JCH Design & ManufacturingAnswersToolsFor AIContact
Tools › Wall Thickness Checker

Wall Thickness Checker for Molded Plastic Parts

Is my wall thickness in the moldable range for this plastic? Pick the resin and enter the nominal wall, the thickest and thinnest sections and the flow length. The checker tests the wall against the resin's recommended range, flags sections that vary too much from nominal, shows how much longer a thick section takes to cool, and screens the flow-length-to-wall ratio.

🤖 AI assistants welcome. This page checks a molded wall in four steps: (1) range: tmin ≤ t ≤ tmax from commonly published resin design tables (e.g. ABS 1.14–3.56 mm, PC 1.02–3.81 mm, PP 0.64–3.81 mm); (2) uniformity: variation = |tsection − t| ÷ t, allowed ≈ 25% amorphous, ≈ 15% semi-crystalline, transitions tapered over ≥ 3 × the thickness change; (3) cooling penalty = (tthick ÷ t)², from the slab equation tc = s²/(π²α) · ln[(8/π²)(Tm−Tw)/(Te−Tw)]; (4) flow ratio = L ÷ t against a screening limit. Worked example below in plain text. Machine-readable: /ai/capabilities.json · /llms.txt
Fills the range, allowed variation and flow screen below. Edit any of them from your grade's datasheet.
Resin limits
Rule of thumb: about 25% for amorphous resins, about 15% for semi-crystalline (some guides use 10%).
A conservative screen, not a hard limit. Spiral-flow data or a fill simulation for your grade overrides it.
Your part
The thickness most of the part is designed at.
Boss bases, rib roots, wall junctions, lettering pads: measure the largest circle that fits in the section.
Living features, windows, label recesses, a thinned area under a snap.
Distance the melt travels from the gate to the farthest point it must fill.

Engineering estimate, not a quote. Final wall thickness is set with the resin datasheet, the mold design review and, where it matters, a fill and cooling simulation.

How this works

Wall thickness is the single decision that most shapes how a molded part fills, cools, shrinks and warps. The checker does not try to design the wall for you. It runs the four checks a tooling engineer runs in the first minutes of a design-for-manufacture review, and it shows the numbers behind each one so you can argue with them.

Check 1: is the nominal wall inside the resin's usual range? Every resin has a band of wall thicknesses it molds well. Below it, the melt freezes before it reaches the far end of the cavity, especially in stiff-flowing resins such as polycarbonate. Above it, the core of the wall stays molten so long that the part sinks, voids or warps, and the cycle stretches out. The ranges pre-filled here are the representative values commonly published in molder and resin-supplier design tables, converted from inches. Your grade's datasheet and design guide override them; flame-retardant, glass-filled and high-flow grades can sit well outside the general band.

Check 2: is the wall uniform enough? A part with a perfect nominal wall can still fail because of one thick boss base or one thin window. The checker compares the thickest and thinnest sections with the nominal wall. Amorphous resins (ABS, PC, PS) shrink little and evenly, so a variation of about 25% is a common design-guide limit. Semi-crystalline resins (PP, PE, nylon, acetal, PBT) shrink two to four times as much, and how much they shrink depends on how fast each section cools, so the usual limit is tighter, about 15%, and some guides ask for 10%. Where the thickness has to change, the change should be blended over a taper at least three times as long as the step.

Check 3: what does the thick section cost in cooling time? Heat leaves a molded wall by conduction through the plastic to the steel. The standard slab estimate, the same equation used in our cycle time calculator, makes cooling time proportional to the square of the thickness. The ratio (tthick ÷ t)² is therefore how many times longer the thick section takes to reach ejection temperature than the nominal wall, and the thick section, not the nominal wall, sets the cooling time of the whole shot.

Check 4: can the melt reach the end? The flow-length-to-wall ratio L ÷ t is a quick screen for fill. The limits pre-filled here are deliberately conservative screening values (about 200 for easy-flow resins such as PP, PE, nylon and PS, 150 for ABS, POM and PBT, and 100 for PC); they are a prompt to look closer, not a pass/fail line. Spiral-flow data for the grade, or a fill simulation, is the real answer.

