Injection molding design guidelines

Injection molded parts typically use a uniform nominal wall of 0.040–0.150 in (1.0–3.8 mm) that varies no more than about 15%, 1–2° of draft, ribs 50–60% of the adjoining wall, and inside radii at least half the wall. General tolerances run about ±0.005 in (±0.13 mm). Semi-crystalline resins shrink 1.5–2.5% and need looser limits than amorphous resins.

Try the interactive lab Check a part in the builder

Nominal wall: 0.040–0.150 in
Draft: 1–2° typical
Rib thickness: 50–60% of wall
General tolerance: ±0.005 in (±0.13 mm)

SSG MFG · design guideDG-01 · 12 rules

What are the injection molding design rules?

12 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.

Design rules and typical values
#	Rule	Typical value
01	Keep walls uniform0.040–0.150 in (1.0–3.8 mm) nominal, varying no more than about 15%; transition over 3× the thickness change	0.040–0.150 in (1.0–3.8 mm) nominal, varying no more than about 15%; transition over 3× the thickness change
02	Core out thick sectionsKeep every section under 0.25 in (6 mm); replace solid mass with ribs on a nominal wall	Keep every section under 0.25 in (6 mm); replace solid mass with ribs on a nominal wall
03	Add draft in the line of draw1–2° typical; 0.5° minimum on polished walls; add 1–1.5° per 0.001 in (0.025 mm) of texture depth	1–2° typical; 0.5° minimum on polished walls; add 1–1.5° per 0.001 in (0.025 mm) of texture depth
04	Radius inside and outside cornersInside radius at least 0.5× wall; outside radius equals inside radius plus wall	Inside radius at least 0.5× wall; outside radius equals inside radius plus wall
05	Size ribs to the wallRib thickness 50–60% of the adjoining wall; height up to 3× wall; spacing at least 2× wall; 0.5–1° draft per side	Rib thickness 50–60% of the adjoining wall; height up to 3× wall; spacing at least 2× wall; 0.5–1° draft per side
06	Design bosses to avoid sinkBoss wall no more than 60% of nominal wall; boss OD about 2× hole ID; base radius about 0.25× wall; tie tall bosses to walls with ribs	Boss wall no more than 60% of nominal wall; boss OD about 2× hole ID; base radius about 0.25× wall; tie tall bosses to walls with ribs
07	Limit the depth of cored holesBlind holes up to about 3× diameter, 2× under 0.188 in (4.8 mm); through holes up to about 6× with pins supported on both halves	Blind holes up to about 3× diameter, 2× under 0.188 in (4.8 mm); through holes up to about 6× with pins supported on both halves
08	Design out undercuts firstEach slide or lifter typically adds $1,000–$5,000 to tool cost; flexible resins such as PP and TPE can strip small bumps of a few percent of diameter	Each slide or lifter typically adds $1,000–$5,000 to tool cost; flexible resins such as PP and TPE can strip small bumps of a few percent of diameter
09	Place the parting line and gate earlyParting line on an edge or step, off cosmetic faces; gate into the thickest section; knit lines away from load and show faces	Parting line on an edge or step, off cosmetic faces; gate into the thickest section; knit lines away from load and show faces
10	Set tolerances by resin shrinkAmorphous resins (ABS, PC, PMMA) shrink about 0.4–0.8%; semi-crystalline PP, POM and PA shrink about 1.5–2.5%; glass fill adds direction-dependent shrink	Amorphous resins (ABS, PC, PMMA) shrink about 0.4–0.8%; semi-crystalline PP, POM and PA shrink about 1.5–2.5%; glass fill adds direction-dependent shrink
11	Hold critical dimensions in one mold halfDimension from datums the tool forms in one half; add about ±0.002–0.004 in (±0.05–0.10 mm) across the parting line or a slide	Dimension from datums the tool forms in one half; add about ±0.002–0.004 in (±0.05–0.10 mm) across the parting line or a slide
12	Call surface finish by SPI gradeSPI A-1 to A-3 for optical and gloss; B-1 to B-3 for general cosmetic; C and D grades or texture for non-cosmetic and hidden faces	SPI A-1 to A-3 for optical and gloss; B-1 to B-3 for general cosmetic; C and D grades or texture for non-cosmetic and hidden faces

These build on the short list on the injection molding process page, with the failure each rule prevents and a drawing for each.

