Injection molding design guide
A molded part is a frozen skin of plastic around a steel core that has to pull out. Uniform walls, draft on every vertical face and no undercut you did not plan for — get those three right and the tool is cheaper, the cycle shorter and the part flat.
Four facts about the mold that set every rule below
Every molding rule is a consequence of how plastic fills, cools and leaves a steel cavity.
1 wall
Plastic cools from the outside in
A thick section stays molten longer than a thin one next to it — it shrinks more, sinks and warps the part. Uniform wall thickness is rule one; everything else follows.
≥ 1°
The part has to let go of steel
Every face parallel to the opening direction drags on the cavity as the part shrinks onto the core. Draft — a slight taper — lets it release without scuffing or bending.
2 halves
The tool opens one way
Anything the two halves cannot form — a side hole, a snap hook, an internal thread — needs a moving core, a slide or a hand-loaded insert. Each one is tooling cost and cycle time.
0.4–2 %
Plastic shrinks
PP shrinks 1.5–2 %, ABS 0.5 %, glass-filled nylon 0.3 % along the fibres and 1 % across. The toolmaker scales the cavity for it; you design so that shrinkage is even.
Wall thickness by resin
Pick one nominal wall and hold it within ± 10 % across the part. Thick where you need stiffness means ribs, not a thicker wall; thin where you need light means the whole part thin.
| Resin | Wall thickness | Shrinkage | Notes |
|---|---|---|---|
| ABS | 1.2–3.5 mm | 0.4–0.7 % | The default cosmetic housing resin; paints and plates well |
| Polycarbonate (PC) | 1.0–3.8 mm | 0.5–0.7 % | Clear and tough; sensitive to sharp corners and stress |
| PC/ABS | 1.2–3.5 mm | 0.5–0.7 % | Housings that need PC toughness at ABS cost |
| Polypropylene (PP) | 0.8–3.8 mm | 1.5–2.0 % | Living hinges, containers; high shrinkage — mind the warp |
| Polyethylene (HDPE) | 0.8–3.0 mm | 1.5–3.0 % | Chemical resistance; cannot be glued or painted |
| Nylon (PA6 / PA66) | 0.8–3.0 mm | 0.8–1.5 % | Gears, clips, structural; absorbs moisture and grows |
| Nylon 30 % glass-filled | 0.8–3.0 mm | 0.3–1.0 % | Stiff structural parts; anisotropic shrinkage warps flat plates |
| POM (acetal) | 0.8–3.0 mm | 1.8–2.5 % | Low friction, snap fits; high shrinkage, poor paint adhesion |
| PMMA (acrylic) | 0.6–3.0 mm | 0.3–0.7 % | Optical lenses and covers; brittle — generous radii |
| TPU / TPE (soft) | 1.0–3.0 mm | 1.0–2.0 % | Grips and seals, Shore 30A–90A; the overmold materials |
| PEEK / PEI (Ultem) | 1.0–3.0 mm | 0.7–1.3 % | High-temperature engineering parts; hot tools and slow cycles |
Ranges are the moldable window; most housings sit at 2.0–2.5 mm, most small clips at 1.2–1.5 mm. Above ~4 mm the cycle time doubles and sink marks appear over ribs; below the minimum the cavity does not fill before the plastic freezes.
- Core out thick sections. Any solid block thicker than the nominal wall becomes a shelled section with ribs. Same stiffness, half the cycle, no sink.
- Transition thickness gradually. Where two thicknesses meet, taper over 3 × the difference. A step is a sink mark and a stress line.
- Flow length limits the wall. Thin walls fill only so far from the gate — roughly 100 × T for ABS, 150 × T for PP. A 300 mm panel at 1.5 mm needs two gates or a thicker wall.
Draft, radii and corners
Draft is not optional. Every face parallel to the pull direction gets it, and textured faces get more.
