A 3D file that looks great on screen is not necessarily mouldable. Plastic design rules (Design for Manufacturing, or DFM) exist to prevent production defects, reduce tooling costs and guarantee repeatability in series. This guide covers the critical points: wall thicknesses, draft angles, ribs, undercuts, gate locations and tolerances.
1. Wall thickness: uniformity above all
This is rule number one in plastic part design. Unlike metal machining, injection moulding is very sensitive to abrupt thickness changes. A thick wall next to a thin wall creates two different cooling rates, generating sink marks (surface depressions) or warpage (post-demoulding distortion).
Practical rule: aim for consistent wall thickness throughout the part. If an area needs extra stiffness, do not thicken it - add ribs on the back face. If an area must be hollow or lightened, core it out and reinforce with a ribbed lattice. Any transition between two wall thicknesses must be gradual (ramped or filleted), never a sharp step.
Typical thicknesses by material: ABS 1.5-3 mm, PP 1.0-3.5 mm, PA6/PA66 1.5-3 mm, PC 2.0-4.0 mm, POM 1.5-3.0 mm. These are guidelines, not absolutes: rheological analysis confirms the optimum values for each geometry.
2. Draft angles: the non-negotiable condition for demoulding
A plastic part must be able to leave the mould without being torn or scratched. Every vertical wall must carry a slight angle relative to the mould opening axis: this is the draft angle.
Minimum value: 1 degree per face for a smooth surface. If the part carries a texture (orange peel, leather grain), the angle must increase with grain depth: add 1 to 2 degrees per 0.025 mm of grain depth. A textured mould with 0 degrees draft systematically tears the surface on every cycle.
Internal surfaces (inside a housing, for example) also need their own drafts, often in the direction opposite to the main opening. Internal cores (pins, slides) have their own separate drafts to define. A false-colour DFM visual analysis (green for correctly drafted zones, red for locked zones) is the standard tool for file checking before launch.
3. Ribs: stiffness without thickness
When a part must be stiff but light, you do not thicken it - you add ribs. Ribs are internal fins that increase the cross-section moment of inertia without increasing wall thickness.
Rib sizing rules: maximum height equal to 3 times the adjacent wall thickness (beyond this, visible sink marks appear on the opposite face), rib thickness 50-60% of wall thickness, base radius 0.25-0.5 times wall thickness, minimum draft angle 0.5 degrees per rib face.
Common issue: ribs that are too tall or too thick create visible sink marks on the aesthetic face opposite them. This is the most frequent problem on ABS-injected housings with many internal ribs. Solution: reduce individual rib thickness and increase their number rather than their individual height.
4. Radii and fillets: mechanical strength and flow
Sharp corners concentrate mechanical stresses and create turbulence in the flow of molten plastic. A right-angle corner is a potential fragility point and a weld-line zone.
General rule: add radii wherever possible, especially at wall-to-floor junctions, wall-to-rib junctions and around through-holes. Minimum recommended radius: 0.5 mm internal radius, 1.0 mm external radius for stressed zones. Aesthetic zones can carry larger radii depending on design intent.
A well-placed radius also improves fill: molten plastic flows better through a rounded profile than a sharp corner. This translates into lower injection pressure, more uniform fill and reduced risk of short shots.
5. Undercuts: the enemies of a simple mould
An undercut is any geometry that prevents direct demoulding along the main mould opening axis. Common examples: a lateral clip, a hole perpendicular to the opening axis, a groove or hook.
The tooling impact is direct: every undercut requires an additional mechanism in the mould (slide, lifter, removable insert). Each mechanism increases complexity, tooling cost and maintenance risk. On a simple mould, a well-identified undercut can sometimes be eliminated by a minor design change (part rotation, clip re-orientation) without affecting function.
Our systematic approach: before validating a 3D file, we identify all undercuts, quantify the mould impact and propose design alternatives where function allows. This approach can significantly reduce tooling complexity.
6. Gate location: position and impact on the part
The gate position determines the plastic flow direction inside the mould, and therefore the weld lines, molecular orientation, residual stresses and surface appearance.