What happens when a rib gets too thick?

Thicken a rib or boss past about 60% of the nominal wall and sink shows up on the face opposite it. Double the wall and cooling time roughly quadruples, because it grows with the square of thickness.

WALL 0.100 in · RIB 55% OF WALL

Wall: 0.100 in(2.54 mm)
Rib at the root: 0.055 in(1.40 mm)
Rib height limit, 3T: 0.300 in
Cooling time, estimate: 10.8 s1.0× a 0.100 in wall

Works: uniform, sink-free

A 55% rib on a 0.100 in wall stiffens the part without a thick spot at the root.

Cooling time is the standard one-dimensional slab estimate with typical resin values. Real cycles add fill, pack and mold-open time; your molder's number governs.

Why does each rule matter?

Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.

Rule 01

Keep walls uniform

0.040–0.150 in (1.0–3.8 mm) nominal, varying no more than about 15%; transition over 3× the thickness change

Why: Uneven walls cool at different rates and pull the part out of shape. Cooling time grows with the square of wall thickness, so the thickest wall sets the cycle.
If you ignore it: Sink marks, internal voids and warp appear where thick meets thin, and the whole part runs at the cycle of its thickest section.

Fig. 1Uniform wall

Do. Every wall within about 15% of nominal T, so the whole part cools and shrinks at one rate.

Avoid. A section twice as thick cools last: it pulls a sink mark into the face above it and can leave a void inside.

Rule 02

Core out thick sections

Keep every section under 0.25 in (6 mm); replace solid mass with ribs on a nominal wall

Why: Thick sections shrink as they cool long after the gate freezes, and no amount of pack pressure can feed them.
If you ignore it: Deep sink on the show face, voids you find only when the part is sectioned, and cycle times two to four times longer than needed.

Fig. 2Core out thick sections

Do. Hollow the section from the back into walls and ribs at T: same stiffness at the face, a fraction of the cooling time.

Avoid. A solid thick section takes several times longer to cool and still sinks at the surface and voids in the middle.

Rule 03

Add draft in the line of draw

1–2° typical; 0.5° minimum on polished walls; add 1–1.5° per 0.001 in (0.025 mm) of texture depth

Why: Plastic shrinks onto cores as it cools. Draft breaks the grip so the part releases without scraping.
If you ignore it: Parts stick on the core, drag marks scuff textured faces, and ejector pins push white stress marks or dents into the part.

Fig. 3Draft angle

Do. Walls taper by the draft angle in the line of draw; each side moves in by H × tan θ, and the part slides off the core.

Avoid. With zero draft the part grips the core as it shrinks: drag marks, scuffed texture, and ejector pins that dent or punch through.

Rule 04

Radius inside and outside corners

Inside radius at least 0.5× wall; outside radius equals inside radius plus wall

Why: Matched radii keep the wall constant through the corner and let resin flow around it without a pressure drop.
If you ignore it: Parts crack at sharp inside corners under load or on snap-fit assembly, and corners warp inward from uneven cooling.

Fig. 4Inside and outside radii

Do. Inside radius at least half the wall and outside radius equal to inside plus T: the corner stays at thickness T and flow turns smoothly.

Avoid. A sharp inside corner concentrates stress about 3× and the corner runs thick: cracks start there, and it cools last.

Rule 05

Size ribs to the wall

Rib thickness 50–60% of the adjoining wall; height up to 3× wall; spacing at least 2× wall; 0.5–1° draft per side

Why: A rib thicker than about 60% of the wall creates a thick spot where it meets the wall. Tall ribs are hard to fill and stick in the tool.
If you ignore it: Sink lines appear on the face opposite each rib, and tall thin ribs short-shot or stay behind in the tool.

Fig. 5Rib proportions

Do. A rib 50–60% of the wall at its base, up to 3× the wall tall, with a small root radius: stiffness without a thick spot.

Avoid. A rib as thick as the wall doubles the mass where it joins, and the face behind it sinks.