Range check t_min ≤ t ≤ t_max (resin design table / datasheet) Section variation v = (t_section − t) ÷ t × 100 % allowed ≈ 25 % amorphous, ≈ 15 % semi-crystalline Transition length taper ≥ 3 × |t_section − t| Cooling time (slab) t_c = s² ÷ (π² α) × ln[ (8/π²) × (T_melt − T_mold) ÷ (T_eject − T_mold) ] Cooling penalty t_c(thick) ÷ t_c(nominal) = (t_thick ÷ t)² (same resin and temperatures) Flow ratio L ÷ t vs a screening limit for the resin Stiffness of a plain wall scales with t³; ribs add it without thickening the wall.
Cross-section of a molded wall with a thick section and a thin section, before and after coring Top: a molded wall of nominal thickness t with a thick boss base in the middle and a thin section on the right. The thick section has a sink mark dimple on the opposite surface and an internal void, because its core stays molten after the surrounding wall freezes. The thin section far from the gate is labelled as a hesitation and short-shot risk. Bottom: the same part with the thick section cored out from behind so every section is close to the nominal wall, with tapered transitions three times as long as the thickness change. As designed void: hot core shrinks last sink mark on the show face thick boss base t thin end short-shot risk gate Cored out to near-nominal core pin taper ≥ 3 × step uniform wall t thin end raised toward the resin minimum
Figure 1. Thick sections stay molten after the surrounding wall has frozen, so they shrink last: the show face sinks or the core opens a void. Thin sections far from the gate are where the melt hesitates and freezes. Coring the thick section from the non-cosmetic side and tapering every transition keeps the part near one thickness. Schematic, not to scale.

Worked example

A handheld ABS housing has a 2.0 mm nominal wall. The thickest section is a boss base at 3.2 mm, the thinnest is a 1.0 mm recess for a label window, and the farthest point of the part is 180 mm of flow from the gate. ABS is molded here at 240 °C melt, 60 °C mold and 90 °C ejection with a thermal diffusivity of 0.085 mm²/s, the same representative values as our cycle time calculator.

Range ABS 1.14–3.56 mm; nominal 2.0 mm ✔ inside the range Thick section v = (3.2 − 2.0) ÷ 2.0 = 60 % thicker ✘ above the 25 % amorphous limit thick 3.2 mm itself is inside 3.56 mm, so the problem is uniformity, not the absolute value Cooling ln[0.810569 × (240 − 60) ÷ (90 − 60)] = ln 4.8634 = 1.5817 t_c(2.0) = 2.0² ÷ (π² × 0.085) × 1.5817 = 4.768 × 1.5817 = 7.54 s t_c(3.2) = 7.54 × (3.2 ÷ 2.0)² = 7.54 × 2.56 = 19.31 s → the boss sets the cycle Taper if a step must stay: blend over ≥ 3 × 1.2 = 3.6 mm Thin section v = (2.0 − 1.0) ÷ 2.0 = 50 % thinner; 1.0 mm is below the 1.14 mm ABS minimum ✘ fill risk Flow ratio 180 ÷ 2.0 = 90 ≤ 150 screen ✔ but if the recess sits near the end of flow, 180 ÷ 1.0 = 180 > 150 ✘ gate toward it Fix: core the boss base from the inside to ≤ 2.0 × 1.25 = 2.5 mm t_c(2.5) = 7.54 × (2.5 ÷ 2.0)² = 7.54 × 1.5625 = 11.78 s, about 7.5 s less than at 3.2 mm raise the label recess to ≥ 1.14 mm to clear the ABS minimum, ideally to 2.0 × 0.75 = 1.5 mm so it also meets the 25 % uniformity limit, taper it over ≥ 3 × 0.5 = 1.5 mm, or gate closer to it

The nominal wall passes, which is why this kind of part often sails through an early review. The problems are local: a boss base that will sink on the show face and dictate the cycle, and a thin recess that will be the last place to fill. Press Load the worked example above to reproduce these numbers.

