---
type: chart
title: "Injection Molding Design Guidelines"
tables: 3
url: https://manufacturingprocesses.org/charts/injection-molding-design-guidelines
---

# Injection Molding Design Guidelines

Recommended wall thickness by polymer, draft angle by surface finish and texture, and the rib, boss and corner ratios that keep a molded part free of sink and warp.

**Uniform wall thickness is the single highest-leverage decision in a
molded part.** Non-uniform walls cause sink, voids, warp and differential
shrink. Where a thickness change is unavoidable, transition gradually — a
3:1 taper minimum — and keep the step under 25% of nominal for amorphous
resins (ABS, PC, PS) and under 15% for semi-crystalline resins (PA, PP, PBT,
POM), which shrink more.

Most consumer and industrial parts land at 2.0–3.0 mm (0.080–0.120 in).
High-flow resins such as PP, POM and LCP hold 1.0–1.5 mm; low-flow resins
such as PC and glass-filled nylon generally want 2.0–3.0 mm.

Draft is measured **per side**, from the direction of mold opening. Zero
draft is possible only on shallow, highly polished faces and always risks
drag marks and ejector damage. The texture rule that matters: add **1–1.5°
of draft for every 0.001 in (0.025 mm) of texture depth**, on top of the base
draft — and ask the texture house for the actual depth rather than guessing
from the SPI or MT code. For deep cores over 50 mm of draw, add roughly 0.5°
per additional 25 mm of depth.

All rib and boss ratios below are relative to the **nominal wall thickness
T**.

## Recommended wall thickness by polymer

| Polymer | Min (in) | Max (in) | Min (mm) | Max (mm) | Flow behaviour |
| --- | --- | --- | --- | --- | --- |
| ABS | 0.045 | 0.14 | 1.14 | 3.56 | Medium flow, forgiving |
| Acetal (POM) | 0.03 | 0.12 | 0.76 | 3.05 | High flow, thin walls OK, high shrink |
| Acrylic (PMMA) | 0.025 | 0.5 | 0.64 | 12.7 | Tolerates thick sections — better than PC for thick optics |
| Liquid crystal polymer (LCP) | 0.03 | 0.12 | 0.76 | 3.05 | Very high flow, can go very thin |
| Long-fiber reinforced | 0.075 | 1 | 1.9 | 25.4 | Thick sections; strong but warp-prone |
| Nylon (PA) | 0.03 | 0.115 | 0.76 | 2.92 | High flow unfilled; glass-filled needs thicker walls |
| Polycarbonate (PC) | 0.04 | 0.15 | 1.02 | 3.81 | Low flow, needs thicker walls and short flow paths |
| Polyester (PBT / PET) | 0.025 | 0.125 | 0.64 | 3.17 | Medium-high flow, high shrink |
| Polyethylene (PE) | 0.03 | 0.2 | 0.76 | 5.08 | High flow, high shrink |
| Polyphenylene sulfide (PPS) | 0.02 | 0.18 | 0.51 | 4.57 | High flow, very thin capable |
| Polypropylene (PP) | 0.025 | 0.15 | 0.64 | 3.81 | High flow, thin walls OK, high shrink |
| Polystyrene (PS) | 0.035 | 0.15 | 0.89 | 3.81 | Easy flow, low shrink |
| Polyurethane (PU) | 0.08 | 0.75 | 2.03 | 19.05 | Thick sections, elastomeric |

## Draft angle by surface condition (degrees per side)

| Surface condition | Min draft (°) | Max draft (°) |
| --- | --- | --- |
| Shutoff / shallow feature (<1mm) | 0.25 | 0.5 |
| SPI A-1/A-2/A-3 diamond polish | 1.5 | 2 |
| SPI B-1/B-2/B-3 paper finish | 1 | 2 |
| SPI C-1/C-2/C-3 stone finish | 1.5 | 2.5 |
| General default, untextured | 1 | 2 |
| SPI D-1/D-2/D-3 dry blast | 2 | 3 |
| Light texture (MT-11010/11020) | 3 | 3 |
| Medium texture (MT-11030) | 3 | 5 |
| Heavy texture / leather grain | 5 | 7 |
| Ribs and internal bosses | 0.5 | 1.5 |

## Rib, boss and corner ratios (relative to nominal wall T)

| Feature | Guideline | Why |
| --- | --- | --- |
| Rib thickness at base | 0.5 – 0.6 × T | Above 0.6 T a sink mark shows on the opposite face |
| Rib thickness (textured or cosmetic face) | 0.4 – 0.5 × T | Extra margin against sink |
| Rib height | ≤ 3 × T | Taller ribs are hard to fill and to eject |
| Rib spacing, center to center | ≥ 2 × T | Closer spacing traps heat and creates a thick section |
| Rib base fillet | 0.25 – 0.5 × T | Smaller cracks; larger creates a thick spot |
| Rib draft | 0.5 – 1.5° per side | Needed to eject the rib |
| Boss outside diameter | 2 – 2.5 × screw major diameter | Resists hoop stress from the screw |
| Boss wall thickness | 0.5 – 0.6 × T | Same sink rule as ribs |
| Boss standoff from a wall | Connect with a rib or gusset, not a thick blend | Avoids a heavy junction that sinks |
| Internal corner radius | ≥ 0.5 × T | Sharp internal corners are the number one stress riser |
| External corner radius | Internal radius + T | Keeps the wall uniform through the corner |
| Hole to edge, hole to hole | ≥ 2 × hole diameter | Avoids weak, hard-to-fill webs |

