What Is Injection Molding?
Injection molding is a high-volume manufacturing process that produces plastic parts by injecting molten thermoplastic resin into a precision-machined mold cavity under pressures of 10,000–30,000 PSI (70–200 MPa). The plastic fills the cavity, cools, solidifies, and the mold opens to eject the finished part. Cycle times range from 10 seconds to 2 minutes depending on part size, wall thickness, and material.
High volume, low per-part cost
Injection molding requires significant upfront tooling investment ($2,000–$100,000+), but once the mold is built, per-part cost is very low — typically $0.10–$5.00 for small-to-medium parts at production volumes. The economics favor injection molding over CNC machining or 3D printing at volumes above 200–500 parts for most geometries.
Complex geometry in one shot
A single mold can produce parts with thin walls (0.040–0.120 in. / 1–3 mm), ribs, bosses, snap fits, living hinges, undercuts (with side actions or lifters), textured surfaces, and multiple materials (overmolding) — all in a single cycle with no secondary assembly.
Material variety
Virtually any thermoplastic resin can be injection molded: commodity plastics (ABS, PP, PE, PS), engineering plastics (nylon, POM, PC, PBT), high-performance plastics (PEEK, PEI/Ultem, PPS), elastomers (TPU, TPE), and glass/carbon-filled compounds. Material choice drives mechanical properties, chemical resistance, temperature rating, and part cost.
Repeatability
Once the mold is validated and process parameters are locked in, injection molding produces thousands to millions of identical parts with typical dimensional variation of ±0.002–0.005 in. (±0.05–0.13 mm). This consistency is difficult to match with CNC machining at high volumes because each CNC part is an independent operation subject to tool wear and setup variation.
The Injection Molding Cycle
Every injection-molded part goes through the same 4-phase cycle. Understanding this cycle explains why wall thickness, cooling time, and gate location matter so much in DFM.
Clamping
The two mold halves close under 50–4,000 tons of clamping force. The force must exceed the injection pressure × projected area of the part, or the mold will flash (leak plastic at the parting line). Larger parts require larger presses.
Injection
A reciprocating screw pushes molten resin through the sprue, runner, and gate into the cavity at 10,000–30,000 PSI. Fill time is typically 0.5–5 seconds. The screw then holds pressure ("pack and hold") to compensate for volumetric shrinkage as the plastic cools.
Cooling
The mold absorbs heat through internal cooling channels (water or oil). Cooling is the longest phase — typically 50–80% of total cycle time. Thicker walls cool slower: doubling wall thickness roughly quadruples cooling time. Uniform wall thickness = uniform cooling = fewer warpage defects.
Ejection
The mold opens, ejector pins push the part off the core, and the part falls or is robotically removed. Draft angle on all vertical walls (1–3° minimum) ensures the part releases cleanly. Insufficient draft causes drag marks, sticking, or part damage.
Mold Design Fundamentals
The mold is a precision tool — typically CNC-machined from P20 pre-hardened steel (production) or 7075-T6 aluminum (prototype). Understanding mold anatomy helps you design parts that are moldable, cost-efficient, and defect-free.
Core & Cavity
The cavity (A-side) forms the external cosmetic surface. The core (B-side) forms the internal features. The part shrinks onto the core during cooling, which is why most ejection happens from the B-side.
Parting Line
The line where the two mold halves meet. Visible on the finished part as a faint line or slight mismatch. Place the parting line on a non-cosmetic edge or along a geometric transition to minimize visual impact.
Gate
The opening through which molten plastic enters the cavity. Common types: edge gate, sub-gate (auto-trimming), tab gate, and hot-tip (direct). Gate location affects fill pattern, weld lines, and vestige (witness mark). Place gates at the thickest wall section.
Runner System
The channels that distribute plastic from the sprue to the gate(s). Cold runners waste material (reground). Hot runners keep plastic molten — no waste, but add $5,000–$30,000 to mold cost. Multi-cavity molds need balanced runners for uniform fill.
