Core answer: Start plastic part walls at 2.0mm by default — 1.5-2.5mm for ABS/PC, 1.2-2.5mm for PP. Make rib thickness 0.5-0.6x the main wall. Use 0.5-1° draft on polished surfaces, and add 1° per 0.025mm of texture depth on grained surfaces. Nail these four numbers down and you eliminate about 80% of sink, warpage, and drag-mark problems. The other 20% lives in material selection and secondary processes — PP painted without pretreatment will always flake, and TPE overmolded on ABS without mechanical interlock will crack within two years.
A client from Shenzhen brought in a prototype a few days ago: of thirty trial housings, twenty-seven had surface depressions and three snaps broke off with a light tug. Five minutes with the part in my hand was enough. Main wall 3.2mm, ribs at 2.5mm, in ABS. With that structure, shrinkage is guaranteed — the surprising outcome would be no shrinkage at all. After ten years in structure design, I've found the pitfall new engineers hit most isn't not knowing the software. It's not having the instinct that plastic flows, shrinks, and gets dragged. Here are lessons from our recent projects, paid for in real money.
1. Wall Thickness and Ribs: Do the Sink-Mark Math at the Drawing Stage
Shrinkage happens because thick areas cool slowly. As plastic drops from melt temperature to room temperature it contracts; thin areas freeze first and hold their shape, while thick areas cool later — the skin is already hard, the core keeps collapsing inward, and the surface sinks. So the structural rule is one sentence: keep the wall thickness of the whole part as uniform as possible.
My default values for clients: ABS and PC+ABS at 1.8-2.2mm, PC at 2.0-3.0mm, PP at 1.5-2.5mm, nylon at 1.5-2.0mm, POM at 1.5-2.5mm. For handheld small housings, 2.0mm is the universal value — stiff enough, easy to mold, and the cost isn't ugly. Large parts like chassis covers over 300mm can go to 2.5-3.0mm, but past 4mm the injection molding shop owner looks at you differently: cooling time doubles and shrinkage becomes nearly impossible to avoid.
The rib rule is even simpler: rib thickness = main wall x 0.5-0.6, rib height no more than 3x the wall, with an R0.3-R0.5 fillet at the root and 0.5°-1° draft in the ejection direction. Why not 0.8x or more? Because the rib root is effectively two masses of plastic stacked together, so the local thickness exceeds 1.5x the main wall and a groove appears on the back side of the rib — the industry calls it a sink mark shadow. That prototype client had ribs at 0.8x, on one side only, over a large area; the front face looked like someone had pressed it with a finger.
We also hit a subtler pitfall. A desktop fan base had a solid 40mm-diameter cylinder in the middle for weight. The back of that cylinder sank into a crater and interfered with the motor bracket during assembly. The fix: turn the solid column into a "sleeve plus three ribs" at 2.0mm wall, leaving the center hollow with no material — strength preserved, shrinkage solved. So whenever you see solid thick material, the first reaction should be: can we core it out?
2. Draft Angle and Graining: Drag Marks on Cosmetic Surfaces Usually Start Here
Core answer: Draft angle can't be a blanket 1°. Polished surfaces can take 0.5-1°, fine textures need 1.5-2°, coarse textures (VDI 33 and above) need 3-5°. Judge by texture depth: every 0.025mm of depth adds 1° of draft. Grained surfaces must also use texture draft, and deep textures should be avoided near the parting line.
Draft is one of those things: leave 0.5° off the drawing and the mold shop won't fix it for you. The result shows up at trial molding as whitening on the cosmetic surface, or in bad cases a full tear. The industry rule of thumb: every 0.025mm of etch depth adds 1° of draft. A fine texture like MT11010 is roughly 0.02mm deep, so about 1° is enough. An obvious sand texture like VDI 33-39 runs close to 0.04mm, so 2-3° is needed. A coarse leather grain like VDI 45 needs at least 4-5°, and some suppliers demand 6°.
Last year we did a portable speaker with a fine-sand PC+ABS housing and a 35mm-deep side wall. We specified 1° draft the first time. At trial molding, the lower part of the side wall came out whitened in patches. Polishing and re-etching the texture cost over 6,000 RMB and a week of schedule. The second attempt used a tapered draft — 1.5° at the top, 2.5° at the bottom — and passed first time. The lesson: on deep-draw parts, draft must increase with depth, not stay constant, because the deeper you go, the harder the shrinking plastic grips the core.
