Injection molding design guide: walls, draft, ribs, gates
SSG MFG engineering6 min readInjection molding
How do you design a part for injection molding?
Design for injection molding by keeping walls uniform, typically 0.040–0.150 in (1.0–3.8 mm) depending on resin, adding at least 1° of draft per side, sizing ribs at 40–60% of the adjoining wall, and coring out thick sections. Gate into the thickest section, radius every inside corner, and hold tight tolerances only on features that affect fit or function.
How thick should injection molded walls be?
Wall thickness sets cycle time, part cost, and most cosmetic defects. Cooling time rises with roughly the square of wall thickness, so doubling a wall from 0.080 in to 0.160 in (2 mm to 4 mm) can nearly quadruple the time the part spends in the mold. Pick the thinnest wall that meets strength and fill requirements, then hold it constant across the part.
| Resin | Recommended wall | Typical shrink |
|---|---|---|
| ABS | 0.045–0.140 in (1.1–3.6 mm) | 0.4–0.7% |
| Polycarbonate (PC) | 0.040–0.150 in (1.0–3.8 mm) | 0.5–0.7% |
| PC/ABS | 0.040–0.150 in (1.0–3.8 mm) | 0.5–0.7% |
| Acrylic (PMMA) | 0.025–0.500 in (0.6–12.7 mm) | 0.2–0.8% |
| Polypropylene (PP) | 0.025–0.150 in (0.6–3.8 mm) | 1.0–2.5% |
| HDPE | 0.030–0.200 in (0.8–5.1 mm) | 1.5–3.0% |
| Acetal (POM) | 0.030–0.120 in (0.8–3.0 mm) | 1.8–2.5% |
| Nylon 66, unfilled | 0.030–0.115 in (0.8–2.9 mm) | 1.0–2.0% |
| Nylon 66, 30% glass | 0.040–0.125 in (1.0–3.2 mm) | 0.2–0.8%, varies with flow direction |
| PBT | 0.025–0.125 in (0.6–3.2 mm) | 1.5–2.2% |
How much draft do injection molded parts need?
Draft is the taper on faces parallel to the direction the mold opens. Without it, the part drags on the steel, scuffs, and resists ejection. Plastic shrinks onto cores, so inside walls usually need as much draft as outside walls, or more.
- 1° per side is the default for most smooth, polished faces.
- 0.5° per side works on short features with a polished finish, at some risk of drag marks.
- Textured faces need about 1–1.5° per side for every 0.001 in (0.025 mm) of texture depth. Light textures need about 1.5°; heavy textures need 3–5°.
- Deep features, over about 2 in (50 mm), release more cleanly with 2° or more.
- Shutoffs, where cavity and core steel touch to form a window, need at least 3° or they wear and flash.
How should ribs and bosses be sized?
Ribs add stiffness without adding wall thickness. Bosses carry screws, inserts, and pins. Both create a thick spot where they meet the wall, which is where sink marks come from, so their proportions matter more than their count.
| Feature | Guideline | Why |
|---|---|---|
| Rib thickness | 0.4–0.6 × t; 0.4–0.5 × t on cosmetic faces | Prevents sink opposite the rib |
| Rib height | ≤ 3 × t | Tall ribs are hard to fill and eject |
| Rib spacing | ≥ 2 × t between ribs | Leaves room for steel and cooling |
| Rib draft | 0.5–1° per side | Ribs are deep, narrow slots in the mold |
| Rib base radius | 0.25–0.5 × t | Reduces stress without thickening the joint |
| Boss outside diameter | About 2 × screw or insert diameter | Resists hoop stress from the fastener |
| Boss wall | ≤ 0.6 × t | Avoids sink on the opposite face |
| Corner radii | Inside ≥ 0.5 × t; outside = inside + t | Keeps the wall uniform through the corner |
Where should the gate go on an injection molded part?
The gate is where plastic enters the cavity. Its location sets the fill pattern, where knit lines form, which areas pack best, and where a small vestige is left. Agree on it with the tooling engineer before the design is frozen.
- Edge or tab gate: simple and low cost; leaves a vestige at the parting line.
- Submarine (tunnel) gate: shears off automatically at ejection; suits small, high-volume parts.
- Pin-point gate: used in three-plate molds to gate onto a top face.
- Hot tip or valve gate: fed from a hot runner, with no runner scrap.
- Fan and diaphragm gates: spread flow across flat or round parts to limit warp.
Gate into the thickest section so it can be packed as it cools, and let flow run from thick to thin. Aim the gate at a wall or core pin to prevent jetting. Keep knit lines, which form where flow fronts meet around holes, away from load paths and cosmetic faces.
How do you handle undercuts in a molded part?
An undercut is any feature that keeps the part from ejecting straight off the core: side holes, snap hooks, threads, or grooves. Each one needs a side action, lifter, or unscrewing mechanism, which adds tool cost, maintenance, and sometimes cycle time.
- Pass-through coring: open a window under a snap hook so core and cavity steel shut off against each other and form the hook without a lifter.
- Bump-off: flexible resins such as PP and TPE can strip a shallow undercut off the core if the material stretches without yielding.
What tolerances can injection molding hold?
Tolerance depends on resin shrink, part size, wall uniformity, and the number of cavities. The Plastics Industry Association (formerly SPI) publishes commercial and fine tolerance charts by resin, and ISO 20457 covers tolerances for molded plastic parts internationally.
- Commercial: about ±0.005 in (±0.13 mm) on the first inch, plus about ±0.002 in per additional inch, in low-shrink resins.
- Fine: about ±0.002–0.003 in (±0.05–0.08 mm) on small features, with added tool and process cost.
- High-shrink semicrystalline resins (PP, HDPE, POM, nylon) need looser tolerances and warp more than amorphous resins such as ABS and PC.
Which design mistakes cause common molding defects?
| Defect | Design cause | Design fix |
|---|---|---|
| Sink marks | Thick sections, heavy ribs, solid bosses | Core out; ribs at 0.4–0.6 × wall |
| Warp | Uneven walls, one-sided ribs, glass fiber orientation | Uniform walls, balanced ribs, gate for even flow |
| Short shots | Thin walls far from the gate, long flow length | Thicken the flow path or add a gate |
| Knit lines | Flow splitting around holes and cores | Move the gate, or move holes off load paths |
| Drag marks | Too little draft, especially on textured faces | Increase draft to match texture depth |
How do you get an injection molded part quoted?
Upload a STEP file or configure the part in the SSG builder at /build. You get an instant budgetary estimate for tooling and piece price, plus a DFM check that flags thin or thick walls, missing draft, and undercuts. When the design is ready, an SSG rep routes the RFQ to principals matched to the part size, resin, and volume, and returns firm quotes.