Rule 06

Design bosses to avoid sink

Boss wall no more than 60% of nominal wall; boss OD about 2× hole ID; base radius about 0.25× wall; tie tall bosses to walls with ribs

Why: A boss is a thick ring of plastic sitting on a wall. Coring it and keeping its wall thin controls sink while the screw still bites.
If you ignore it: A sink ring shows on the show face behind every boss, and freestanding bosses crack or strip when the screw is driven.

Fig. 6Boss design

Do. Boss OD about 2× the hole, boss wall at most 60% of T, cored down to the wall and braced with gussets.

Avoid. A thick, solid boss is a heat sink in the middle of the part: sink on the show face and a void around the screw.

Rule 07

Limit the depth of cored holes

Blind holes up to about 3× diameter, 2× under 0.188 in (4.8 mm); through holes up to about 6× with pins supported on both halves

Why: Core pins are cantilevered in the melt stream. Long, thin pins deflect and run hot.
If you ignore it: Core pins bend or break, holes come out oval or off-position, and the tool comes out of production for repair.

Fig. 7Cored hole depth

Do. A drafted core pin no deeper than about 4× its diameter stays straight under injection pressure and releases cleanly.

Avoid. A long, thin pin deflects under metal pressure and heat checks; holes run off-position and pins break in production.

Rule 08

Design out undercuts first

Each slide or lifter typically adds $1,000–$5,000 to tool cost; flexible resins such as PP and TPE can strip small bumps of a few percent of diameter

Why: Anything that blocks straight pull needs a side action. Pass-through cores and shut-offs often replace a slide at no cost.
If you ignore it: The tool quote climbs, cycle time grows, and slides wear, flash and need maintenance for the life of the program.

Fig. 8Undercuts and side actions

Do. Where an undercut is worth it, a slide pulls sideways before ejection. Better still, move the feature into the line of draw or use a pass-through core.

Avoid. A side hole with no side action locks the part in the steel; every slide or lifter added to fix it adds tool cost and cycle time.

Rule 09

Place the parting line and gate early

Parting line on an edge or step, off cosmetic faces; gate into the thickest section; knit lines away from load and show faces

Why: The parting line leaves a witness and possible flash, and the gate leaves a vestige. Flow from the gate sets where knit lines form.
If you ignore it: Flash and gate marks land on the show face, and knit lines crack under load or show as lines on painted and clear parts.

Fig. 9Parting line

Do. A flat parting line at the largest section, off sealing and cosmetic faces, with critical dimensions inside one die half.

Avoid. A dimension across the parting line carries die-half mismatch and flash thickness, typically another ±0.004 in (±0.10 mm) or more.

Rule 10

Set tolerances by resin shrink

Amorphous resins (ABS, PC, PMMA) shrink about 0.4–0.8%; semi-crystalline PP, POM and PA shrink about 1.5–2.5%; glass fill adds direction-dependent shrink

Why: Semi-crystalline resins shrink more, and less predictably, so the same tolerance costs more tool iterations.
If you ignore it: Parts fall out of tolerance at T1, steel is recut several times, and glass-filled parts warp along the flow direction.

Standard: ISO 20457

Fig. 10Shrink and warp

Do. The cavity is cut oversize by the resin's shrink rate, and even walls and gating let the part shrink the same amount everywhere.

Avoid. Different shrink across and along the flow, or between thick and thin areas, bows the part out of flat.

Rule 11

Hold critical dimensions in one mold half

Dimension from datums the tool forms in one half; add about ±0.002–0.004 in (±0.05–0.10 mm) across the parting line or a slide

Why: Mold closure and slide travel add their own variation to any dimension that crosses them.
If you ignore it: Features that cross the parting line drift out of tolerance shot to shot and fail inspection that the tool cannot fix.

Standard: ASME Y14.5

Fig. 11A complete drawing package

Do. Every requirement is on the drawing: general tolerance, material by specification, finish by specification, critical dimensions and revision.

Avoid. Whatever the drawing leaves blank, the supplier decides, usually with the cheapest local equivalent.