One more detail that gets overlooked: graining changes dimensions. An etch depth of 0.03mm means 0.03mm growth per side, 0.06mm across. If you're dimensioning a mating step, key travel, or snap clearance, the drawing must state clearly whether a dimension is "before graining" or "after graining." Our convention: all functional dimensions are given after graining, cosmetic surfaces keep etch allowance. Don't dismiss 0.06mm — snap interference is only around 0.1mm to begin with, so get the direction wrong and the part either won't assemble or rattles.
3. Material Selection and Secondary Processes: Painting, Overmolding, Ultrasonic Lines
Late in a structure design, most problems aren't about shape — they're about material and surface-process compatibility. The two pitfalls that hurt us most in recent years were paint adhesion and soft-over-rigid overmolding.
Painting. PP and PE are non-polar with low surface energy, so direct painting, hot stamping, and silk screening all adhere poorly. It may survive two months on a desk, but a cross-hatch adhesion test in the lab peels it off in sheets. We had an outdoor power supply project where the housing was specified as PP with a matte lacquer. Samples looked great, but during reliability testing — 48 hours at 65°C and high humidity — the coating edges started lifting. We switched to flame treatment or primer on the PP before painting, which added over 2 RMB per part. Had we chosen PC+ABS or ABS from the start, painting would have been trouble-free. The right order in material selection is: process first, then material, then shape — most people do it backwards.
Overmolding. With TPE or TPU over a rigid plastic, many people assume chemical bonding is enough. In reality, except for a few dedicated overmolding grades, most combinations need mechanical interlock as a backstop. For a sports watch band connector housing, we cut dovetail grooves plus through-holes in the ABS rigid part so the soft material flows through and forms a rivet — pull-out force above 80N before we dared ship it. With a flat lap joint only, it delaminates at 20N on the test rig. Design points: the rigid overmold surface needs grooves, holes, or a wavy interlock at least 0.5mm deep; keep the soft material wall between 0.8mm and 2.0mm — too thin and it short-fills, too thick and it shrinks badly.
Finally, ultrasonic lines. Two ultrasonically welded parts need a triangular energy director on the contact surface, typically 0.3-0.5mm high, 0.6-1.0mm wide at the base, with a 60° or 90° tip angle — plus a step joint for location so the parts don't shift sideways during welding. Excessive flash after ultrasonic welding usually means the energy director is too tall or the amplitude is too high. It's not a mold problem.
FAQ: Plastic Structure Design and Process Materials
Q: How many millimeters should a plastic part wall be?
A: ABS/PC+ABS 1.8-2.2mm, PC 2.0-3.0mm, PP 1.5-2.5mm, kept overall within 1.5-3.0mm, and the ratio between thickest and thinnest sections should not exceed 2:1.
For handheld products, 2.0mm is the safe value. If strength is insufficient, add ribs rather than wall thickness — rib thickness at 0.5-0.6x the main wall, or a sink mark shadow appears on the back. Large housings can go to 2.5-3.0mm, but beyond 4mm both cooling time and shrinkage risk rise noticeably.
Q: How do I set draft on a grained surface so it doesn't drag?
A: Convert from texture depth — every 0.025mm adds 1° of draft. Fine textures about 1-1.5°, medium about 2-3°, and coarse grains like VDI 45 need 4-5°.
For deep-draw parts, make the draft a taper that is smaller at the top and larger at the bottom, with 1-1.5° more at the base, because shrinking plastic grips harder with depth. Also remember graining grows dimensions by about 0.03mm per side, so mating dimensions must state whether they are before or after graining.
Q: Why does TPE overmolded on ABS crack and delaminate?
A: For most combinations, chemical bonding alone isn't enough — mechanical interlock is essential. The rigid surface needs grooves, through-holes, or a wavy structure so pull-out strength stays stable above 60-80N.
In practice: cut dovetail grooves or through-holes at least 0.5mm deep into the rigid part so the soft material flows through and rivets; keep the soft wall at 0.8-2.0mm. A flat lap joint delaminates at around 20N, and the problem becomes more obvious after drops or high-temperature aging.
Q: Can PP be painted or silk screened directly?
A: Not recommended. PP has low surface energy and poor coating adhesion, failing cross-hatch and damp-heat tests. It needs flame treatment or a primer first, adding roughly 1-2 RMB per part.
If appearance requirements are high, switch to ABS or PC+ABS, which are far more mature for painting, plating, and hot stamping. The material sequence should be: define the surface process first, work back to the material, and design the shape last.
Top comments (0)