Plastic Part Design for Injection Moulding: 10 Rules That Prevent Costly Rework
- Shubh Poojara
- 1 day ago
- 10 min read
Most injection moulding failures are not material failures or process failures. They are design failures — geometry that was created without knowing or applying the rules that govern how plastic flows into a cavity, cools, and ejects. The mould is just revealing what was already wrong with the drawing.
The 10 plastic part design rules in this guide are not theoretical. They are derived from the patterns we see repeatedly at PlastFab Works across our injection moulding services — the failures that show up at first article, the remakes that could have been avoided, and the decisions made during design that determined the outcome.
Apply these rules before you submit a drawing for tooling. The earlier in the design process they are applied, the cheaper the corrections are. For a broader overview of DFM across all plastic manufacturing processes, see our guide on what is design for manufacturing.
Table of Contents
Rule 1: Keep Wall Thickness Uniform
Cross-section comparison infographic: uniform wall thickness (green, correct) vs non-uniform wall with thick boss and thin section (red, incorrect) — showing differential cooling and sink mark formation
Uniform wall thickness is the most important single rule in injection moulded plastic part design. When wall sections vary significantly, the thicker sections cool more slowly than the thinner sections. The differential cooling creates internal stress that manifests as warping, sink marks, and residual stress that weakens the part in service.
The recommended nominal wall thickness range for most engineering thermoplastics is 1.5 mm to 4 mm. Within a single part, wall thickness should ideally vary by no more than 25%. Where thickness transitions are unavoidable — for example, where a rib or boss meets a thin wall — taper the transition over a length of at least 3× the wall height.
Target range: 1.5–4.0 mm nominal, depending on material and part size
Maximum variation: No more than 25% difference between adjacent wall sections
Transition rule: Taper thickness changes over a length ≥ 3× the wall height
Thick islands: Core out thick sections rather than leaving solid material — it reduces sink risk and cycle time
Rule 2: Apply Correct Draft Angles to Every Vertical Face
Draft angles are the taper applied to vertical faces — faces parallel to the direction in which the mould opens. Without draft, the part grips the mould during ejection, causing surface tearing, ejector pin marks, and in severe cases, part breakage.
Draft is not cosmetic. It is a functional requirement of the moulding process. Every vertical face needs it.
Smooth surfaces: 1° minimum per side — the industry standard for most engineering thermoplastics
Lightly textured surfaces: 1.5–2° per side — texture creates microscopic undercuts that increase friction on ejection
Heavily textured surfaces (e.g. leather grain): 3–5° per side — the deeper the texture, the more draft is required
Side cores and lifters: Features that require zero-draft faces can be accommodated with side actions in the tool, but each side action adds to tool cost and cycle time
Draft analysis — a colour heat map of all faces relative to the pull direction — should be run on every moulded part before tooling is approved. Our mold design services include draft analysis as a standard step in every tool design.
Rule 3: Design Ribs at 60% of Adjacent Wall Thickness
Ribs are one of the most effective ways to add structural stiffness to an injection-moulded part without increasing wall thickness. A rib running perpendicular to the primary load direction can double part stiffness with a fraction of the material that would be needed to achieve the same stiffness through wall thickness alone.
But ribs cause sink marks on the opposite surface if they are too thick. The mechanism is simple: a thick rib cools more slowly than the adjacent wall, the material contracts as it cools, and the surface above the rib is pulled inward.
Rib thickness: 50–60% of adjacent wall thickness — the most critical number in rib design
Rib height: Maximum 3× the wall thickness. Taller ribs are prone to filling problems and cooling differential
Rib base radius: R0.5–1.0 mm at the rib root to reduce stress concentration
Rib draft: 0.5–1.0° per side — ribs are tall thin features and need draft like all vertical faces
Rib spacing: Minimum 2× wall thickness between parallel ribs to allow the tool steel to cool adequately
Rule 4: Size Bosses Correctly for Screws and Inserts
Bosses are cylindrical features used to accept screws, heat-set inserts, or press-fit pins. Incorrectly sized bosses are one of the most common causes of first-article failures — they either strip on assembly, crack under load, or sink on the cosmetic surface.
