Injection Molding
Injection molding forces molten thermoplastic into a steel mold under high pressure, producing high-volume identical plastic parts.
- Part
- Forming
- Variants
- 4
- Revised
- 2026-08-11
At a glance
- Family
- Plastics and Rubber
- Typical tolerances
- ±0.005 in (±0.127 mm) commercial on features under 1 in; ±0.002 in (±0.05 mm) precision; ±0.1–0.2% of dimension on larger parts. Add tolerance for anything spanning the parting line or a side action.
- Surface finish
- SPI A-1 mirror (about 0.5 µin / 0.012 µm Ra) through SPI D-3 dry blast (about 125 µin / 3.2 µm Ra), plus MT-series molded textures
- Typical volumes
- 1,000–1,000,000+ parts; economics are strongest above 10,000
- Lead time
- 2–4 weeks for an aluminum bridge tool, 6–12 weeks for a hardened steel production tool; parts in hours to days once the tool is sampled
- Materials
- Plastic
What it is
Injection molding forces molten thermoplastic into a closed steel mold under high pressure, holds it while it cools, and ejects a finished part — typically on a 15–60 second cycle. It is the default process for plastic parts made in the thousands to the millions: enclosures, connectors, closures, gears, medical disposables, and most molded consumer goods. Nearly any thermoplastic runs on it — ABS, PP, PC, nylon, acetal, PEEK — plus glass- and mineral-filled compounds, and thermosets on modified machines.
The economics reduce to one number: the mold. Tooling is a multi-week capital item; after it exists, the marginal cost of a part is measured in cents. Below roughly 1,000 parts that trade rarely pays, and above 10,000 nothing else competes on unit cost. Commercial tolerances run about ±0.005 in (±0.127 mm) on molded features, with ±0.002 in (±0.05 mm) achievable on well-controlled dimensions in a hardened precision tool.
How it works
- Dry the resin. Hygroscopic polymers — nylon, PC, PET, ABS, PBT — are dried 2–4 hours at 175–250 °F (80–120 °C) to well under 0.02% moisture. Wet resin hydrolyzes in the barrel, showing up as silver streaking and a loss of impact strength that no process adjustment recovers.
- Plasticize. A reciprocating screw melts pellets through barrel heat and shear, then retracts as it meters a shot. Typical melt temperatures: PP 400–480 °F (200–250 °C), ABS 410–480 °F (210–250 °C), nylon 500–550 °F (260–290 °C), PC 540–610 °F (280–320 °C).
- Inject. The screw drives forward as a ram and fills the cavity in roughly 0.5–4 seconds. Injection pressure at the nozzle commonly runs 5,000–20,000 psi (35–140 MPa). Clamp tonnage is sized from projected area — a working rule is 2–5 tons per square inch, at the higher end for stiff, low-flow resins and thin walls.
- Pack and hold. At about 95–98% fill the machine switches from velocity to pressure control and packs additional melt in to compensate for cooling shrinkage, holding until the gate freezes off. This phase, not the fill, determines sink marks, dimensional repeatability, and residual stress.
- Cool. Coolant circulates through the mold, held at 60–140 °F (15–60 °C) for commodity resins and 180–250 °F (80–120 °C) for PC, PPS, and PEEK.
Why is cooling most of the cycle?
Cooling time scales with the square of the wall thickness, because heat has to conduct out through that wall. It is normally 50–80% of total cycle time. Going from a 2.5 mm wall to 2.0 mm cuts the cooling term by roughly a third — far more leverage than any barrel-temperature tweak.
- Eject. The mold opens and ejector pins, sleeves, or a stripper plate push the part off the core. Draft is what makes this possible; parts with no draft gall and scuff on the way out.
- Degate and regrind. Cold sprues and runners are trimmed and can usually be reground and blended back at 10–25%. Hot runner systems eliminate that scrap entirely at higher tooling cost.
Which variants of the process matter?