## Notes

**Polishing does not reliably reduce the draft requirement.** Some sources
say an SPI A polished surface can go as low as 0.5°; others state a 1.5–2°
minimum for SPI A-1/A-2. The higher figure is used here, because a high
polish increases vacuum adhesion between part and core. The sub-0.5° case is
listed separately and restricted to shallow features. Under-drafting a deep
polished core is a common and expensive mistake.

**The wall thickness table comes from a single primary source** (Protolabs),
with the millimeter columns computed at 25.4 mm/in. Five rows — ABS, PC, PP,
nylon and acetal — were independently spot-checked and matched. The
remaining eight rows (acrylic, LCP, long-fiber, polyester, PE, PPS, PS, PU)
are single-source.

**The SPI finish grade to draft mapping is industry practice, not a
standard.** SPI defines the mold finish, not a draft requirement. Confirm
with the moldmaker for the specific texture and draw depth.

**Sink-mark rule of thumb:** any local section thicker than about 60% of the
nominal wall will show on the opposite surface of a cosmetic face. Core it
out or rib it instead of leaving solid mass.

The rib thickness ratio of 0.5–0.6 × T was confirmed by two sources. The
tightened 0.4–0.5 × T figure for cosmetic and textured faces is common shop
practice rather than a published standard, as are the rib height, spacing,
fillet, boss and corner-radius ratios.

## FAQ

### What wall thickness should I use for an injection molded part?

Most parts land at 2.0–3.0 mm. ABS runs 1.14–3.56 mm, polycarbonate 1.02–3.81 mm and polypropylene 0.64–3.81 mm. The stronger rule is uniformity: hold variation within 25% of nominal for amorphous resins and 15% for semi-crystalline ones.

### How much draft angle does an injection molded part need?

1–2° per side is the general default on an untextured wall. A dry-blast SPI D finish wants 2–3°, light texture wants at least 3°, and heavy leather grain wants 5–7° or more. Ribs and internal bosses can run 0.5–1.5°.

### How much extra draft does texture need?

Add 1–1.5° for every 0.001 in (0.025 mm) of texture depth, on top of the base draft. Ask the texture house for the actual depth rather than inferring it from the SPI or MT code.

### How thick should a rib be?

0.5–0.6 × the nominal wall at the base, dropping to 0.4–0.5 × on a textured or cosmetic face. Anything above 0.6 × will show as a sink mark on the opposite surface. Keep rib height at or below 3 × wall and spacing at 2 × wall or more.

### What causes sink marks?

A local section thicker than roughly 60% of the nominal wall. It cools last, shrinks after the surface has frozen, and pulls the opposite face inward. The fix is to core the thick section out and replace it with ribs.

### How big should a boss be for a self-tapping screw?

Outside diameter 2–2.5 × the screw's major diameter, with a boss wall of 0.5–0.6 × the nominal part wall. Connect the boss to a nearby wall with a rib or gusset rather than a thick blend, which would create a heavy junction that sinks.

### What internal corner radius should I use?

At least 0.5 × the nominal wall thickness. Sharp internal corners are the leading stress riser in a molded part and also restrict melt flow. Make the external radius the internal radius plus one wall thickness so the wall stays uniform through the corner.

## Sources

- [Protolabs — Improving Part Design with Uniform Wall Thickness (Plastic Wall Thickness Chart)](https://www.protolabs.com/resources/design-tips/improving-part-design-with-uniform-wall-thickness/)
- [3D DFM — Injection Molding Design Guidelines: Wall Thickness, Ribs & Draft](https://3ddfm.com/)
- [Evok Polymer — Injection Molding Draft Angle: Complete Design Guide](https://evokpoly.com/)

## Related processes

- [Injection Molding](https://manufacturingprocesses.org/processes/forming/injection-molding.md)
- [Overmolding](https://manufacturingprocesses.org/processes/forming/overmolding.md)
- [Insert Molding](https://manufacturingprocesses.org/processes/forming/insert-molding.md)
- [Compression Molding](https://manufacturingprocesses.org/processes/forming/compression-molding.md)
- [Liquid Silicone Rubber (LSR) Molding](https://manufacturingprocesses.org/processes/forming/liquid-silicone-rubber-lsr-molding.md)

## Related charts

- [Surface Finish Chart](https://manufacturingprocesses.org/charts/surface-finish-chart.md)
- [Common Engineering Material Properties](https://manufacturingprocesses.org/charts/material-properties.md)

---

*Source: [Manufacturing Processes](https://manufacturingprocesses.org/charts/injection-molding-design-guidelines)*

*Last updated: August 11, 2026*