Before we cut a single line of steel for a new injection mold, our engineering team always conducts a thorough review of the plastic part design. In our 30-plus years of manufacturing experience, we’ve seen how seemingly small design decisions — a wall that’s slightly too thick here, a corner left sharp there — can turn into costly rework, scrapped parts, or extended lead times down the line.
This guide walks through the core design principles our team applies every day. Whether you’re designing a part for the first time or troubleshooting an existing design, these guidelines will help you avoid the most common pitfalls.
1. Wall Thickness: Keep It Uniform
Uniform wall thickness is the single most important rule in injection molding design. When wall sections vary significantly, thick and thin areas cool at different rates inside the mold. Thin sections solidify quickly, while thick sections stay molten longer and continue to shrink. The result? Warping, sink marks, and dimensional instability — problems that are difficult to fix after the mold is built.
Why Variation Causes Problems
Plastics have a high coefficient of thermal expansion. Even a modest temperature difference between a thick and a thin wall section creates enough differential shrinkage to distort a part after ejection. In severe cases, excessive shrinkage in a thick section can create internal voids — air pockets trapped inside the part — even with extended packing and cooling times.
Gating Into Thick Sections
When a design requires different wall thicknesses, gating location matters enormously. We always recommend gating into the thicker section first. This allows the packing pressure to reach the thin sections before the thick wall solidifies, improving surface quality and dimensional control. Gating into a thin section that flows into a thick one does the opposite — the thin wall freezes off prematurely, cutting off packing pressure to the thick section and causing sink or voids.
Transitioning Between Thicknesses
When abrupt changes in wall thickness are unavoidable, taper the transition gradually — ideally over a distance of at least three times the wall thickness. A sudden step creates a stress concentration and a sharp flow front that can trap air or cause weld lines.
Practical Alternatives to Thick Walls
When a part needs extra stiffness in certain areas, our first instinct is not to increase wall thickness. Thicker walls mean longer cooling times (cooling time scales roughly with the square of wall thickness), more material, and higher cycle costs. Instead, we typically recommend:
- Ribs — thin vertical walls perpendicular to the main wall. They add stiffness with minimal material and short cooling times.
- Rib-and-grid structures — for large flat panels that need stiffness in multiple directions, a grid of short, thin ribs on one side is far more efficient than increasing wall thickness.
- Dimpled or waffle surfaces — dimples reduce effective thickness while adding surface area and improving mold cooling efficiency.
2. Rib Design: Stiffness Without the Penalty
Ribs are one of the most effective tools in injection mold design. Done correctly, a ribbed thin-wall design can match the stiffness of a solid thicker part while using significantly less material and running on a much shorter cycle.
We consistently specify rib thickness at no more than 70% of the nominal wall thickness. If a rib is as thick as the wall it attaches to, the junction creates a local mass concentration that cools slowly, pulling the surface inward and creating a visible sink mark on the opposite side of the part.
For highly filled materials — glass-fiber or mineral-filled resins — shrinkage is lower, so slightly thicker ribs may be acceptable. For unfilled materials, staying at or below 70% is essential.
Rib Height and Spacing
In our standard rib designs, we typically target:
- Height: 2–4× the nominal wall thickness. Taller ribs add more bending stiffness but require more careful attention to draft and ejection.
- Spacing: 8–10× the wall thickness between parallel ribs. Ribs spaced too closely create deep, narrow channels that are difficult to cool and polish.
Draft on Ribs
All ribs need draft to allow the part to release without sticking. For standard unfilled resins with a polished finish, 1° of draft per side is typically sufficient. For deep ribs, glass-filled materials, or textured surfaces, we increase draft to 1.5–2° per side. Very short ribs (under 3mm) can sometimes be molded at zero draft, but we treat this as the exception rather than the rule.
3. Boss Design: Getting Fastener Points Right
Bosses — cylindrical posts used for screw attachment, press-fit inserts, or locating features — are present in nearly every plastic enclosure we manufacture. They’re also one of the most frequently over-designed features we see in customer submissions.
Wall Thickness Applies Here Too
The same 70% rule that governs ribs applies to boss walls. A boss whose wall thickness equals the surrounding nominal wall will create a heavy section at the base, leading to sink marks on the opposite surface. We design boss walls to 70% of nominal wall thickness, using gussets and connecting ribs for structural support rather than relying on mass.
Supporting Bosses Properly
A freestanding boss on a flat surface is mechanically weak — it will flex or crack under torque during screw insertion. Our standard approach is to connect bosses to nearby walls with ribs, and to reinforce the boss itself with gussets positioned at 90° or 120° intervals.
Ejection Considerations
Tall, deep bosses can stick in the mold during ejection. We use ejector sleeves (rather than simple pins) for bosses that exceed 10mm in height, as sleeves distribute ejection force evenly around the boss circumference and reduce the risk of deformation or cracking.
Screw and Insert Compatibility
For self-tapping screws, the pilot hole diameter is typically 80–90% of the screw’s major diameter, depending on the resin. For ultrasonic or heat-staked brass inserts, our application engineers can provide specific boss geometry recommendations based on insert supplier specifications.
4. Corner Design: Radii Over Sharp Edges
Sharp corners are one of the most common design choices that look fine on screen but cause real problems in production. We recommend adding radii to all corners — internal and external — as a standard practice.
Why Sharp Corners Are Problematic
A sharp internal corner is a stress concentration point. Under load, stress concentrates at the corner tip, often causing brittle materials to crack at stresses far below the rated tensile strength. From a mold-making standpoint, sharp internal corners require EDM (electrical discharge machining) or multiple progressive tool passes — adding time and cost. Plastic melt also dislikes sharp corners: flow velocity and pressure change abruptly, which can create non-fill issues, air entrapment, and jetting defects.
