Design for Injection Moulding: 14 Rules That Cut Tooling Cost
Good injection moulding design follows a set of well-understood rules. Apply all 14 below before submitting your STEP file and you will avoid the most common causes of tooling rework, extended lead times, and scrap. Nordmould applies these checks as part of its free DFM review — but the earlier you apply them in CAD, the lower your tooling cost.
Why does part design affect tooling cost so directly?
The mould tool is a precision negative of your part. Every feature that is difficult to demould, fill, or inspect must be solved in the tool — with additional steel, more machining time, or moving components. Re-machining an already-built tool typically costs €500–3,000 per change. Design changes made before tooling begins cost nothing.
Rule 1: Keep wall thickness uniform
Vary wall thickness by no more than 15–25 % across a single part. Thick sections take longer to cool than thin ones. Where they meet, the differential shrinkage creates sink marks, warpage, and internal voids. If you need structural mass, add ribs rather than increasing wall thickness.
Rule 2: Stay within the recommended wall-thickness range for your material
Target a nominal wall of 1.5–3.5 mm for most engineering polymers. Thin walls below 0.8 mm risk short shots on long flow paths; walls above 4 mm extend cycle time and increase sink risk. The table below gives material-specific guidance.
| 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 | 2.0–5.0 mm |
Rule 3: Add draft angles to every vertical face
Add at least 1° of draft to all faces parallel to the direction of pull. Zero-draft walls grip the tool during ejection, causing drag marks, part sticking, and eventual tool damage. Textured surfaces need more — typically 3–5° depending on texture depth. Draft must be added before tooling is cut; retrofitting it requires re-machining.
Rule 4: Proportion ribs correctly
Keep rib thickness at 50–70 % of the adjacent wall, and limit rib height to 3× the nominal wall. Ribs that are too thick draw material away from the opposite face and leave a sink mark. Ribs that are too tall are difficult to fill and demould. Always add a radius of 0.25–0.4× the rib thickness at the base.
Rule 5: Design bosses to the correct proportions
Boss outer diameter should be 2–3× the insert or screw diameter; boss wall thickness should be 40–60 % of the nominal wall. Bosses that are too thin crack under assembly loads. Bosses that are too thick cause sink on the cosmetic face opposite. Connect bosses to walls or ribs with gussets rather than leaving them standing free.
Rule 6: Eliminate undercuts wherever possible
Re-orient or re-partition your part to avoid any feature that prevents straight pull from the tool. Holes, hooks, and recesses that point sideways or inward require side actions, lifters, or collapsible cores — each one adds €500–2,000 to tooling cost and introduces a wear surface that widens tolerances over time. When undercuts are unavoidable, flag them explicitly in your STEP submission.
Rule 7: Place the parting line deliberately
Choose a parting line that runs along the sharpest geometric edge of the part and keeps cosmetic surfaces in the cavity (B-side). A poorly placed parting line leaves a flash witness line on a functional or visible face. The parting line also determines which surfaces need draft in which direction — so it is a primary DFM decision, not a detail.
Rule 8: Specify gate location and accept weld lines on non-critical faces
Agree the gate location before tooling begins. The gate is where plastic enters the cavity; it leaves a witness mark and, on parts with multiple flow fronts, generates weld lines where flows meet. Weld lines are weaker than the bulk material — 20–40 % strength reduction is typical. Place them away from load-bearing features and out of cosmetic view.
Rule 9: Round all internal corners with a generous radius
Use a minimum internal corner radius of 0.5 mm; 1.0 mm or more is preferred. Sharp internal corners concentrate stress during ejection and in service. They also create stress risers in the tool steel itself, leading to premature cracking of the cavity. External corners carry less risk but still benefit from a small radius for appearance.
Rule 10: Core out thick sections
Replace solid thick sections with cored geometry — a uniform-thickness shell with internal webs. Solid sections above 4 mm cool slowly, create sink marks, and trap voids. Coring reduces material cost, shortens cycle time, and improves dimensional stability. The core does not need to be accessible from outside the part — a blind pocket on the B-side is sufficient.