Boss outer diameter: 2× the insert outer diameter — this provides sufficient wall thickness around the insert to resist hoop stress
Boss inner diameter: Match to the insert specification with the appropriate press or thermal fit allowance
Boss height: Maximum 3× the boss outer diameter without gussets. Taller bosses require triangular gussets connecting them to the nearest wall
Boss wall thickness: Maintain 60% of adjacent wall thickness to prevent sink marks on the opposite surface
Boss draft: 0.5° minimum on the outer diameter — bosses are tall cylindrical features and must draft like any vertical face
Rule 5: Choose Gate Location Before You Finalise Geometry
Top-view injection moulding diagram showing three gate location options on the same part — gate at thin end (incorrect, shows incomplete fill), gate at thick section (correct, shows complete fill), gate on cosmetic surface (incorrect, shows gate vestige on visible face) — with flow front paths shown
Gate location determines how the cavity fills, where weld lines form, and where the gate vestige will appear on the finished part. It is one of the most consequential decisions in injection moulded part design — and one of the decisions most frequently made too late, after the cosmetic and structural requirements have already constrained the available options.
Fill from thick to thin: Place the gate at the thickest section of the part. Plastic flows more easily through thick sections and fills thin sections last. Gating at a thin section causes premature freeze-off and short-shot risk.
Avoid cosmetic surfaces: The gate vestige (the small mark left after the runner is cut) is difficult to eliminate completely. Specify gate location on non-cosmetic faces wherever possible.
Control weld line position: Weld lines — where two flow fronts meet — form at the point furthest from the gate. Gate location controls where the weld line falls. Keep weld lines away from structural features, holes, and cosmetic surfaces.
Single gate preferred: Multiple gates introduce more weld lines. Use a single gate wherever part geometry and fill requirements allow.
Rule 6: Place the Parting Line Where You Can Hide It
The parting line is the line on the part surface where the two halves of the mould meet. It is always visible to some degree — at minimum as a faint witness mark, at worst as a step or flash line if the tool is not perfectly matched.
The parting line location is determined by the part geometry, but within the constraints of the geometry there is usually room to move it to a more acceptable position. The general rules are:
Keep it on non-cosmetic surfaces: A witness line on a back face or a mating face that is hidden in assembly is invisible in use.
Put it at a natural transition: A sharp edge, a step, or a radius break conceals the parting line better than a flat cosmetic surface.
Avoid complex curved parting lines: The more complex the parting line profile, the more expensive the tool is to make and maintain. Simple flat or stepped parting lines are significantly cheaper than curved 3D parting lines.
Account for flash: Flash — thin plastic that bleeds across the parting line — is more visible on dark colours and on flat surfaces. Specify parting line location with post-processing constraints in mind.
Rule 7: Compensate for Material Shrinkage in the Tool Dimensions
All thermoplastics shrink as they cool from melt temperature to room temperature. The amount of shrinkage is specific to the material grade, the wall thickness, and the processing conditions. If the tool is cut to nominal part dimensions, the finished part will always be undersized.
Shrinkage must be applied to the tool dimensions — the tool is made slightly oversized so that the part comes out at nominal. The typical shrinkage rates for common engineering thermoplastics are:
ABS: 0.4–0.7% — one of the lowest shrinkage thermoplastics, good dimensional stability
Polypropylene (PP): 1.5–2.5% — high shrinkage, prone to warping in asymmetric parts
Nylon PA6: 0.7–1.5% — shrinkage increases significantly with moisture absorption post-moulding
Nylon PA66: 1.0–1.5% — slightly higher than PA6, more sensitive to wall thickness variation
HDPE: 1.5–3.0% — high shrinkage, directional (higher in flow direction than transverse)
Polycarbonate (PC): 0.5–0.7% — low shrinkage, good dimensional accuracy
Shrinkage compensation must be specified on the tool design drawing, not the part drawing. The part drawing shows nominal dimensions. The tool designer applies the shrinkage factor.
Rule 8: Design Out Undercuts Where Possible
An undercut is any feature that prevents the part from releasing from the mould in the pull direction without a secondary mould action. Undercuts are not inherently wrong — but each one requires a side action, lifter, or collapsible core in the tool, and each of these adds tooling cost, maintenance complexity, and potential for flash at the action interface.
Before accepting an undercut in the design, ask whether the feature can be redesigned to eliminate it:
Through-holes: A through-hole parallel to the pull direction requires no side action. A through-hole perpendicular to pull is an undercut. Reorienting features to be parallel to pull eliminates side actions.
Snap-fit hooks: External snap-fits are typically undercuts. Design snap-fits so they can flex clear of the mould on ejection rather than requiring a side action to release them.