| Feature | Rule | Why |
|---|---|---|
| Draft — smooth, shallow faces | 1° minimum; 2° preferred | Under 1° the part drags on the steel, whitens and marks at the ejector |
| Draft — deep cores and ribs | 0.5° per 25 mm of depth, min 1° | A 100 mm-deep box needs 2°+ on the inside; the core pulls a vacuum otherwise |
| Draft — textured faces | +1° per 0.025 mm of texture depth | A medium texture (0.05 mm) needs 3°; texture grips the steel as the part shrinks |
| Inside corner radius | ≥ 0.5 × T, ideally 1 × T | Sharp inside corners concentrate stress and create thick spots where the walls meet |
| Outside corner radius | inside R + T | Keeps the wall uniform through the corner — a constant-thickness bend, not a thick knuckle |
| Edge on a parting line | sharp or ≤ 0.2 mm | A radius on a parting edge cannot be cut in both halves without a witness step |
| Snap-fit and hook faces | draft on the non-functional faces only | The catch face is a designed undercut (see below); every other face still needs draft |
Zero-draft faces are possible — with a slide, a hand-loaded insert or a polished cavity and slow ejection — but each is a line on the tooling quote. Ask the engineer before you design one in.
Ribs, bosses and gussets
Stiffness comes from geometry, not thickness. These proportions add stiffness without sink marks, voids or a slow cycle.
| Feature | Rule | Why |
|---|---|---|
| Rib thickness at base | 0.5–0.6 × T | Thicker ribs create a thick knot at the wall that sinks on the cosmetic side |
| Rib height | ≤ 3 × T | Tall thin ribs trap air, fill last and bend on ejection |
| Rib spacing | ≥ 2 × T between ribs | Closer, the steel between ribs cannot be cooled and the wall sinks |
| Rib draft | 0.5–1° per side | Ribs are deep cores — they need more draft than the wall |
| Rib base radius | 0.25–0.5 × T | Removes the stress riser; larger radii thicken the base and sink |
| Boss outer diameter | 2 × the hole diameter | Thinner, the screw splits the boss; thicker, it sinks |
| Boss wall thickness | 0.6 × T; boss height ≤ 3 × OD | A free-standing boss is a chimney of thick plastic — tie it to a wall with gussets |
| Boss-to-wall connection | gusset or rib, never a solid fillet | Solid fillets create a thick section; gussets stiffen without one |
| Core out under the boss | recess the wall opposite | The boss footprint is the classic sink mark — remove material behind it |
For thread-forming screws in a boss the hole is 0.8 × the screw OD with a 0.5 mm counterbore lead-in; for a brass insert (heat-staked or molded-in) follow the insert maker’s hole spec. Ultrasonic inserts need a 1° tapered hole.
Undercuts, side actions and the parting line
The tool opens in one direction. Anything it cannot form on the way out is an undercut — solvable, but each solution has a price.
| Feature | Solution | Tooling effect |
|---|---|---|
| Side hole or window through a wall | shut-off — a pass-through core from the other half | Free if the hole can open toward the parting line; leaves a witness line |
| Snap-fit hook, small | bump-off (stripped over the core) | Free for PP / PE / TPU with ≤ 5 % strain; not for glass-filled or brittle resins |
| External undercut, one side | slide (side action) | + 1–2 weeks and roughly 10–25 % on tooling; a mark where the slide meets |
| Internal undercut | lifter or collapsible core | Complex, wears; often cheaper to redesign the feature open toward the pull |
| Internal thread | unscrewing core or hand-loaded insert | Unscrewing tools are the most expensive mechanism in molding; design the thread as an insert or make it external |
| External thread | split along the parting line | Free; the thread carries a parting-line witness — fine for caps, not for seals |
| Living hinge | 0.25–0.5 mm PP web, gate on one side | Free in PP with flow across the hinge; flex it warm right out of the tool |
Place the parting line where a witness line is acceptable — on an edge, not across a cosmetic face — and where the tool can vent. Gate location decides the flow, the weld lines and the warp; the engineer will propose it, but leave a 3 mm flat for it on a non-cosmetic face.
- Open every feature toward the parting line. A hook that faces the pull direction is a shut-off; the same hook turned 90° is a slide.
- Design the ejector pads in. Ejector pins need 3–5 mm flat landings on the B-side; a part with no flat surface gets pin marks in the wrong place.
- Vent the last place to fill. Blind ribs and boss tops trap air and burn (diesel effect). Keep the far end of the flow path reachable from the parting line.