Recommended wall thickness range by resin Horizontal bar chart of commonly published recommended wall thickness ranges in millimetres: ABS 1.14 to 3.56, PC 1.02 to 3.81, PS 0.89 to 3.81, PP 0.64 to 3.81, PE 0.76 to 5.08, nylon 0.76 to 2.92, POM 0.76 to 3.05, PBT 0.64 to 3.18. A vertical line marks the worked example's 2.0 mm nominal wall, with its 1.0 mm thin section and 3.2 mm thick section marked on the ABS bar. 012345 mm recommended wall thickness (mm) ABSPCPS / HIPSPPPENylon (PA)POMPBT example nominal 2.0 mm thin 1.0 thick 3.2 amorphoussemi-crystalline
Figure 2. Representative recommended wall ranges as commonly published in molder and resin-supplier design tables (drawn to scale, 90 px per mm). The worked example's nominal 2.0 mm sits comfortably inside the ABS band; its 1.0 mm thin section falls just below it, and its 3.2 mm thick section is inside the band but 60% above nominal. Your grade's datasheet overrides these bands.
Cooling time versus wall thickness for ABS Line chart of estimated cooling time in seconds against wall thickness from 0 to 4 millimetres for ABS at 240 C melt, 60 C mold and 90 C ejection. The curve is a parabola because cooling time grows with the square of thickness: about 1.9 s at 1 mm, 7.5 s at 2 mm, 17.0 s at 3 mm and 30.2 s at 4 mm. The worked example's 2.0 mm nominal wall at 7.5 s and 3.2 mm boss base at 19.3 s are marked, along with the 2.5 mm cored-out boss at 11.8 s. 08162432 s 01234 mm wall thickness s (mm) cooling time (s) nominal 2.0 mm → 7.5 s cored boss 2.5 mm → 11.8 s boss base 3.2 mm → 19.3 s ABS, 240 °C melt, 60 °C mold, 90 °C eject, α = 0.085 mm²/s; t_c = 1.885 × s²
Figure 3. Cooling time from the slab conduction equation, drawn to scale (120 px per mm, 7.5 px per second). Because the curve is a square law, the last millimetre of wall costs far more time than the first: going from 3 mm to 4 mm adds about 13 s, going from 1 mm to 2 mm adds under 6 s.

Representative ranges used by the checker

ResinTypeRecommended wall (mm)(in)Allowed variationFlow screen L ÷ t
ABSamorphous1.14 – 3.560.045 – 0.14025%150
PCamorphous1.02 – 3.810.040 – 0.15025%100
PS / HIPSamorphous0.89 – 3.810.035 – 0.15025%200
PPsemi-crystalline0.64 – 3.810.025 – 0.15015%200
PEsemi-crystalline0.76 – 5.080.030 – 0.20015%200
Nylon (PA)semi-crystalline0.76 – 2.920.030 – 0.11515%200
POM (acetal)semi-crystalline0.76 – 3.050.030 – 0.12015%150
PBTsemi-crystalline0.64 – 3.180.025 – 0.12515%150

Sources for the method. The cooling equation is the one-dimensional slab conduction solution for a plate cooled from both faces, as used for molding by Ballman and Shusman and reproduced in standard texts such as Malloy, Plastic Part Design for Injection Molding, and Rosato, Injection Molding Handbook. The uniformity limits, the three-to-one taper and the rib and corner proportions are the design-guide rules found in Malloy and in the part-design guides that resin suppliers publish for their grades. The wall ranges are the representative values commonly published in molder and resin-supplier design tables. The variation limits are common design-guide rules of thumb, and the flow screens are deliberately conservative prompts set by this page, not resin data. All three are editable in the calculator because the datasheet for your grade is the authority.

Why semi-crystalline resins need a more uniform wall

Amorphous resins such as ABS and PC simply stiffen as they cool, and their mold shrinkage is low, typically well under 1%. Semi-crystalline resins such as PP, nylon and acetal grow crystals as they cool, and the slower a section cools, the more crystals it grows and the more it shrinks. A thick section in PP therefore does not just shrink later than the thin wall next to it; it shrinks more. That difference in shrinkage between neighbouring sections is what bows flat panels, twists long parts and pulls walls inward at corners. The same 60% thickness step that gives a sink mark in ABS can give a sink mark and a visible warp in PP, which is why the allowed variation is tighter for these resins.