Rule 12

Call surface finish by SPI grade

SPI A-1 to A-3 for optical and gloss; B-1 to B-3 for general cosmetic; C and D grades or texture for non-cosmetic and hidden faces

Why: Polish grade sets hand-polish hours on the tool, and texture depth sets how much draft the wall needs.
If you ignore it: An unspecified finish gets quoted and built to the toolmaker's default, and a late texture change forces a draft recut in steel.

Standard: SPI mold finish guide (A-1 to D-3)

What tolerances can injection molding hold?

Typical values for unfilled amorphous resins in a stable production process. Semi-crystalline and glass-filled resins need the wider end of each range. Tight values need tuned steel, capability studies and often more than one tool iteration.

Typical and tight tolerances with the cost of going tight
Feature	Typical	Tight	Cost of tight
Linear, under 1 in (25 mm)	±0.005 in (±0.13 mm)	±0.002 in (±0.05 mm)	Moderate
Linear, 1–6 in (25–150 mm)Resin shrink variation grows with length.	±0.005 in + 0.002 in per in	±0.003 in + 0.001 in per in	Moderate
Linear, over 6 in (150 mm)	±0.3% of length	±0.15% of length	High
Hole diameter, under 0.5 in (13 mm)	±0.003 in (±0.08 mm)	±0.001 in (±0.025 mm)	Moderate
Wall thickness	±0.005 in (±0.13 mm)	±0.002 in (±0.05 mm)	Moderate
Flatness, up to 3 in (75 mm)Needs uniform walls and balanced cooling; ribs help.	0.010 in (0.25 mm)	0.004 in (0.10 mm)	High
Across parting line or slide	Add ±0.004 in (±0.10 mm)	Add ±0.002 in (±0.05 mm)	Moderate

Basis: ISO 20457 / SPI tolerance guidelines. Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.

How does the material change the rules?

The same injection molding rules shift with the alloy or compound.

Polypropylene (PP)
PP shrinks about 1.5–2.5% and can warp on long flat walls, so hold wider tolerances and rib large panels. It flexes enough to strip small undercuts and to make living hinges about 0.008–0.015 in (0.2–0.4 mm) thick.
Nylon 66, 30% glass-filled (PA66-GF30)
Glass fill shrinks less across flow than along it, which warps flat parts unless walls are uniform and gates are placed with care. The glass is abrasive, so budget hardened steel rather than aluminum or P20 for long runs.
Polycarbonate (PC)
PC shrinks about 0.5–0.7% and holds tight tolerances, but it is notch sensitive, so keep inside radii at least 0.5× wall. It needs higher melt temperature and more draft on textured faces than ABS.
Acetal (POM)
Acetal shrinks about 2% and sinks readily behind thick features, so hold ribs and boss walls near 50% of nominal. Its low friction and fatigue resistance make it a common choice for gears and snap fits.
ABS
ABS shrinks about 0.4–0.7% and is forgiving to mold, which makes it a reference resin for wall and rib rules. It textures and paints well, but draft still has to grow with texture depth.
PEEK (polyether ether ketone)
PEEK molds at about 700–750 °F (370–400 °C) with a mold temperature near 350 °F (175 °C), so tools are hardened steel and cycle windows are narrow. Keep walls toward the thin end of the range to control cost at $40 or more per lb.

Injection molding design questions

What is the minimum wall thickness for injection molding?

Most resins can fill walls of about 0.020 in (0.5 mm) over short flow lengths, but a practical production minimum is usually 0.030–0.040 in (0.8–1.0 mm). Thin-wall parts need high injection speed, more gates and often a larger press. Flow length to wall ratio matters as much as thickness: easy-flow PP and nylon reach further than PC at the same wall.

How much draft does an injection molded part need?

Plan on 1–2° per side for most walls. Polished walls can go as low as 0.5°, and deep cores or ribs benefit from more. Textured walls need an extra 1–1.5° for every 0.001 in (0.025 mm) of texture depth, so a medium texture often needs 3° or more. Inside walls that the part shrinks onto need more draft than outside walls.

How thick should ribs be on a molded part?

Ribs are typically 50–60% of the wall they join, so a 0.100 in (2.5 mm) wall takes ribs of about 0.050–0.060 in (1.3–1.5 mm). Keep them no taller than about 3× the wall, space them at least 2× the wall apart, and give them 0.5–1° of draft per side. Use two short ribs rather than one tall one.