Insert molding, two-shot and LSR — the extra rules
The same wall, draft and rib rules apply. Each variant adds a few of its own.
| Variant | Rule | Why |
|---|---|---|
| Insert molding — metal inserts | ≥ 0.5 × insert diameter of plastic around it; knurl or undercut the insert | Thin plastic over a cold insert cracks as it shrinks; a smooth insert pulls out |
| Insert molding — locating | the insert must sit on a core pin or in a pocket with ≤ 0.05 mm play | Inserts float in the melt otherwise; robot-placed inserts need a chamfer lead-in |
| Insert molding — cycle | budget 5–15 s extra per shot | Loading time is cycle time; vertical machines or a rotary table hide it |
| Two-shot / overmold — bond | chemically compatible pair (PC + TPU, PP + TPE) or mechanical interlock | Incompatible pairs delaminate; interlocks (through-holes, dovetails) work with any pair |
| Two-shot — soft layer | 1.0–3.0 mm TPE, uniform, over a 1.5 mm+ substrate | Thin soft skin tears; thick skin sinks and slows the cycle |
| Two-shot — tooling | rotary or core-back tool; 2 × cavity cost | Two-shot needs two cavities and a two-barrel machine; overmolding in two separate tools is cheaper under ~10 k parts |
| LSR (liquid silicone) — wall | 0.4–8 mm; flash-free with 0.005 mm shut-offs | LSR flows like water — the tool must be tighter than a thermoplastic tool |
| LSR — draft and undercuts | little or no draft needed; undercuts up to 30 % strain strip fine | Silicone stretches off the core; this is why seals and gaskets are LSR |
| LSR — shrinkage | 2–4 %, held by the toolmaker | Higher than thermoplastics; tight-tolerance seals need a sampled tool before hardening |
All three are quoted by an engineer, not the instant engine — the tool concept (rotary, insert loading, cold-deck LSR) is decided with you before steel is cut.
Tolerances molded parts hold
Molding is repeatable, not precise: the tool is machined to ± 0.02 mm, but the plastic shrinks around it by a percentage that depends on the resin, the wall and the day.
| Dimension | Typical | Precision (on request) | Notes |
|---|---|---|---|
| Feature size, < 25 mm, in one half | ± 0.1 mm | ± 0.05 mm | Steel-safe features machined in the cavity; the FabDigit service standard |
| Feature size, 25–100 mm | ± 0.15 mm | ± 0.08 mm | Shrinkage scatter grows with length |
| Feature size, 100–300 mm | ± 0.3 mm | ± 0.15 mm | Glass-filled and amorphous resins hold tighter than PP / POM |
| Across the parting line | ± 0.15 mm extra | ± 0.08 mm | Two halves, two machined datums; keep mating fits in one half |
| Wall thickness | ± 0.1 mm | ± 0.05 mm | Core shift on deep cores adds to it |
| Flatness, 100 mm | 0.3–0.5 mm | 0.15 mm | Uniform walls and balanced cooling; ribs across the warp direction |
| Hole diameter (core pin) | ± 0.05 mm | ± 0.025 mm | Pins are ground; the hole is the most precise molded feature |
| Molded thread | class 6 / 2A | — | Tighter threads are tapped after molding |
Every "precision" figure is achieved by molding, measuring and re-cutting the steel (steel-safe design, first-article to correction) — that loop is the difference between a T1 sample and a production part, and it is priced.
- Keep mating fits in one half. Two bosses that must align to a PCB should be in the same half of the tool; across the parting line they drift.
- Tolerance the function. ± 0.05 mm on a snap-fit gap is normal; ± 0.05 mm on the outside of a housing is a re-quote.
- Design steel-safe. Make first-shot features slightly small (holes) or slightly large (pins) so the correction removes steel instead of welding it.
Surface finish, texture and cosmetics
The cavity finish is the part finish. Choose it before the tool is polished — repolishing costs more than polishing.
| Finish | Spec | Design consequence |
|---|---|---|
| Non-cosmetic (B-side) | SPI C-1 to D-3 / VDI 27–36 | Cheapest; ejector marks, gate vestige and witness lines allowed here |
| Standard cosmetic | SPI B-1 to B-3 | 600-grit paper finish; fine for painted or textured parts |
| High gloss / optical | SPI A-1 to A-3 | Diamond-buffed; needs hardened steel (S136), 2°+ draft, no weld lines on the face |
| Texture (bead / leather / grain) | VDI 3400 or Mold-Tech code + draft rule above | Hides sink, weld lines and scratches; add 1° draft per 0.025 mm depth |
| Molded-in colour | Pantone / RAL on a resin swatch | Colour shifts with wall thickness; clear parts show every flow line |
| Painting / plating / laser etch | secondary operation | Design jig-locating features; PP and POM need plasma treatment to hold paint |
Every finish, texture and secondary operation is a line on the engineer’s quote; texturing is applied after the tool is proven, so it never delays the T1 sample.
