The complete interactive reference for wall thickness, ribs, bosses, draft, undercuts, snap fits, and more
1. Wall thickness
The single most impactful design decision - affects cycle time, cost, strength, and defects
Click the dots to explore wall thickness rules
Uniform wall thickness is the foundation of good injection molding design. Every other design rule builds on it.
Material wall thickness ranges
ABS
1.1 - 3.5 mm
Polycarbonate
1.0 - 4.0 mm
Polypropylene
0.8 - 3.8 mm
Nylon (PA)
0.8 - 3.0 mm
Polyethylene
0.8 - 5.0 mm
POM (Acetal)
0.8 - 3.0 mm
Key rules
Keep wall thickness uniform throughout the part
Where thickness must change, use a 3:1 taper ratio
Thinner walls = faster cooling = shorter cycle time
Cooling time grows with the square of wall thickness
Minimum wall depends on flow length and material
2. Draft angles
Draft allows parts to release cleanly from the mold without damage or drag marks
Draft angle guidelines
Smooth surfaces
1 - 2 deg per side
Textured surfaces
1.5 deg + 1 deg per 0.025 mm texture depth
Ribs
0.5 - 1 deg minimum
Bosses (inner)
0.5 - 1 deg
Bosses (outer)
0.5 - 1 deg
Deep draws (>50mm)
Add 0.5 deg extra
Why draft matters
Without draft, parts grip the core during ejection, causing drag marks, scratches, distortion, or even broken ejector pins. Textured surfaces need extra draft because the texture creates micro-undercuts. Always apply draft in the direction of mold pull.
3. Rib design
Ribs add stiffness without increasing wall thickness - but only when sized correctly
Click the dots to explore rib design rules
Ribs are the most effective way to add stiffness. Multiple thin ribs outperform one thick rib.
Rib dimension rules
Rib thickness 0.5 - 0.6x wall (T)
Rib height ≤ 3x wall (T)
Rib spacing ≥ 2x wall (T) apart
Base radius 0.25 - 0.4x T
Draft per side 1 - 2 deg minimum
Top thickness Slightly narrower (draft)
Pro tip: use multiple thin ribs
If a single rib is not stiff enough, add parallel ribs rather than making one rib thicker. Three ribs at 0.5T give far more stiffness than one rib at 1.5T - without sink marks. Cross-ribs (grid pattern) provide stiffness in two directions.
4. Boss design
Screw bosses, alignment bosses, and insert bosses - all follow the same wall-ratio logic
Standalone boss
Boss wall = 0.5-0.6x T. OD = 2x screw diameter. Max height = 3x OD. Core from below to at least 2/3 of height. Fillet radius at base ≥ 0.25x T.
Gusseted boss
Add gussets when height exceeds 2x OD. Gusset thickness = 0.5x T. 3-4 gussets evenly spaced. Essential for high-torque screw applications and tall bosses.
Wall-attached boss
Never attach boss directly flush to a wall. Connect via a thin rib (≤ 0.6x T). Offset boss from wall by at least 2x T to avoid thick section accumulation.
Insert boss
For heat-set or ultrasonic inserts: boss OD = insert OD + 2x wall. Allow 0.1-0.2 mm radial clearance for knurls. Boss wall can be 0.6-0.8x T for insert expansion.
5. Radii and fillets
Sharp corners are the enemy: they concentrate stress, impede flow, and weaken the mold
✗ Sharp corner
✓ Filleted corner
Fillet and radius rules
Inside radius: minimum 0.5x wall thickness (T)
Outside radius: inside radius + wall thickness
Ideal inside radius: 0.75x T (best flow)
Never use zero radius - causes 3x stress concentration
Consistent radii improve flow and reduce cycle time
Too-large fillets create thick sections (same as boss issue)
Fillet at parting line: use 0 or match parting to avoid flash
6. Undercuts
Features that prevent straight mold pull - need side actions, lifters, or design workarounds
External undercut
Hole, slot, or protrusion on the outside of the part perpendicular to mold pull. Requires side action (cam, slide).
Internal undercut
Internal thread, groove, or barb inside the part. Requires collapsible core, unscrewing mechanism, or lifter.
Snap-fit undercut
Intentional barb for snap assembly. Can sometimes be ejected by deflection (bumped off) if material is flexible enough.
Side actions (slides/cams)
Moving mold components that retract perpendicular to the pull direction before the mold opens. Adds mold cost (15-30% per action) and maintenance. Most common solution for external undercuts like side holes and windows.
Lifters
Angled internal components that move both vertically and laterally during ejection. Used for internal undercuts. Less expensive than side actions but limited in travel distance. Common for internal clips and hooks.
Collapsible cores
Multi-segment cores that collapse inward to release internal undercuts like threads. Complex and expensive but necessary for features like bottle caps and threaded closures.
Bump-off (stripping)
Part deflects over the undercut during ejection. Only works for flexible materials (PP, PE, TPE), shallow undercuts (max 2-5% of diameter), and features with lead-in ramps. Lowest mold cost option.