Threaded features: External threads are undercuts. Where threads are required, specify a threaded insert (pressed or heat-set into a boss) rather than moulding the thread directly.
Recessed logos or text: Embossed text (raised on the part, recessed in the tool) is not an undercut. Engraved text (recessed on the part) requires no side action if the text faces the pull direction.
Rule 9: Design Snap-Fits to the Strain Limits of the Material
Snap-fits are one of the most elegant features in injection-moulded part design — they create assembly without fasteners and are effectively free to manufacture since they are formed in the mould. But a snap-fit that exceeds the material's allowable strain on assembly will crack, white, or permanently deform on first use.
The critical design parameter is the deflection strain during assembly — the strain induced in the snap-fit cantilever as it deflects over the mating feature. This must stay below the material's permissible strain, which is typically 50–70% of the yield strain for a one-time assembly or 30–40% for repeated assembly (such as a battery cover).
ABS: Permissible strain 2–4% — stiff, medium snap-fit performance
Polypropylene: Permissible strain 5–8% — excellent for high-deflection snap-fits and living hinges
Nylon PA66: Permissible strain 4–6% — good snap-fit material, tough
Polycarbonate: Permissible strain 3–4% — stiffer, requires careful geometry for flexible snap-fits
Acrylic (PMMA): Permissible strain 0.5–1% — very brittle, poor for snap-fits. Avoid.
Rule 10: Place Weld Lines Away from Structural and Cosmetic Features
Weld lines — also called knit lines — form wherever two flow fronts meet in the cavity. They are inherent to injection moulding and cannot be eliminated in parts with holes, multiple gates, or complex geometry. What can be controlled is where they form.
Weld lines are the weakest point in an injection-moulded part. Tensile strength at a weld line is typically 75–85% of bulk material strength, and lower still for glass-filled grades. They are also visible on the surface, appearing as a faint line in the direction of flow.
Keep weld lines away from holes: Flow fronts splitting around a hole reunite on the downstream side. Place holes in low-stress, non-cosmetic areas.
Avoid weld lines on snap-fits and living hinges: The cyclic strain on a snap-fit at a weld line will cause fatigue failure well before the same feature in solid material.
Use gate location to move weld lines: Changing gate position moves where flow fronts meet. If a weld line is falling on a critical feature, a gate relocation study can move it to a less sensitive location.
Increase melt temperature locally: Higher melt temperature at the weld line improves molecular diffusion across the interface. If weld line strength is critical, mould processing conditions can be optimised to strengthen it.
For a full DFM review of your injection moulded part before tooling is committed, see our product design services. We review every part for draft, wall uniformity, gate location, and weld line risk before quoting tooling.
Frequently Asked Questions
What is the minimum wall thickness for injection moulding?
The practical minimum wall thickness for injection moulding is around 0.8–1.0 mm for small parts, rising to 1.5 mm for medium parts and 2.0 mm for large parts. Below these minimums, fill becomes unreliable and the risk of short shots increases. The recommended nominal for most engineering thermoplastics is 1.5–3.0 mm.
How much draft angle do I need for injection moulding?
The standard minimum is 1° per side for smooth surfaces. Textured surfaces need 2–3° depending on texture depth. As a rule: 0.025 mm of texture depth requires 1° of additional draft. Zero draft is only acceptable on features with side-action release, which adds tool cost.
Why does my injection moulded part have sink marks?
Sink marks are caused by localised thick sections — usually ribs, bosses, or thick walls — that cool more slowly than surrounding material. As the thick section cools and contracts, it pulls the opposite surface inward. The fix is to reduce the rib or boss thickness to 50–60% of the adjacent wall, or to core out thick wall sections.
Can I injection mould a part with undercuts?
Yes, but each undercut requires a side action, lifter, or collapsible core in the tool. These add tooling cost (typically ₹20,000–₹1,50,000 per action depending on complexity) and maintenance requirements. Where possible, redesign features to eliminate undercuts or to allow them to flex clear on ejection.
What causes warping in injection moulded parts?
Warping is caused by differential shrinkage — when different sections of the part cool and shrink at different rates. The main causes are: non-uniform wall thickness, asymmetric geometry, incorrect gate location, insufficient cooling time, and high-shrinkage materials like PP and HDPE in thin-walled parts. The primary design fix is wall thickness uniformity.
Great insights!