What to send for a tooling quote
Molding is engineer-quoted at FabDigit. The more of this you send, the fewer rounds before you have a tooling price and a piece price.
- The 3D solid (STEP), final wall design. The engineer runs a wall-thickness and draft check and proposes gates, parting line and ejection on it.
- Resin and colour. “PC/ABS, black, UL 94 V-0” beats “plastic”. If you have a preferred grade (Sabic Cycoloy C2950), say so — the tool is scaled to its shrinkage.
- Annual quantity and the first order. Decides aluminum vs P20 vs hardened steel and how many cavities. 500 parts a year is an aluminum tool; 50 k is a 4-cavity P20 tool.
- Cosmetic faces and finish. Mark A-surfaces on a drawing or screenshot; state SPI class or texture code.
- Critical dimensions and mating parts. A drawing with the 3–5 dimensions that matter; a STEP of the mating part is even better.
- Inserts, overmold, LSR. Insert part numbers and where they load; the soft-material grade and Shore hardness; whether the LSR part seals a fluid.
Tooling and piece-price ranges by tool grade and quantity — and where molding crosses over machining and cast urethane — are in the injection molding cost guide.
Injection molding design — FAQ
What wall thickness should an injection molded part have?
One uniform nominal wall, typically 1.2–3.5 mm for ABS and PC/ABS, 0.8–3.8 mm for PP and 0.8–3.0 mm for nylon and POM, held within ± 10 % across the part. Most housings sit at 2.0–2.5 mm. Stiffen with ribs (0.5–0.6 × T thick, ≤ 3 × T tall) rather than a thicker wall; above ~4 mm the cycle doubles and sink marks appear.
How much draft angle does injection molding need?
1° minimum on every face parallel to the pull direction, 2° preferred; deep cores need about 0.5° more per 25 mm of depth, and textured faces need an extra 1° per 0.025 mm of texture depth (a medium texture ≈ 3°). Zero-draft faces are possible with slides or polished cavities but are priced as tooling features.
What tolerances can injection molding hold?
± 0.1 mm on features under 25 mm within one half of the tool (± 0.05 mm precision on request), ± 0.15 mm at 25–100 mm, ± 0.3 mm at 100–300 mm, plus about ± 0.15 mm across the parting line. Core-pin holes hold ± 0.05 mm. Use DIN 16742 / ISO 20457 tolerance classes on the drawing and keep mating fits in one half.
How do I avoid sink marks?
Keep the wall uniform, keep ribs at 0.5–0.6 × the wall thickness, core out under bosses, transition thickness changes over 3 × the difference, and put the gate near the thickest section so it packs last. Texture hides what remains.
What is an undercut and how do I remove one?
Any feature the two tool halves cannot form as they open — a side hole, a snap hook facing sideways, an internal thread. Turn the feature toward the parting line so it becomes a shut-off, strip small hooks in flexible resins (bump-off), or accept a slide (roughly 10–25 % on tooling). Internal threads are best made as inserts.
Can FabDigit do insert molding, two-shot and LSR?
Yes — all three are quoted by an engineer with the tool concept (insert loading, rotary or core-back two-shot, cold-deck LSR) agreed before steel is cut. Design rules: ≥ 0.5 × insert diameter of plastic around inserts, chemically compatible or interlocked material pairs for two-shot, and 0.4–8 mm walls with little or no draft for LSR.
Aluminum or steel tooling?
Aluminum (7075) tools run 5,000–10,000 shots with unfilled resins (fewer with glass fill) and are the right choice to validate a design or produce up to a few thousand parts; P20 pre-hardened steel runs 100 k–1 M shots for standard production; S136 / H13 hardened steel for abrasive glass-filled resins, high-gloss cosmetics and 1 M+ shots. Your annual quantity decides it.
What should I send for an injection molding quote?
The STEP model with final walls, the resin and colour (grade if you have one), first-order and annual quantity, marked cosmetic faces with SPI class or texture code, a drawing with the critical dimensions, and any inserts or overmold materials. The engineer returns a tooling price, a piece price by quantity and a DFM report.
Design it for the tool, then let an engineer price the tool.
Upload the model — a FabDigit engineer returns a DFM report, a tooling quote by tool grade and piece prices by quantity, usually within two business days.