Ejector Pins
Spring-loaded steel pins that push the part off the core. They leave small circular witness marks (typically ⌀0.125–0.250 in.) on the B-side. Place ejectors on non-cosmetic, structurally reinforced areas (bosses, ribs).
Cooling Channels
Drilled or conformal-cooled passages in the mold that circulate water at 50–180°F (10–82°C) depending on resin. Cooling channel layout is the #1 factor controlling cycle time and warpage. Conformal cooling (3D-printed inserts) can reduce cycle time 20–40% on complex parts.
DFM Rules for Injection Molding
Uniform wall thickness
Maintain consistent wall thickness throughout the part (target 0.060–0.120 in. / 1.5–3 mm for most resins). Thick-to-thin transitions cause differential cooling → sink marks on thick sections, warpage, and internal voids. If thickness must vary, transition gradually (3:1 taper ratio).
Draft angle on all vertical walls
Apply 1° minimum draft per side on untextured surfaces, 1.5–3° on textured surfaces. Shut-off faces need 3–5° minimum. Zero-draft walls stick to the mold, cause drag marks, and shorten mold life. Draft is free — it costs nothing to add during design but is expensive to fix after the mold is cut.
Rib design: 60% of wall thickness
Ribs add stiffness without increasing wall thickness. Keep rib thickness at 50–60% of the adjacent wall to avoid sink marks on the opposite surface. Rib height should not exceed 3× wall thickness. Add 0.5–1° draft per side on ribs. Fillet the rib base at 25–50% of wall thickness.
Boss design for fasteners
Bosses (cylindrical features for screws or press-fits) should have an OD of 2–2.5× the ID, a wall thickness of 60% of the nominal wall, and be connected to adjacent walls with ribs or gussets — never a thick section. Unsupported tall bosses (height > 2× OD) deflect during screw insertion.
Avoid undercuts (or design for them)
Undercuts — features that prevent the part from being pulled straight out of the mold — require side actions, lifters, or collapsing cores. Each adds $1,000–$10,000 to mold cost. Simple undercuts (snap-fit hooks) can use a bumping/stripping action if the material is flexible enough (PP, PE, TPE).
Core out thick sections
Never design a solid block of plastic. Thick sections (>0.200 in. / 5 mm) cause extended cooling time, sink marks, voids, and warpage. Core out thick areas to maintain uniform wall thickness. Use ribs and gussets for structural stiffness instead of material volume.
Common Injection Molding Materials
| Resin | Type | Shrinkage | Key Properties | Typical Use |
|---|---|---|---|---|
| ABS | Amorphous | 0.4–0.7% | Good impact, paintable, easy to mold | Consumer electronics, enclosures, toys |
| Polycarbonate (PC) | Amorphous | 0.5–0.7% | Optical clarity, high impact, 250°F HDT | Lenses, safety shields, medical housings |
| Nylon 6/6 (PA66) | Semi-crystalline | 1.0–2.5% | High strength, wear resistance, hygroscopic | Gears, bearings, structural clips |
| POM (Delrin) | Semi-crystalline | 1.8–2.5% | Low friction, dimensional stability | Gears, bushings, valve bodies |
| Polypropylene (PP) | Semi-crystalline | 1.0–2.5% | Chemical resistance, living hinges, FDA | Containers, caps, medical disposables |
| PC/ABS Blend | Amorphous | 0.5–0.7% | Impact + heat resistance of PC, moldability of ABS | Automotive interiors, laptop housings |
| PEEK | Semi-crystalline | 1.2–1.5% | 480°F HDT, chemical resistance, sterilizable | Aerospace, medical implants, oil & gas |
Shrinkage matters for mold design
The mold cavity is cut oversized to compensate for material shrinkage. Amorphous resins (ABS, PC) shrink 0.4–0.7% — predictable and uniform. Semi-crystalline resins (nylon, POM, PP) shrink 1.0–2.5% and can shrink non-uniformly depending on wall thickness and cooling rate. Higher shrinkage = harder to hold tight tolerances. Always confirm shrinkage rate with your molder before finalizing the mold design.
