Interactive reference for part designers: pick a topic, then drag the sliders – the part redraws and the design checks update live.
1. Wall Thickness
Keep the nominal wall as uniform as possible, within the material range below.
Design one nominal wall and keep it everywhere.
Change thickness gradually: taper over at least 3× the thickness change.
Core out thick areas instead of leaving solid plastic.
Thinner walls cool faster: cycle time grows roughly with wall thickness squared.
Thickness variation
keep within about ±10%
Transition taper
≥ 3 : 1
Typical range
1–3.5 mm
Try it – drag the sliders
Recommended wall thickness by material
Material
Min (mm)
Max (mm)
Range (in)
ABS
1.1
3.6
0.043 – 0.142
Acetal (POM)
0.8
3.0
0.031 – 0.118
Acrylic (PMMA)
0.6
3.8
0.024 – 0.150
LCP
0.8
3.0
0.031 – 0.118
Nylon (PA)
0.8
2.9
0.031 – 0.114
Polycarbonate (PC)
1.0
3.8
0.039 – 0.150
Polyester (PBT)
0.6
3.2
0.024 – 0.126
Polyethylene (PE)
0.8
5.1
0.031 – 0.201
PPS
0.5
4.6
0.020 – 0.181
Polypropylene (PP)
0.6
3.8
0.024 – 0.150
Polystyrene (PS)
0.9
3.8
0.035 – 0.150
Polyurethane (PU)
2.0
19.0
0.079 – 0.748
Typical practical ranges. Thinner is possible for small parts with short flow; thicker sections should be cored out.
2. Draft Angles
Add draft on every face parallel to the mold opening so parts release cleanly.
1–2° is a safe default; 0.5° only on polished, shallow faces.
Deep parts and cores need more draft than shallow ones.
Textured faces need extra draft (see Surface Finish).
Draft the inside (core side) at least as much as the outside.
Default draft
1–2°
Minimum, polished
0.5°
Texture
+1.5° per 0.025 mm depth
Try it – drag the sliders
3. Ribs
Ribs add stiffness without thickening the wall – if they are thin enough not to sink.
Rib thickness 50–60% of the wall it sits on (40–50% on glossy show faces).
Height up to 3× the wall.
Space ribs at least 2× the wall apart.
Draft 0.5–1° per side; radius the base 0.25–0.5× wall.
Thickness
0.5–0.6 t
Height
≤ 3 t
Spacing
≥ 2 t
Try it – drag the sliders
4. Bosses
Bosses take screws and inserts; they must be cored and supported.
Boss OD about 2–2.5× the hole diameter.
Boss wall about 60% of the nominal wall, cored out.
Tie bosses to walls with ribs or gussets instead of standing alone.
Radius the base; use the screw maker's hole size for self-tapping screws.
Outer diameter
≈ 2–2.5 × hole
Boss wall
≈ 0.6 t
Base radius
0.25–0.5 t
Try it – drag the sliders
5. Radii & Fillets
Rounded corners help flow, reduce stress and keep the wall uniform.
Inside radius at least 0.5× the wall.
Outside radius = inside radius + wall, so the corner stays the same thickness.
Sharp inside corners concentrate stress and are where parts crack.
Edges on the parting line can stay sharp for a clean shut-off.
Inside radius r
≥ 0.5 t
Outside radius R
r + t
Ideal r
≈ 0.6–0.75 t
Try it – drag the sliders
6. Undercuts
Anything that stops a straight pull needs a side action – or a smarter design.
First try to remove it: open the feature to the parting line or use a pass-through core.
Side holes and outer undercuts need sliders; inner undercuts need lifters.
Small undercuts can be bumped off in flexible resins like PP or PE.
Every action adds cost, cycle time and maintenance.
Best option
redesign to straight pull
Outside undercut
slider
Inside undercut
lifter / collapsible core
Try it – drag the sliders
7. Snap Fits
Cantilever snaps must bend without passing the resin's strain limit.
Taper the beam (thickness down to about half at the tip) to spread strain evenly.
Radius the root at least 0.5× beam thickness.
Keep strain under the allowable limit – use the calculator below.