External corners (convex): fillet radius = 1.5× the wall thickness
Internal corners (concave): fillet radius = 0.5× the wall thickness
This pairing maintains consistent wall thickness through the corner. These are minimums — larger radii are always better from a stress and flow perspective.
Chamfers as an Alternative
Chamfers are a practical alternative on parting-line edges or features where a machined radius would require a custom tool. A chamfer of 0.5× the wall thickness or less on external edges provides stress relief without significantly affecting flow or part geometry.
5. Surface Finish and Texture: Plan Before You Cut
Surface finish is often an afterthought in early design stages, but it directly affects mold cost, cycle time, and what defects are visible on the final part. We encourage customers to specify finish early — ideally before mold design begins.
| SPI Grade | Method | Ra (µm) | Typical Use |
|---|---|---|---|
| A1 | #3 diamond compound | ~0.01 | Optical lenses, mirror surfaces |
| A3 | #15 diamond compound | ~0.04 | Clear parts, high-gloss consumer goods |
| B3 | 320-grit abrasive cloth | ~0.12 | Semi-gloss, standard cosmetic parts |
| C3 | 320-grit stone | ~0.30 | Low-sheen commercial parts |
| D2 | 240-grit bead blast | ~0.80 | Matte, textured appearance |
| D3 | 24-grit bead blast | ~4.00 | Rough matte, functional surfaces |
<p>For a complete breakdown of every SPI grade — including polishing methods, Ra tolerances, and mold steel requirements — see our SPI surface finish standards guide.
Each higher level of finish requires completing all lower-level steps first. This is why high-polish finishes add significant cost — the labor is compounded at every step. A practical note from our production floor: a scratch or tool mark on an A1 surface requires re-polishing from scratch. Plan for this in your maintenance budget.
Textured Finishes
Textures can simulate leather, wood grain, or brushed metal. They hide defects such as weld lines and flow marks that would be obvious on a polished surface, and improve grip while reducing visible scratching during product life. Textures are applied after the mold is polished to an appropriate base finish.
| Texture Type | Approx. Depth | Required Base Finish |
|---|---|---|
| Fine sand | 50 µm | SPI B |
| Leather grain | 125 µm | SPI C |
| Netting pattern | 150 µm | SPI C |
| Wood grain | 250 µm | SPI D |
6. Draft Angles: Make Ejection Effortless
Draft is the slight taper applied to vertical surfaces to allow the part to release cleanly when the mold opens. It’s one of the most frequently debated topics between product designers and our molding engineers, because draft changes the appearance and interior volume of a part.
Our position is simple: insufficient draft creates real production problems (sticking, drag marks, part damage), while the visual impact of a 1–2° taper is almost imperceptible to end users. We’d rather discuss draft early than deal with ejection issues in production.
| Surface Finish | Typical Resin | Draft per Side |
|---|---|---|
| SPI A1 (mirror) | Acrylic | 0.5° |
| SPI B3 (semi-gloss) | ABS | 1.5° |
| Sand texture | 20% GF Polycarbonate | 2° |
| Leather texture | Soft PVC | 4° |
| Leather texture | ABS | 7.5° |
We add approximately 1° of additional draft for every 20 µm of texture depth beyond a polished base. Deep textures on stiff resins can require surprisingly large draft angles — this is one of the most common things designers are surprised by when we review their files.
Material Considerations
Glass-filled and mineral-filled resins have lower shrinkage than unfilled grades, which means they grip the mold more tightly. These materials require more draft. Flexible resins like soft PVC and TPE can be molded with less draft, since the part can deform slightly during release without damage.
Where Draft Can Be Reduced
Cores, pins, and ribs that are very short (under 3mm) can often be molded with minimal draft without causing ejection problems. Textured surfaces on the moving side of the mold (core side) also sometimes allow reduced draft, since the part naturally grips the moving side and ejects cleanly with the mold motion. Our mold designers evaluate draft requirements feature by feature rather than applying a blanket rule.
7. Undercuts: Understand the Cost Before You Commit
An undercut is any feature that prevents the molded part from being pulled straight out of the mold. Common examples include side holes, horizontal bosses, snap-fit hooks, and internal threads. Undercuts aren’t impossible to mold — but every undercut adds mechanical complexity, and complexity means higher tooling cost, longer maintenance intervals, and additional failure points.
Common Solutions
Side actions (slides)
A sliding steel block retracts laterally as the mold opens. Reliable and precise, but adds to tool cost and introduces wear surfaces requiring periodic maintenance.
Lifters
A small angled pin moves forward and laterally with the ejector system. Compact and effective for internal undercuts, but like slides they add wear surfaces.
Profiled ejector pins
A contoured pin forms the cavity beneath small undercuts like snap hooks. The simplest and lowest-cost approach — does leave an ejector pin witness mark.
Redesign
Often the most cost-effective solution. A snap hook perpendicular to the mold can frequently be reoriented in the draft direction, eliminating the undercut entirely.
When Undercuts Are Worth It
Some functional features — snap-fit assemblies, internal threads, living hinges — genuinely require undercuts and are worth the mold complexity. In these cases, our engineering team designs the mold mechanism with service access and wear surfaces in mind from the start. A well-designed slide can outlast the production life of the tool with proper maintenance.
Ready to Review Your Design?
Our DFM review process examines every aspect of your part geometry before we quote the mold — identifying issues like these before they become costly changes.