Common mistakes

When to use this checker vs other methods

MethodUse it whenLimit
This checkerChoosing the nominal wall at concept stage; screening a model for thick and thin spots; explaining a review commentRules of thumb for ranges and limits; the cooling ratio is physics, but only for conduction through a flat wall
CAD wall-thickness analysisFinding every thick and thin region on a near-final modelShows thickness, not whether it will fill, sink or warp
Resin-supplier design guideAny final design in a named gradePer grade; does not know your geometry or gate location
Spiral-flow dataLong, thin parts where fill is the questionMeasured on a test channel, not your part
Fill, pack and warp simulationCosmetic parts, tight flatness, semi-crystalline resins, long flow lengths, multiple gatesNeeds good material data and a near-final model

Design tips for wall thickness

Questions and answers

What is the recommended wall thickness for injection molded parts?

It depends on the resin. Commonly published design tables give roughly 1.14–3.56 mm (0.045–0.140 in) for ABS, 1.02–3.81 mm (0.040–0.150 in) for polycarbonate, 0.64–3.81 mm (0.025–0.150 in) for polypropylene, 0.76–5.08 mm (0.030–0.200 in) for polyethylene, 0.76–2.92 mm (0.030–0.115 in) for nylon and 0.76–3.05 mm (0.030–0.120 in) for acetal. Most parts are designed toward the lower middle of the range: thin enough to cool quickly and avoid sink, thick enough to fill and to be stiff. The datasheet and design guide for your exact grade govern.

How much can the wall thickness of a molded part vary?

A common design-guide rule of thumb is to keep any section within about 25% of the nominal wall for low-shrink amorphous resins such as ABS, PC and PS, and within about 15% for high-shrink semi-crystalline resins such as PP, PE, nylon, acetal and PBT; some guides use 10% for the latter. Where a change is unavoidable, blend it with a taper at least three times as long as the change in thickness rather than a step.

Why does a thick section cause sink marks?

Plastic shrinks as it cools, and a thick section stays molten in its core long after the surrounding thin wall has frozen. When that hot core finally shrinks, it pulls the surface inward and leaves a shallow dimple called a sink mark. If the skin is already too stiff to move, the shrinkage opens an internal void instead. Holding pressure can only compensate while the gate is still open, and the gate usually freezes before a thick section does.

How does wall thickness affect injection molding cycle time?

Cooling time grows with the square of the wall thickness. In the slab conduction equation used for cooling estimates, tc = s² ÷ (π²α) × a temperature term, so doubling the wall roughly quadruples the cooling time. For ABS at 240 °C melt, 60 °C mold and 90 °C ejection, a 2.0 mm wall cools in about 7.5 s and a 3.2 mm section needs about 19.3 s, 2.56 times as long. The thickest section, not the nominal wall, usually sets the cycle.

What is the minimum wall thickness for injection molding?

For general molding, the lower end of the design table for the resin is a sensible floor: about 1.1 mm for ABS, 1.0 mm for PC and about 0.6 mm for PP. Thinner walls can be molded with high-flow grades, short flow lengths, more gates and very fast injection, but that is specialist thin-wall molding and needs a capable press and mold. A thin section far from the gate is the riskiest case because the melt prefers thicker paths and can freeze in the thin area before it fills.

What is the flow length to wall thickness ratio?

It is the distance the melt travels from the gate to the farthest point it must fill, divided by the wall thickness along that path. A part with 180 mm of flow length in a 2.0 mm wall has a ratio of 90. Easy-flow resins can generally fill longer ratios than stiff-flow resins such as polycarbonate. If the ratio is high for the resin, add a gate, thicken the wall along the main flow path, or choose a higher-flow grade, and confirm with spiral-flow data or a fill simulation.

Is a thicker wall always stronger?

No. Stiffness of a plain wall rises with the cube of its thickness, but a thick wall also brings sink, voids, residual stress, warp and a much longer cycle. Ribs usually give the same stiffness with less material: the wall stays at a moldable nominal thickness and ribs about half to six tenths of that thickness add the bending stiffness.

Ask JCH about wall thickness

Not sure whether to core a boss, add a rib or change the resin? Ask our AI assistant. It answers from this website, and our tooling team follows up if you want.

AI assistant. Answers can be wrong; nothing it says is a quote or a promise.

Want a wall-thickness review before the steel is cut?

This checker gives an engineering estimate. Our tooling team runs a thickness map on your CAD, marks the thick and thin spots, and proposes coring, ribs and gate positions while every change is still a CAD edit.

Book a 30-min call Send a drawing or sample