Quick reference
ABS is one of the most common resins for device covers, bezels and housings. It molds easily, takes texture and paint well, and has good impact strength at room temperature. Most problems with molded ABS covers come back to a handful of geometry rules. Here they are in one table, with the reasoning in the sections that follow.
| Feature | Typical guideline for ABS | Why it matters |
|---|---|---|
| Nominal wall | ~1.2–3.5 mm; ~2.0–2.5 mm is common for covers | Too thin will not fill; too thick sinks and cools slowly |
| Wall variation | Keep within about ±25% of nominal | Uneven walls cause warp and sink |
| Draft on walls | ≥1° per side; more on textured faces | Lets the part eject without drag marks |
| Rib thickness at base | ~50–60% of the adjoining wall | Avoids sink marks on the show face |
| Rib height | Up to ~3 × wall thickness | Taller ribs are hard to fill and eject |
| Boss outer wall | ~60% of nominal wall, cored out | Solid bosses sink and void |
| Inside corner radius | ~0.5 × wall or more | Reduces stress and helps flow |
| Mold shrinkage | Roughly 0.4–0.7% | Mold is cut oversize to compensate |
Why wall thickness comes first
Molten plastic flows into the mold, packs, then shrinks as it cools. Thick sections cool last. While they are still shrinking, they pull on the surrounding material, which shows up as a dip on the visible face (a sink mark) or as internal voids. Thin sections next to thick ones cool at different rates, and that difference warps the part.
A uniform wall is therefore the foundation of a good cover. Choose one nominal thickness, design every feature relative to it, and where the wall must change, blend the transition over a distance of about three times the difference instead of using a sudden step.
Thin is not always cheaper
A thinner wall uses less resin and cools faster, but it needs higher injection pressure and can make long, flat covers hard to fill. For covers of typical hand-held size, around 2.0–2.5 mm is a comfortable balance.
Draft: designing for ejection
When the plastic cools, it shrinks onto the core of the mold. Without draft, the ejector pins have to drag the part off, which scuffs the surface or distorts the walls. Draft is a small taper on every face parallel to the opening direction.
Start with at least one degree per side on walls. Textured surfaces need more, because the texture locks into the steel. A common rule is to add about one degree for every 0.025 mm of texture depth. Light textures often need around 1.5–2 degrees; coarse textures can need three degrees or more. Check the texture supplier's recommendation for the pattern you choose.
Draft should be drawn in the CAD model, not left to the toolmaker. It changes the shape of the part, and features such as snap-fit hooks and screw bosses must be positioned with draft in mind.
Ribs and bosses: stiffness without sink
Ribs stiffen a cover far more efficiently than thickening the whole wall. The trick is to keep them thin relative to the wall they sit on.
Ribs
- Base thickness about half to 60% of the wall
- Height up to about three times the wall
- Spacing at least about two to three times the wall between parallel ribs
- A root radius of roughly a quarter to half the wall where the rib meets the wall
- Draft of about half a degree per side or more
Bosses
Screw bosses should be cored out so their wall is similar to a rib, not a solid cylinder. Connect tall bosses to nearby walls with small gussets rather than making them thicker. Follow the screw maker's guidance for the hole diameter if you use thread-forming screws for plastics.
Defects you can design out
Many molding defects have a geometry cause. Fixing the design is usually cheaper than fighting the defect with process settings.
| Defect | What you see | Common design cause | Design fix |
|---|---|---|---|
| Sink mark | Shallow dip on show face | Thick rib, boss or wall junction | Thinner ribs, cored bosses, uniform wall |
| Warp | Cover rocks on a flat table | Uneven walls; long flat panel | Uniform wall; add ribs or a slight dome |
| Short shot | Part not fully filled | Wall too thin far from the gate | Thicker wall or better gate location |
| Weld line | Faint line on the surface | Flow fronts meeting around holes | Move holes or gate; keep line off show face |
| Drag marks | Scuffs along walls | Too little draft for the texture | Increase draft |
| Stress whitening | White marks near snap fits | Sharp corners; strain too high | Add radii; lengthen snap-fit arm |
Tolerances on molded covers
Molded parts can be very repeatable once a tool is tuned, but the first shots rarely match the CAD model perfectly. Shrinkage depends on wall thickness, flow direction, gate position and processing conditions, so features far from the gate or across thick sections shrink slightly differently from the rest.
For a cover, focus tight tolerances on the features that mate with other parts: screw boss positions, snap-fit hooks, and the outline that meets the base. Give looser tolerances to cosmetic outlines and decorative features. Industry tolerance guides for plastics, such as those published by resin suppliers and molding associations, distinguish between commercial and fine tolerance grades; commercial grades are the economical default.
It is normal to adjust the tool after the first samples. Leaving steel on critical features, sometimes called "steel safe" design, lets the toolmaker remove a little material to bring a dimension into range rather than adding material back, which is much harder.
Snap fits and assembly features
Covers often clip on rather than screw on. Cantilever snap fits are the most common type. Their deflection must stay within what ABS can tolerate without cracking or whitening, so longer, tapered arms are better than short, stiff ones. Undercuts on snap hooks need either a side action in the mold or a pass-through window in the part, which affects tool cost, so discuss them early.
Screw-together covers need bosses on one side and clearance holes on the other. Keep the parting line and gate away from the bosses so weld lines do not form at the screw.
Gates, parting lines and cosmetics
The toolmaker chooses gate and ejector positions, but you can guide them. Mark the cosmetic faces on the drawing, and say where gate marks, ejector marks and the parting line are acceptable. On most covers, the inside surface or a hidden edge is best.
Specify texture by a recognised standard such as SPI or VDI grades, or by a named texture from a texture supplier. Specify color by a reference such as a color chip or a standard color number, and ask for a sample plaque if matching matters.
When ABS is not the right resin
ABS suits most indoor covers. Consider alternatives when:
- The part sees heat above roughly 80 °C, sunlight or outdoor weathering: consider ASA or PC/ABS
- The part must survive hard impacts at low temperatures: consider PC or PC/ABS
- The part sees oils, solvents or cleaning chemicals: consider PP, PBT or a chemically resistant grade
- The cover must be transparent: consider PC or PMMA
Prototyping before tooling
Before cutting steel, it is common to build a few covers by 3D printing or urethane casting to check fit and appearance, or to machine them from ABS block for functional testing. These parts will not show molding defects such as sink or weld lines, so review the molded design for those separately.
Next steps
Upload the cover model through the quote form and note the expected quantity, texture and color. The reviewing engineer will check wall thickness, draft, ribs and undercuts before quoting and suggest changes that make the tool simpler and the parts more consistent.