What causes sink marks on injection molded parts?

Sink marks form where a thick section keeps shrinking after the surface has frozen and pulls the skin inward. The usual causes are ribs or boss walls thicker than about 60% of the nominal wall, solid sections over 0.25 in (6 mm), and gates too far from the thick area. Coring out the section fixes the cause; more pack pressure only masks it.

How do you design snap fits for injection molding?

Size the cantilever so its bending strain at full deflection stays below the resin's allowable limit, which for many unfilled resins is a few percent for a one-time assembly and less for repeated use. Taper the beam from root to tip, radius the root to at least half the beam thickness, and design the catch so it molds with a pass-through core instead of a slide.

What tolerance standard applies to injection molded parts?

ISO 20457 is the current international standard for tolerances on molded plastic parts, replacing DIN 16901 in many shops. In the US, drawings often use a title-block tolerance such as ±0.005 in (±0.13 mm) with tighter callouts on critical features. Either way, state the resin, because shrink sets what is achievable.

Check your part against these rules.

Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run injection molding every day.

Build a part Send a drawing

Injection molding design guidelines

Rule

Keep walls uniform0.040–0.150 in (1.0–3.8 mm) nominal, varying no more than about 15%; transition over 3× the thickness change

Core out thick sectionsKeep every section under 0.25 in (6 mm); replace solid mass with ribs on a nominal wall

Add draft in the line of draw1–2° typical; 0.5° minimum on polished walls; add 1–1.5° per 0.001 in (0.025 mm) of texture depth

Radius inside and outside cornersInside radius at least 0.5× wall; outside radius equals inside radius plus wall

Size ribs to the wallRib thickness 50–60% of the adjoining wall; height up to 3× wall; spacing at least 2× wall; 0.5–1° draft per side

Design bosses to avoid sinkBoss wall no more than 60% of nominal wall; boss OD about 2× hole ID; base radius about 0.25× wall; tie tall bosses to walls with ribs

Limit the depth of cored holesBlind holes up to about 3× diameter, 2× under 0.188 in (4.8 mm); through holes up to about 6× with pins supported on both halves

Design out undercuts firstEach slide or lifter typically adds $1,000–$5,000 to tool cost; flexible resins such as PP and TPE can strip small bumps of a few percent of diameter

Place the parting line and gate earlyParting line on an edge or step, off cosmetic faces; gate into the thickest section; knit lines away from load and show faces

Set tolerances by resin shrinkAmorphous resins (ABS, PC, PMMA) shrink about 0.4–0.8%; semi-crystalline PP, POM and PA shrink about 1.5–2.5%; glass fill adds direction-dependent shrink

Hold critical dimensions in one mold halfDimension from datums the tool forms in one half; add about ±0.002–0.004 in (±0.05–0.10 mm) across the parting line or a slide

Call surface finish by SPI gradeSPI A-1 to A-3 for optical and gloss; B-1 to B-3 for general cosmetic; C and D grades or texture for non-cosmetic and hidden faces

Feature

Typical

Tight

Cost of tight

Linear, under 1 in (25 mm)

±0.005 in (±0.13 mm)

±0.002 in (±0.05 mm)

Moderate

Linear, 1–6 in (25–150 mm)Resin shrink variation grows with length.

±0.005 in + 0.002 in per in

±0.003 in + 0.001 in per in

Moderate

Linear, over 6 in (150 mm)

±0.3% of length

±0.15% of length

High

Hole diameter, under 0.5 in (13 mm)

±0.003 in (±0.08 mm)

±0.001 in (±0.025 mm)

Moderate

Wall thickness

±0.005 in (±0.13 mm)

±0.002 in (±0.05 mm)

Moderate

Flatness, up to 3 in (75 mm)Needs uniform walls and balanced cooling; ribs help.

0.010 in (0.25 mm)

0.004 in (0.10 mm)

High

Across parting line or slide

Add ±0.004 in (±0.10 mm)

Add ±0.002 in (±0.05 mm)

Moderate

What are the injection molding design rules?

What happens when a rib gets too thick?