marks, cracked corners — was designed in, and could have been designed out with a disciplined DFM pass. Run your part against this checklist, hold uniform walls, give every face draft, round your corners, tolerance only what matters, and design out the undercuts you can. Where a box won’t tick, raise it with your toolmaker now. See how DFM fits the wider moulding picture in our complete guide, then send us your part for a free DFM review — we’ll tell you honestly what to change before anyone cuts steel.