Injection Molding Tolerances
| Feature | Standard | Fine | Notes |
|---|---|---|---|
| Linear dimensions | ±0.005 in./in. (±0.13 mm/25 mm) | ±0.002 in./in. (±0.05 mm/25 mm) | Applies per inch of dimension. Accumulates on large parts. |
| Flatness | ±0.005 in./in. | ±0.002 in./in. | Warpage is the main failure mode. Uniform walls minimize warpage. |
| Hole diameter | ±0.002 in. (±0.05 mm) | ±0.001 in. (±0.025 mm) | Core pins hold tighter tolerances than mold cavity features. |
| Wall thickness | ±0.003 in. (±0.08 mm) | ±0.001 in. (±0.025 mm) | Controlled by mold steel — machined to ±0.0005 in. |
| Parting line mismatch | ±0.003 in. (±0.08 mm) | ±0.001 in. (±0.025 mm) | Depends on mold construction and press condition. |
Cost Structure
Injection molding cost has two components: NRE (tooling) and recurring (per-part). Understanding both helps you decide if the volume justifies the investment.
| Mold Type | Material | Tooling Cost | Mold Life | Lead Time | Typical Use |
|---|---|---|---|---|---|
| Prototype (soft) | 7075-T6 aluminum | $2,000–$10,000 | 1,000–10,000 shots | 2–4 weeks | Design validation, pilot runs |
| Bridge (semi-hard) | P20 pre-hardened steel | $8,000–$30,000 | 50,000–200,000 shots | 4–6 weeks | Low-volume production, market testing |
| Production (hard) | H13 or S7 hardened steel | $15,000–$100,000+ | 500,000–2,000,000+ shots | 6–12 weeks | High-volume production |
| Multi-cavity | H13 hardened steel | $30,000–$200,000+ | 1,000,000+ shots | 8–16 weeks | Very high volume (4–32 cavities) |
Break-even rule of thumb
For a part that costs $5.00/piece CNC-machined and $0.50/piece injection-molded with a $5,000 prototype mold: break-even is at approximately 1,100 parts ($5,000 ÷ ($5.00 − $0.50) = 1,111). Below that quantity, CNC is more economical. Above it, injection molding. Use the Injection Molding Cost Breakdown for detailed volume-tier analysis.
When to Choose Injection Molding
Is your production volume above 500 parts?
Injection molding — tooling cost amortizes across the volume, driving per-part cost well below CNC machining.
CNC machining or 3D printing for low-volume plastic parts. No tooling investment required.
Does the part have thin walls, ribs, snap fits, or living hinges?
Injection molding — these features are natural to the process and add minimal cost. CNC machining thin walls in plastic is slow and fragile.
If the part is a solid block with pockets and bores, CNC machining may be more straightforward.
Do you need parts within 2 weeks?
CNC machining or 3D printing — mold lead time is typically 4–8 weeks for prototype tools and 8–16 weeks for production tools.
If you can wait 4–8 weeks for tooling, injection molding delivers production parts at the lowest per-piece cost.
Does the part require tolerances tighter than ±0.002 in.?
CNC machining — injection molding standard tolerance is ±0.005 in./in. Features tighter than ±0.002 in. may require secondary CNC operations after molding.
Injection molding tolerances (±0.002–0.005 in.) are sufficient for most functional plastic parts.
Frequently Asked Questions
What is the minimum order quantity for injection molding?
What is draft angle and why is it required?
What is the difference between a hot runner and a cold runner?
How do injection molding tolerances compare to CNC machining?
What materials are commonly injection molded?
When should I choose injection molding vs. CNC machining for plastic parts?
Related Resources
Ready to Get Injection Molded Parts?
Upload your 3D model and get a quote for prototype or production tooling. MakerStage provides DFM feedback, material recommendations, and mold-flow analysis on every project.
Get Free Quote Fast