Design for Injection Moulding: 14 Rules That Cut Tooling Cost
Good injection-moulded parts are usually not complicated. They have steady walls, enough draft, clean ribs, sensible gates, and no surprise undercuts. Most tooling cost comes from the features that break those rules and have to be solved in steel.
Apply the 14 checks below before sending a STEP file. Nordmould uses the same type of checks in its free DFM review, but the cheapest time to fix geometry is still inside CAD.
Why does part design affect tooling cost so directly?
The mould tool is a precision negative of the part. Every face has to be machined, polished, vented, cooled, and released. If the part cannot pull straight from the tool, the mould needs moving steel. If the wall thickness swings too much, the process has to fight sink, warp, and variable shrinkage. If the drawing tolerances are tighter than the function needs, inspection and tool correction become part of the price.
Re-machining a tool after trial shots can cost from hundreds to thousands of euros, depending on whether the change is a small insert adjustment or a new side action. A design change before tool design usually costs an engineer's time.
Rule 1: Keep wall thickness uniform
Vary wall thickness by no more than about 15-25 % across one part where the design allows it. Thick sections cool slower than thin sections. Where they meet, the differential shrinkage creates sink marks, warpage, and internal voids. If you need stiffness, add ribs or a cored section rather than making the wall solid.
Rule 2: Stay within the recommended wall-thickness range for your material
Target a nominal wall of 1.5-3.5 mm for many engineering polymers. Thin walls below about 0.8 mm need short flow paths, high-flow grades, and careful gating. Walls above about 4-5 mm extend cycle time and increase sink risk. Flexible materials often need thicker sections for handling and tear resistance.
| Material | Recommended wall range |
|---|---|
| ABS | 1.5-3.5 mm |
| PC | 1.0-3.5 mm |
| PP | 1.5-4.0 mm |
| POM | 1.5-3.5 mm |
| PMMA | 1.5-3.5 mm |
| TPE / TPU | 1.5-5.0 mm |
Rule 3: Add draft angles to every vertical face
Add at least 1° of draft to pull-direction faces where the design allows it. Zero-draft walls scrape on ejection, mark the surface, grip the tool, and can damage thin features. Smooth, shallow faces may work with less, but that needs moulder approval. Textured faces need more draft, often 3-5° depending on texture depth.
Rule 4: Proportion ribs correctly
Keep rib thickness around 40-60 % of the adjacent wall for cosmetic parts, and limit rib height to about 2.5-3.0x the nominal wall. A rib that is too thick behaves like a local thick wall and leaves a sink mark on the opposite face. A rib that is too tall is hard to fill, vent, cool, and eject. Add a root radius, commonly around 0.25x the rib thickness, without creating a heavy mass at the base.
Rule 5: Design bosses to the correct proportions
Boss outer diameter should usually be 2-3x the screw or insert diameter, with boss wall thickness around 40-60 % of the nominal wall. Thin bosses crack under assembly load. Thick bosses sink the opposite face. Support bosses with gussets or ribs instead of leaving them as tall freestanding tubes.
Rule 6: Eliminate undercuts wherever possible
Re-orient or re-partition the part to avoid features that prevent straight pull from the tool. Side holes, hooks, windows, and inward-facing lips may need side actions, lifters, collapsible cores, or hand-loaded inserts. Each added mechanism increases tool cost, tool-build time, maintenance, and tolerance stack-up. If an undercut is functional, flag it in the RFQ instead of letting the toolmaker discover it later.
Rule 7: Place the parting line deliberately
Choose a parting line that follows a natural edge and keeps visible surfaces on the cavity/A-side where possible. A poor parting line leaves flash or a witness line on a sealing, sliding, or visible face. The parting line also decides which surfaces need draft in which direction, so it should be reviewed before the model is frozen.
Rule 8: Specify gate location and accept weld lines on non-critical faces
Agree the gate location before tooling begins. The gate leaves a mark, drives the filling pattern, and decides where weld lines form. Weld lines can reduce strength, especially in filled materials or around holes, but the loss depends on resin, temperature, pressure, venting, and flow-front angle. Put weld lines away from snap hooks, bosses, clips, pressure seals, and cosmetic A-surfaces.