Rule 11: Apply tolerances only where function demands it
Reserve tight tolerances (±0.05 mm or better) for mating interfaces, snap fits, and functional features only. Over-toleranced drawings force slower cycle times, tighter process control, and higher inspection cost across the entire run. Non-functional faces, interior walls, and cosmetic surfaces should remain at standard commercial tolerance. Nordmould's DFM review routinely identifies over-toleranced drawings and recommends relaxing non-critical specs.
Rule 12: Design self-mating snap fits with the correct engagement geometry
Snap-fit deflection beams should be designed to 2–4 % strain at maximum deflection for ABS or PC. Exceeding the elastic limit causes permanent deformation or fracture on first assembly. Taper the beam so the root is thicker than the tip — this distributes bending stress evenly. Add clearance under the hook to allow deflection without contacting the tool wall.
Rule 13: Account for insert moulding requirements at the design stage
If your part requires metal inserts, design the boss geometry around the insert dimensions and specify the insert standard (e.g., DIN 16903) before tooling begins. Inserts must be positioned by the tool, which requires pockets or pins. Retroactively adding insert pockets to a finished tool is a significant rework cost. Nordmould offers insert moulding as a standard capability — state the requirement in your STEP submission.
Rule 14: Avoid feature depths that exceed the practical ejection ratio
Keep blind-hole depth below 2× the hole diameter for cores without internal cooling, and below 4× for cores with cooling channels. Deep, narrow cores flex under injection pressure, drift off-centre, and are difficult to eject cleanly. Where deep holes are functionally required, consider drilling or milling as a secondary operation after moulding.
How Nordmould applies these rules
Nordmould checks all 14 rules — and several secondary ones — during the free DFM review. You receive a written manufacturability note within 2 business days of submitting your STEP file. The note identifies specific features that will cause problems, ranks them by cost impact, and suggests geometry changes. No obligation to proceed with tooling follows a DFM review.
For complex assemblies or tight-tolerance parts, Nordmould can run mould-flow simulation to confirm fill, predict weld-line location, and validate cooling before the tool is cut. This is offered as an optional paid service and is included as standard in the Production tier.
Frequently asked questions
What is DFM in injection moulding? Design for Manufacturability (DFM) is the practice of optimising part geometry for the injection moulding process before tooling begins. Nordmould provides a free written DFM review for every new project.
How much does poor DFM add to tooling cost? Undercuts, non-uniform walls, and missing draft angles are the three most common causes of tooling rework. In Nordmould's experience, a single unresolved undercut can add €500–2,000 in side-action or lifter costs.
What is the recommended wall thickness for ABS injection moulding? For ABS, a uniform wall of 1.5–3.5 mm is the standard target. Thinner walls risk incomplete fill; thicker walls cause sink marks and long cycle times. Nordmould checks wall thickness in the free DFM review.
How much draft angle does an injection-moulded part need? Most external surfaces need at least 1° of draft per side. Textured or engraved surfaces need 3–5°. Nordmould flags zero-draft faces in the DFM review because they cause part sticking and tool damage.
Can I have undercuts in an injection-moulded part? Yes, but every undercut adds a side action, lifter, or collapsible core to the tool — each one adds cost and lead time. Nordmould recommends eliminating or re-orienting undercuts during DFM where possible.
What is the maximum rib height-to-thickness ratio? Keep rib height below 3× the nominal wall thickness and rib thickness at 50–70 % of the wall. Taller or thicker ribs cause sink marks on the opposite surface. Nordmould checks all rib proportions during DFM.
Does gate location affect part quality? Yes. Gate location controls weld-line position, fill pressure, and cosmetic appearance. Nordmould proposes gate locations during the DFM review and agrees them with the customer before tooling starts.
Submit your STEP file to Nordmould for a free DFM review — receive a written manufacturability note with specific geometry recommendations within 2 business days, at no obligation.
Last reviewed: 2026-05