Moldflow analysis simulates fill, pack, cooling, and warpage before steel is cut, and is standard practice on any tool with a long flow path or a tight flatness requirement. Gas-assisted injection molding injects nitrogen into a partly filled cavity to hollow out thick sections, which removes sink marks from handles and structural ribs and cuts material and cycle. Multishot (two-shot) molding runs two injection units into a rotating tool to combine two resins or colors in one part. In-mold decoration places a printed film in the cavity so graphics are molded in, permanently, rather than printed on afterward.
Design guidelines
Wall thickness
Keep it uniform and thin. Most thermoplastics mold well between 0.040 and 0.140 in (1.0–3.5 mm): ABS 0.045–0.140 in (1.14–3.56 mm), PC 0.040–0.150 in (1.02–3.81 mm), PP 0.025–0.150 in (0.64–3.81 mm). Where thickness must change, blend over at least 3× the step rather than jumping. Per-polymer minimums and maximums are tabulated on /charts/injection-molding-design-guidelines.
Draft
Use 1–2° per side as the untextured default. Shutoffs and features under 1 mm tall can go down to 0.25–0.5°. Ribs and internal bosses need 0.5–1.5°. Textured surfaces need much more: 3° for light MT-11010/11020 textures, 3–5° for medium texture, and 5–7° for heavy leather grain. The shop rule is to add roughly 1.5° per 0.001 in (0.025 mm) of texture depth on top of the base draft.
Corners and radii
Internal corner radius ≥ 0.5 × nominal wall; external radius = internal radius + wall, which keeps the wall uniform through the corner. Sharp internal corners are the most common cause of field cracking: at R/T = 0.5 the stress concentration factor sits near 1.5, but at R/T = 0.1 it climbs past 3.
Ribs
Rib base thickness 0.5–0.6 × wall, dropping to 0.4–0.5 × wall behind a cosmetic or textured face. Height ≤ 3 × wall. Center-to-center spacing ≥ 2 × wall. Base fillet 0.25–0.5 × wall. Ribs stiffen far more efficiently than thick walls, because bending stiffness goes with the cube of section depth.
Bosses
Boss outside diameter 2–2.5 × the screw's major diameter; boss wall 0.5–0.6 × nominal wall. Never blend a boss straight into a side wall — connect it with a rib or gusset so you do not create a heavy junction that sinks. Core the boss all the way to the base.
Holes and cores
Keep hole-to-hole and hole-to-edge spacing ≥ 2 × hole diameter. Blind core pins should stay under about 3:1 length-to-diameter; a core shut off at both ends can run to about 5:1. Beyond that the pin deflects and the hole comes out tapered or out of position.
Undercuts and threads
Every side action, lifter, or unscrewing core adds tooling cost and a tolerance stack. Shallow undercuts in flexible resins can often be bumped off with no mechanism at all. External threads split cleanly across the parting line; internal threads need an unscrewing or collapsible core, or a molded-in insert.
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Nominal wall | 0.060–0.120 in (1.5–3.0 mm) | 0.020–0.200 in (0.5–5 mm) | Thin fills fast and cools fast; thick sinks and voids |
| Wall transition | Taper over 3× the step | Abrupt step | Sudden changes freeze flow and warp the part |
| Draft, untextured | 1.5° per side | 0.25° at shutoffs | Below this the part drags and scuffs on ejection |
| Draft, textured | 3° light, 5–7° heavy grain | — | About 1.5° per 0.001 in of texture depth |
| Internal radius | 0.5 × wall | 0.25 × wall | Stress concentration climbs sharply below 0.5 T |
| Rib thickness | 0.5 × wall | 0.6 × wall | Above 0.6 T a sink mark shows on the opposite face |
| Rib height | 2.5 × wall | 3 × wall | Taller ribs are hard to fill and to eject |
| Boss OD | 2 × screw major dia. | 2.5 × screw major dia. | Resists hoop stress from a thread-forming screw |
| Hole spacing | 2 × hole diameter | — | Thin webs between holes are weak and hard to fill |
Cost drivers
Tooling dominates everything else. A single-cavity aluminum bridge tool, a single-cavity P20 steel tool, and a 16-cavity hardened H13 tool with a hot runner differ by more than an order of magnitude in both price and break-even volume. Per-part cost is then machine rate × cycle time ÷ cavity count, plus material, plus scrap.