Rule 9: Round all internal corners with a generous radius
Use an internal radius of at least 0.5 mm on small parts; for stronger design, target about 0.5x the nominal wall. Sharp internal corners concentrate stress in the moulded part and in the tool steel. External edges can be smaller for appearance, but they still benefit from a light radius to improve flow and reduce handling damage.
Rule 10: Core out thick sections
Replace solid thick masses with cored geometry: a uniform shell with ribs or internal webs. Solid sections above about 4-5 mm cool slowly, show sink, trap voids, and extend cycle time. A blind pocket on the non-cosmetic side is often enough to remove mass without changing the outside shape.
Rule 11: Apply tolerances only where function demands it
Reserve tight tolerances, such as ±0.05 mm, for mating interfaces, snap fits, sealing surfaces, and functional datums. Over-toleranced drawings force slower processing, more tool correction, and more inspection. Non-functional faces, inside ribs, and hidden walls should use standard moulding tolerances unless there is a clear reason.
Rule 12: Design self-mating snap fits with the correct engagement geometry
Calculate snap-fit strain from the selected resin and beam geometry. For ABS or PC, 2-4 % strain at maximum deflection can be a useful early target, but the actual limit depends on grade, notch sensitivity, moulded-in stress, temperature, and assembly cycles. Taper the beam so stress is spread along its length, and leave clearance under the hook for deflection.
Rule 13: Account for insert moulding requirements at the design stage
If the part uses metal inserts, design the plastic around the insert drawing and assembly load. The tool must locate the insert repeatably, protect it from flash, and eject the part without pulling the insert loose. State the thread standard, insert material, plating, pull-out requirement, torque requirement, and whether the insert is moulded in or heat-staked after moulding. Nordmould can review insert moulding feasibility during DFM.
Rule 14: Avoid feature depths that exceed the practical ejection ratio
Keep blind-hole depth below about 2x the hole diameter for simple uncooled cores, and below about 4x only where tooling and cooling support it. Deep, narrow cores flex under injection pressure, drift off-centre, trap heat, and make ejection harder. If a deep accurate hole is critical, drilling or milling after moulding may be cheaper and more stable.
How Nordmould applies these rules
Nordmould's free DFM review checks the main geometry risks before tooling: wall thickness, draft, ribs, bosses, undercuts, gate access, ejector risk, cosmetic faces, and tolerance priorities. The output should identify the features that affect cost or quality and suggest practical geometry changes.
For complex assemblies, filled materials, thin walls, or tight-tolerance parts, mould-flow simulation can be quoted to confirm fill pattern, weld-line location, pressure demand, and cooling risk before the tool is cut. Whether simulation is needed depends on the part and production tier; it should be agreed during quoting.
Frequently asked questions
What is DFM in injection moulding? Design for Manufacturability (DFM) is the practice of optimising part geometry for injection moulding before tooling begins. Nordmould provides a free written DFM review for new moulding projects.
How much does poor DFM add to tooling cost? Undercuts, non-uniform walls, and missing draft angles are common causes of tooling rework. A single unresolved undercut can add side actions, lifters, extra machining, and hundreds or thousands of euros in tool cost.
What is the recommended wall thickness for ABS injection moulding? For ABS, a uniform wall of 1.5-3.5 mm is a good starting target. Thinner walls need short flow paths and careful gating; thicker walls increase sink and cycle time. Nordmould checks wall thickness during DFM.
How much draft angle does an injection-moulded part need? Most pull-direction walls should have at least 1° of draft per side where the design allows it. Textured or engraved surfaces often need 3-5°. Low-draft faces should be agreed before tooling because they affect ejection and surface quality.
Can I have undercuts in an injection-moulded part? Yes, but each undercut must be solved with a side action, lifter, collapsible core, hand-loaded insert, or part redesign. During DFM, Nordmould may recommend eliminating or re-orienting undercuts where the function allows it.
What is the maximum rib height-to-thickness ratio? Keep rib thickness around 40-60% of the nominal wall for cosmetic parts, with rib height usually below 2.5-3.0x the nominal wall. Taller or thicker ribs need careful review because they can cause sink, fill problems, and ejection drag.
Does gate location affect part quality? Yes. Gate location controls fill pressure, weld-line position, fibre orientation, shrinkage, and the visible gate mark. Gate position should be proposed during DFM and agreed before tooling starts.
Submit your STEP file to Nordmould for a free DFM review before tooling starts.
Last reviewed: 2026-05