Basic rules for gate positioning: place the gate on a non-aesthetic zone (hidden face, flank), direct flow towards the thickest zones (flow naturally takes the path of least resistance), avoid gates directly opposite cores or obstacles (risk of visible weld lines), prefer a gate equidistant from part edges for balanced fill.
Common gate types: direct sprue gate (visible mark), submarine gate (mark below parting surface, hidden), fan gate (for wide flat parts), tunnel gate (mark at sprue tip, automatic). The choice of gate type affects tooling cost and the quality of the residual mark on the part.
7. Tolerances: what is actually achievable in injection moulding
Plastic injection tolerances are not the same as metal machining tolerances. Plastic shrinks on cooling (shrinkage rates range from 0.3% for PC to 2% for PP), and this shrinkage varies with flow orientation, local thickness and cooling conditions.
Typical achievable injection tolerances: general dimensions +/- 0.1 to +/- 0.3 mm depending on part size and material, critical dimensions (guides, shafts) +/- 0.05 to +/- 0.1 mm with precise process control, flatness and warpage: difficult to guarantee below 0.2 mm without prior rheological analysis and mould-flow simulation. Tighter tolerances are possible but require upfront simulation and sometimes post-moulding calibration.
8. LGR Design Studio partnership: from sketch to production file
Moulding Injection works in partnership with LGR Design Studio (engineering office, Wavre, in-house CNC). This collaboration handles projects from the product design stage: converting a sketch into a 3D file, integrating DFM constraints from the outset, rheological analysis (injection simulation) and a documented DFM report before mould launch approval.
Practical outcome: clients who go through this design stage before commissioning tooling avoid costly modifications during manufacture. A mould corrected after machining costs more and takes longer than a design revised upstream on file.
9. Common DFM errors and how to fix them
Zero draft on textured surfaces: fix by adding the required draft angle before texturing is applied. Uniform thick walls: core out and replace with a ribbed structure. Abrupt thickness transitions: replace with tapered or ramped transitions. Lateral undercut with clip: consider converting the clip to a snap-fit on the parting plane. Gate on a visible aesthetic face: relocate to a hidden zone or switch to a submarine or tunnel gate.
10. Send us your 3D file for a DFM review
Send your 3D file (STEP or IGES preferred) or your sketch. We carry out the DFM analysis, document the critical points and propose technical remedies. DFM report within 5 working days, no commitment required.
FAQ
FAQ
What is DFM in plastic injection moulding?
DFM (Design for Manufacturability) is the analysis of a 3D file from a plastic injection manufacturability perspective. It verifies draft angles, wall thicknesses, sink mark risks, undercuts and gate locations before mould manufacture is launched. The goal is to identify and correct problems on file rather than during production.
What is the minimum wall thickness in plastic injection moulding?
Minimum thickness depends on material and geometry. As a guide: ABS 1.5 mm, PP 1.0 mm, PC 2.0 mm, PA6 1.5 mm. Below these values, molten plastic may not fully fill the cavity (short shot). Rheological analysis confirms the minimum value for each specific part.
What is the minimum draft angle in plastic injection moulding?
The minimum angle is 1 degree per face for a smooth surface. For a grained or textured surface, add 1-2 degrees per 0.025 mm of grain depth. A textured surface with no draft systematically tears during demoulding. Internal surfaces have their own drafts to define independently.
Does an undercut always increase tooling cost?
Yes, unless it can be eliminated by a design modification. Every undercut requires an additional mechanism (slide, lifter) that increases mould complexity and manufacture time. We systematically analyse whether an undercut can be removed by a minor design change before validating the addition of a mechanism.
What tolerances are achievable in plastic injection moulding?
For general dimensions, expect +/- 0.1 to +/- 0.3 mm depending on material and part size. For critical dimensions (shafts, guides), +/- 0.05 to +/- 0.1 mm with precise process control. Material shrinkage (0.3% for PC, up to 2% for PP) is the main variable to control, and it is modelled upstream by rheological simulation.
