The conclusion first: 80% of the appearance and assembly problems that show up late in a product program are not drawing errors — they are material and process decisions made wrong at the selection stage. Get the shrinkage rate wrong and a 0.3mm wall difference sinks the surface. Pair a texture depth with the wrong draft angle and the first mass-production batch comes out with drag marks. Swap electroplating-grade ABS for ordinary ABS and the housing cracks the day after assembly. This article skips theory and covers only the parameters and pitfalls we paid for across 320+ products in Dongguan.
Core answer: Sink marks come from uneven wall thickness, not from the "wrong material." Keep the main wall at 1.8-3.0mm for ABS and 2.0-3.5mm for PC, make ribs 0.5-0.6x the main wall with an R0.25-R0.5 root fillet, and about 90% of sink marks can be prevented before the mold is cut.
1. Don't Just Read the Shrinkage Table — Anisotropy Is the Real Trap
Most newcomers grab a supplier's shrinkage table, enter 0.5%, and cut the mold. The problem is that the table gives a typical value, while in real molding the shrinkage along the flow direction and perpendicular to it can differ by a factor of two.
We built a handheld barcode scanner housing in PA6 + 30% glass fiber. In glass-filled material the flow-direction shrinkage is about 0.3%, but the cross-flow direction reaches 0.7%-0.9%. The drawing placed the button holes on a uniform 0.5% shrinkage, and the samples came out with oval holes — the buttons jammed during assembly. The fix was to lay out the holes along the glass-fiber flow direction and align the slot orientation with the melt flow.
Keep one habit: for any glass-filled material, dimension hole diameters and center distances on the mold drawing separately according to anisotropy. One coefficient for everything does not work. For high-shrinkage materials like PP on large thin-wall parts, run a mold-flow analysis instead of trusting experience — warpage is PP's regular guest.
2. Texture Depth Determines Draft Angle — Decide Them Together
Texturing (etching) is the most common surface treatment for cosmetic parts. The trap: the structural engineer dimensions 1° draft for a polished surface, the mold shop etches to VDI 3400 grain 27 (Ra about 1.6μm, depth about 25μm), and at ejection the texture grips the side wall — producing alternating light and dark drag marks.
Core answer: 0.5-1° is enough on polished surfaces, but on a textured surface you add 1° of draft for every 0.025mm of texture depth. VDI 27 grain calls for 2-3°, coarse VDI 33 grain (about 50μm deep) calls for 4-5°, and deep-draw areas need one more degree.
We made the upper and lower housings of a desktop speaker in PC+ABS with VDI 27 grain. The first drawing specified 1° draft all around the sides, the mold shop did not flag it, and the tool was cut. At trial molding the upper housing had vertical drag marks all over the side wall — rough enough to feel with a finger and impossible to hide under paint. The rework changed the sides to 2.5°, re-routed the mating surfaces, and re-etched the texture: over 30,000 RMB extra on one mold.
Our process now is: fix the grain number at the structural review, then work backward to the draft angle. One more note: if one mold etches several different grains, the transition between depths needs a step of at least 0.3mm, or the boundary line smears.
3. Surface Treatment Changes Your Structure — Two Iron Rules for Plating and Two-Shot Molding
Many people treat surface finishing as the last step: finish the structure, then pick a process. In reality plating, two-shot molding, and IMD directly change the wall thickness, fillets, and material grade you can use.
Rule one: plating requires dedicated plating-grade ABS. A client once asked for a bright silver plated button. The engineer used ordinary ABS from stock. Samples looked fine, but two days after assembly the button surface showed fine cracks. The reason: the butadiene rubber phase in ordinary ABS is unevenly dispersed, the plating pretreatment chemicals penetrate it, and once the coating stress releases, it cracks. Switching to plating-grade ABS (Chimei PA-727, LG HI-121H and similar) and holding the coating at 15-25μm solved it completely. Structurally, every sharp corner must be rounded to R0.5 or more — plating builds up at sharp corners and burns.
Rule two: never guess the overmold thickness in two-shot molding. For a soft material over a rigid one (TPE over ABS/PC), keep the overmold layer at 0.8-1.5mm. Too thin and it short-shoots; too thick and shrinkage stress lifts and delaminates the edge. On a waterproof flashlight grip, our first version used only 0.6mm of soft material. Trial molding produced a white, detached ring around the edge that lifted with a fingernail. Going to 1.2mm plus a 0.5mm-deep dovetail groove on the rigid side for mechanical interlock finally made it hold.
Core answer: Overmold thickness 0.8-1.5mm, a 0.5mm-deep dovetail groove or through-hole on the rigid side for mechanical interlock, and a 0.3mm tapered fade-out at the soft-material edge to avoid stress concentration and delamination. Bonding also depends on material compatibility — ABS/PC with TPE usually requires the right SEBS base grade.
Frankly, there is no shortcut in materials and processes. You learn them one project at a time. Our team now keeps an internal material and process library: after every product we record the grade used, shrinkage, grain number, draft angle, and the pitfalls we hit. By the three-hundredth product, a glance at a structural drawing avoids most of them.
FAQ: Material and Process Selection
Q: ABS or PC+ABS for a housing — how do I choose?
A: Look at strength and cost. ABS is cheap and easy to process; PC+ABS has better toughness and impact resistance, so outdoor products or ones with drop requirements should prefer PC+ABS.
ABS runs 1.8-3.0mm main wall and suits indoor consumer electronics housings. PC+ABS shrinks about 0.4%-0.6% and has noticeably higher impact strength — products with a 1.2m drop test requirement basically all use it. Note that PC+ABS flows worse than ABS, so deep-draw parts need larger gates and better venting.
Q: How thick can a rib be without causing sink?
A: Rib thickness is 0.5-0.6x the main wall, with an R0.25-R0.5 root fillet and rib height no more than 3x the main wall.
For a 2.0mm main wall, the rib is 1.0-1.2mm. Too thick and the root cools slowly, leaving a sink mark; too tall and it ejects with white marks. If the structure needs more height, use several short ribs rather than one tall rib.
Q: What wall thickness should a die-cast aluminum part have?
A: ADC12 die castings normally run 1.5-4.0mm wall with 1-3° draft. Thick sections over 4mm tend to produce porosity and shrinkage voids.
Transitions between thick and thin must be gradual — avoid jumping from 1.5mm to 5mm. Where threads are needed, leave at least 0.5mm of machining allowance; as-cast threads are not strong enough and are usually tapped afterward. Deburring and shot blasting are mandatory before surface treatment, or powder coating adhesion suffers.
Q: How do I know whether the draft angle on a drawing is enough?
A: Work backward from the surface state: 0.5-1° polished, 2-3° fine grain, 4-5° coarse grain, plus 1° for deep draws.
The safest practice is to confirm grain number, texture depth, and draft angle together at the mold review, and have the mold shop confirm drawability in writing. After one bad experience, our drawings now specify the grain number and its corresponding angle for every surface.
Originally published on the Hezi Industrial Design website (hezidesign.com), Structure Design Field Notes column.