Practical breakpoints:
- Under 100 parts: urethane casting or additive — no mold pays back.
- 100–1,000: aluminum bridge tooling, single cavity.
- 1,000–100,000: P20 or NAK80 steel, one to four cavities.
- Over 100,000: hardened steel, high cavitation, hot runner, automated part removal.
Ways to take cost out:
- Thin the wall. Cooling time goes with wall squared. Dropping a 2.5 mm wall to 2.0 mm cuts cooling roughly a third and takes material out at the same time.
- Kill the side actions. Redesigning an undercut into a through-hole formed by a shutoff between core and cavity removes a slide, its maintenance, and its tolerance stack.
- Add cavities, not machines. Once annual volume passes a few tens of thousands, a second or fourth cavity is almost always cheaper per part than more machine hours.
- Loosen non-functional tolerances. Call out ±0.002 in only where it does something; ±0.010 in elsewhere lets the molder run a faster, cooler cycle.
- Texture instead of polish. SPI A-series finishes are hand-polished with diamond compound and are among the most expensive line items on a mold quote. An MT texture hides sink and knit lines and costs far less.
Variants
4 named
Moldflow analysis
Gas-assisted Injection Molding
Multishot Injection Molding
In-Mold Decoration
Questions
7 questionsWhat draft angle do I need for injection molding?
Use 1–2° per side on untextured surfaces as a default, and 0.5–1.5° on ribs and internal bosses. Textured surfaces need substantially more: about 3° for a light MT texture and 5–7° for heavy leather grain. The working rule is to add roughly 1.5° of draft for every 0.001 in (0.025 mm) of texture depth.
What is the minimum wall thickness for injection molding?
For most thermoplastics the practical range is 0.040–0.140 in (1.0–3.5 mm). High-flow resins such as polypropylene, acetal, and LCP fill down to about 0.025–0.030 in (0.64–0.76 mm), while low-flow polycarbonate wants at least 0.040 in (1.02 mm). Uniformity matters more than the absolute number.
What tolerance can injection molding hold?
About ±0.005 in (±0.127 mm) is standard commercial practice on features under an inch, and ±0.002 in (±0.05 mm) is achievable on well-controlled dimensions in a hardened tool. On larger parts, think in percentage terms — ±0.1 to ±0.2% of the dimension — because polymer shrinkage, not machining, sets the variation.
How thick can a rib be before it causes a sink mark?
Keep the rib base at 0.5–0.6 times the nominal wall thickness. Behind a cosmetic or gloss face, drop to 0.4–0.5 times the wall. Above 0.6 T the rib holds enough heat that the opposite surface pulls in as it cools, which reads as a visible sink line.
How many parts do I need before injection molding makes sense?
Roughly 1,000 parts is the crossover against urethane casting and additive manufacturing, and above about 10,000 parts nothing else competes on unit cost. Below 1,000, the mold cost per part swamps the savings on the part itself.
Why is cooling most of the injection molding cycle?
Heat has to conduct out through the part wall, so cooling time scales with the square of wall thickness. It typically accounts for 50–80% of a 15–60 second cycle. Reducing a 2.5 mm wall to 2.0 mm cuts the cooling term by roughly a third.
Can injection molding produce threads?
Yes. External threads split across the parting line at no extra tooling complexity. Internal threads need an unscrewing core or a collapsible core, both of which add cost and maintenance — for low volumes a molded-in or heat-staked brass insert is usually cheaper and stronger.