For repeated assembly use about 60% of the one-time strain limit.
Root radius
≥ 0.5 t
Tapered beam
tip ≈ 0.5 t
Deflection
y = k · ε · L² / t
Try it – drag the sliders
8. Living Hinges
A thin web molded in PP or PE that can flex thousands of times.
Use PP (best) or PE; most other resins crack.
Hinge thickness 0.25–0.4 mm, radiused on both sides.
Gate so the melt flows across the hinge, never along it.
Flex the hinge right after molding to orient the molecules.
Material
PP or PE
Thickness
0.25–0.4 mm
Flow
across the hinge
Try it – drag the sliders
9. Surface Finish
Specify SPI polish or texture early – it drives draft, steel and cost.
Glossy SPI A finishes need hardened steel and show every flaw.
SPI B and C are cost-effective for most internal and semi-visible parts.
Blasted and textured finishes hide sink and flow lines but need more draft.
Allow about 1.5° extra draft for each 0.025 mm of texture depth.
Glossy
SPI A-1 to A-3
Semi-gloss / matte
SPI B / C
Textured
SPI D, VDI, MT
Try it – drag the sliders
SPI finish grades and typical draft
SPI
Method
Ra (µm)
Typical use
Min draft
A-1
Grade #3 diamond buff
0.012–0.025
Lenses, mirrors, high gloss
0.5–1°
A-2
Grade #6 diamond buff
0.025–0.05
High-gloss cosmetic parts
0.5–1°
A-3
Grade #15 diamond buff
0.05–0.10
Gloss cosmetic parts
1°
B-1
600 grit paper
0.05–0.10
Semi-gloss, light cosmetic
1°
B-2
400 grit paper
0.10–0.15
Semi-gloss, general
1–1.5°
B-3
320 grit paper
0.28–0.32
Medium finish
1.5°
C-1
600 grit stone
0.35–0.40
Low gloss, internal parts
1.5°
C-2
400 grit stone
0.45–0.55
Matte, internal parts
1.5–2°
C-3
320 grit stone
0.63–0.70
Matte, non-cosmetic
2°
D-1
Dry blast, glass bead #11
0.80–1.00
Satin texture
2–3°
D-2
Dry blast, #240 oxide
1.00–2.80
Dull texture
3–5°
D-3
Dry blast, #24 oxide
3.20–18.0
Coarse texture
5° +
Draft values are typical minimums for shallow features; deep parts need more.
10. Tolerances
Hold tight tolerances only on features that really need them.
Put general tolerances on everything and tight ones only on critical fits.
Keep critical dimensions within one mold half, not across the parting line.
High-shrink resins (PP, PE, POM, PA) need looser tolerances than PC or ABS.
Uniform walls and good cooling matter more than tight numbers on a drawing.
Commercial (0–25 mm)
± 0.10 mm
Fine (0–25 mm)
± 0.05 mm
High-shrink resins
× 1.5–2
Try it – drag the sliders
Typical achievable tolerances (stable resins such as ABS, PC)
Dimension (mm)
Commercial
Fine (extra cost)
0 – 25
± 0.10 mm
± 0.05 mm
25 – 50
± 0.15 mm
± 0.08 mm
50 – 100
± 0.20 mm
± 0.10 mm
100 – 200
± 0.30 mm
± 0.15 mm
over 200
± 0.15 % mm
± 0.08 % mm
Guide values for well-designed parts. High-shrink resins (PP, PE, POM, PA) typically need 1.5–2× these values; glass-filled grades shrink less along the flow than across it.
11. Gate Placement Strategy
Where the plastic enters decides sink, weld lines, warp and cosmetics.
Gate into the thickest section and flow from thick to thin.
Keep gate marks off cosmetic and functional surfaces.
Place weld lines away from load-bearing and visible areas.
Balance flow so all edges fill at the same time; vent the last-to-fill spots.
Edge / tab gate
general, easy to trim
Sub / tunnel gate
auto-degating, small parts
Pin-point / hot tip
top gating, 3-plate or hot runner
Try it – drag the sliders
12. DFM Checklist
Run through this list before you release a part for tooling.