Design strategies to eliminate undercuts
Reorient the part to align features with pull direction
Use snap fits with built-in deflection instead of rigid hooks
Replace side holes with slots open to the parting line
Use pass-through holes (core from both sides) instead of blind features
Split the part into two simpler halves that assemble together
Use shut-off (sliding shutoff) surfaces at parting line for through-holes
Replace internal threads with external snap features
Design windows as open on one edge instead of fully enclosed
7. Snap fits
Eliminate fasteners and reduce assembly cost - but design within strain limits
Cantilever snap
Most common type. A flexible beam with a hook at the end deflects during assembly and locks behind a ledge. Max strain: 2% for ABS, 1.2% for PC, 4-6% for PP. Taper the beam for even stress distribution.
Annular snap
Ring-shaped interference. The outer ring expands over a bead on the inner part. Used for caps, lids, and cylindrical assemblies. Requires uniform radial deflection. Semi-crystalline materials work best.
Torsional snap
Uses a flexing hinge or living hinge section to deflect. Less common but useful for lids and enclosures. Design the hinge section thin enough to flex without permanent deformation.
Snap fit design rules
Taper cantilever beams (thicker at root) for even stress
Add radius at the beam root to prevent stress cracking
Check material allowable strain (varies 1-8% by resin)
45 deg entry angle for easy assembly, 90 deg retaining angle for permanence
Lead-in chamfer on both mating parts for guided assembly
Lugs/guides to prevent side-loading during engagement
For repeated assembly, keep strain below 60% of max allowable
Test prototypes - FEA alone misses creep and fatigue effects
8. Living hinges
Thin flexible sections molded in one piece - only certain materials work
Living hinge geometry
Thickness: 0.20 - 0.50 mm (PP), 0.25 - 0.38 mm ideal. Generous radii on both sides (R ≥ 0.25 mm). Gate should be positioned so flow crosses perpendicular to the hinge line to orient molecules along the flex axis.
Material compatibility
Polypropylene
Excellent Best choice, flexes millions of cycles
Polyethylene
Good Works but less durable than PP
Nylon
Limited Low cycle life, needs moisture
ABS
Poor Brittle hinge, cracks quickly
Polycarbonate
Poor Not suitable for living hinges
9. Texture and surface finish
Surface finish affects appearance, grip, draft requirements, and mold cost
SPI Grade
Finish
Method
Draft needed
Use case
A-1
Mirror / lens
Diamond buff
1 deg min
Optical lenses, clear parts
A-3
High gloss
Fine diamond buff
1 deg min
Consumer electronics
B-1
Semi-gloss
600 grit paper
1 deg min
General cosmetic
C-1
Matte
600 stone
1.5 deg min
Interior parts
D-1
Sandblast
Dry blast glass bead
2 deg min
Grip surfaces
MT-xxxxx
Mold-Tech texture
Chemical etch
1.5 deg + 1 deg/0.025mm depth
Leather grain, geometric patterns
Texture draft rule of thumb
For every 0.025 mm (0.001 in) of texture depth, add 1 degree of additional draft beyond the minimum. Example: a Mold-Tech texture with 0.075 mm depth needs 1.5 deg base + 3 deg additional = 4.5 deg total draft. Without sufficient draft, the texture will drag and leave white marks on the part surface during ejection.
10. Tolerances
Tighter tolerances = higher cost. Design to the loosest tolerance that still works.
Achievable tolerances by feature
Linear dimensions
± 0.1 - 0.3 mm
Hole diameters
± 0.05 - 0.1 mm
Flatness
0.1 - 0.5 mm per 100 mm
Across parting line
Add ± 0.1 mm to above
Tight (achievable)
± 0.05 mm with process control
High precision
± 0.025 mm (specialized tooling)
Tolerance design tips
Keep critical dimensions on one side of the parting line
Use datums from features formed by the same mold half
Expect higher variation across parting line (mold alignment)
Shrinkage varies by direction (flow vs cross-flow)
Glass-filled materials have lower, more consistent shrinkage
Post-mold shrinkage continues for 24-48 hours
Amorphous resins (ABS, PC) hold tighter tolerances than semi-crystalline (PP, PA)
Test dimensional stability at expected service temperature
11. Gate placement strategy
Gate location affects fill pattern, weld lines, warpage, and cosmetics
✓ Gate placement do's
Gate into the thickest section (pack thin from thick)
Center gate for radially symmetric parts
Place gate on non-cosmetic surface
Gate into a wall to prevent jetting
Position to push weld lines to non-critical areas
Use flow simulation to predict weld line locations
Consider multiple gates for long/complex parts
Use fan or tab gates for flat parts to reduce stress
✗ Gate placement don'ts
Gate into thin sections (causes hesitation, short shots)
Gate opposite a boss or pin (creates weak weld line)
Gate on cosmetic or textured surfaces
Gate near areas with tight tolerances (high stress zone)
Place gate where it creates unbalanced flow
Gate at the end of a long flow path (pressure drop)
Ignore gate vestige in assembly areas
Use too-small a gate (excessive shear, burn marks)
12. DFM checklist
Run through this checklist before finalizing your design for tooling