Injection MoldingDesign Guide
The design rules that decide whether a molded part comes out clean or fights you: wall thickness, draft, ribs, bosses, gates, and tolerance. These are what our DFM review checks before steel is cut.
Engineer reviewed quote
Wall thickness
Wall thickness is the single most important decision in a molded part. It drives cycle time, cost, strength, and every cosmetic defect you are trying to avoid. The rule that matters more than any number: keep the wall uniform. Molten plastic shrinks as it cools, and it shrinks unevenly wherever the wall changes thickness. That is what causes sink marks, warp, and locked-in stress.
Each resin has a workable range. Stay inside it, hold it constant across the part, and core out anything thick instead of leaving a solid mass.
| Resin | Recommended wall | Metric |
|---|---|---|
| ABS | 0.045" – 0.140" | 1.15 – 3.55 mm |
| Polycarbonate (PC) | 0.040" – 0.150" | 1.00 – 3.80 mm |
| Polypropylene (PP) | 0.025" – 0.150" | 0.65 – 3.80 mm |
| Polyethylene (PE) | 0.030" – 0.200" | 0.75 – 5.00 mm |
| Nylon (PA) | 0.030" – 0.115" | 0.75 – 2.90 mm |
| Acetal (POM) | 0.030" – 0.120" | 0.75 – 3.00 mm |
| Acrylic (PMMA) | 0.025" – 0.150" | 0.65 – 3.80 mm |
General ranges for cosmetic and structural parts. Filled grades and long flow lengths shift these; we confirm with a fill analysis during DFM.
Draft angle
Draft is the slight taper on any face that runs in the direction the part pulls out of the mold. Without it, the part drags against the steel as it ejects, scuffing the surface or sticking outright.
- /Smooth walls: 1 degree per side is a safe default.
- /Textured surfaces: Add roughly 1 degree for every 0.001" of texture depth.
- /Deep ribs and tall cores: Add extra draft so the part releases without drag.
- /Zero draft: Possible on some faces, but it costs tooling and cycle time. We flag it.
Ribs
Ribs add stiffness without adding wall thickness, which is exactly what you want, because thickening the wall causes sink. The trick is keeping the rib thin enough that it does not create a sink mark of its own on the show surface.
- /Thickness: 40 to 60 percent of the nominal wall.
- /Height: No more than about 3 times the wall thickness.
- /Draft: At least 0.5 degrees per side.
- /Spacing: Keep ribs at least 2 wall thicknesses apart.
Bosses
Bosses are the cylindrical posts that take screws, threaded inserts, or locating pins. They fail the same way thick walls do: too much material at the base pulls a sink on the far face.
- /Wall thickness: 40 to 60 percent of the nominal wall, same as ribs.
- /Outside diameter: Around twice the hole diameter for screw retention.
- /Base blend: A small radius, roughly 0.25 times the wall, to reduce stress.
- /Tall bosses: Support with gussets or ribs rather than a thicker post.
Gate location
The gate is where molten resin enters the cavity. Its position sets how the part fills, where weld lines land, and which face carries the gate vestige. You do not always control it, but it is worth understanding what the toolmaker is balancing.
- /Fill from thick to thin: Gate at the heaviest section so the melt packs out before it freezes off.
- /Keep it off cosmetic faces: Every gate leaves a vestige. Put it where it will not show.
- /Mind weld lines: Where two flow fronts meet they form a weld line. Steer them away from load paths.
- /Balance multi-cavity fills: Runner layout keeps every cavity filling evenly. Unbalanced fills mean inconsistent parts.
Tolerances
Tolerance in molding comes from three places: the steel, the resin shrink, and how the part is designed. Hardened production tools hold tighter numbers than soft prototype tools, and features on one side of the parting line hold tighter than features that cross it.
| Tool type | Typical tolerance |
|---|---|
| Prototype (MUD) | ±0.005" – ±0.010" |
| Bridge | ±0.003" – ±0.008" |
| Production (SPI) | ±0.002" – ±0.005" |
Want the tooling tiers side by side, including volume and lead time? See prototype vs production tooling.
Common questions.
It depends on the resin. Most engineering thermoplastics mold cleanly between 0.040" and 0.140" (1 to 3.5 mm). The bigger rule is uniformity: keep the wall as consistent as possible. Thick-to-thin transitions cause sink, warp, and internal stress no matter which resin you pick.
One degree per side is a safe default for smooth walls. Textured surfaces need more, roughly one additional degree for every 0.001" of texture depth. Deep ribs and tall cores want extra draft so parts eject without drag marks. Zero-draft is possible but adds tooling cost and cycle time, so we flag it in DFM.
The outside of a thick section cools and solidifies before the core does. As the core shrinks it pulls the surface inward, creating a sink mark, or forms a void inside. Coring out thick sections to a uniform wall fixes both and shortens cycle time.
Keep ribs and boss walls at 40 to 60 percent of the nominal wall thickness. Go thicker and you get a sink mark on the opposite face. Ribs should be no taller than about three times the wall, with at least 0.5 degrees of draft. Tall bosses get supported with gussets or ribs rather than thickened.
Production tooling in hardened steel holds roughly +/-0.002" to +/-0.005" on well-designed features; prototype tooling runs +/-0.005" to +/-0.010". Tight tolerances on thin walls or across the parting line are harder and we call them out during the review.
Yes. Every project gets a 12-point DFM review, resin, gate scheme, draft, wall thickness, ejection, and more, before any steel is cut. The point is to find cost and quality issues while they are still cheap to fix.
Related
Ready to mold the part?
Send the CAD and an engineer reviews the design against every rule above, then quotes it. See the full injection molding process.
Get a Quote