Design for injection moulding: uniform wall thickness first
Plastic shrinks as it cools, and thick sections shrink more and cool more slowly than thin ones. The result is sink marks, internal voids and warpage. The basic rule is therefore to keep the wall thickness as uniform as possible throughout the part. Transitions between thicknesses should be gradual, over a length of about three times the difference in thickness.
Which thickness is sensible depends on the material. ABS and PC typically work well between about 1.2 and 3.5 mm, while PP, PA and POM can be moulded thinner. Thicker walls than necessary mean longer cycle times, and cycle time drives the unit price in production. If stiffness is needed, ribs are almost always better than thicker walls.
A part designed for 3D printing or machining often has solid sections that work there but not in a mould. We core out such sections from the back so the wall becomes uniform, and replace solid material with a network of ribs. The part becomes lighter and gets a shorter cycle time without losing stiffness.
Draft angles and parting line
All faces parallel to the tool's opening direction need a draft angle, so the part releases without scuffing. The guide value is at least 0.5–1° on polished surfaces. Textured surfaces need more, often an extra 1–1.5° per 0.025 mm of texture depth, according to the toolmaker's or texture supplier's guidance. Deep parts generally need a larger angle than shallow ones, because friction against the core increases with depth.
The parting line, where the two halves of the tool meet, always leaves a faint witness line on the part. We place it on an edge where it is not visible and does not interfere with a seal, in consultation with the toolmaker. Holes and recesses not in the opening direction need side actions or loose cores, which make the tool more expensive. A change in geometry, such as a through slot instead of a blind groove, can often remove the need entirely.
Undercuts are features that hook into the tool. They can sometimes be solved with a through opening in the base that lets a core from the other side form the hook. The technique is often used for snap fits and saves a side action. We suggest such solutions early, before the toolmaker prices the tool.
Ribs, radii and screw bosses
A rib gives stiffness without thick walls. As a guide value, rib thickness is 50–60 per cent of the wall, or less for materials prone to sink marks. Height should be no more than about three times the wall thickness and spacing between ribs at least twice. Ribs also get draft and a small radius at the root.
Sharp internal corners cause stress concentrations and poorer filling. Inside radii should be at least half the wall thickness and outside radii equal to the inside radius plus the wall thickness, so the wall stays uniform around the corner. Screw bosses are tied to the wall with ribs and kept free of thick sections. The boss wall is made about 60 per cent of the nominal wall to avoid sink marks on the visible side.
Snap fits are sized for the strain the material can take. A tongue that tapers towards the tip spreads the strain more evenly than a straight one, and a radius at the root reduces the risk of breakage. We do a simplified bending calculation and then test the function with a printed prototype.
Material choice and shrinkage
The material affects both the design and the tool. Amorphous plastics such as ABS and PC shrink little and evenly, roughly 0.4–0.7 per cent. Semi-crystalline plastics such as PP, PA and POM shrink more, often 1–2.5 per cent, and differently along and across the flow. Glass-filled grades shrink less but get direction-dependent properties.
Snap fits work best in tough materials such as PP, PA and POM, which tolerate more strain than PC and ABS. PP suits living hinges, which can be flexed thousands of times without breaking. We choose the material for temperature, chemical, stiffness and surface requirements and state the designation on the drawing. We describe how material choice ties in with the product's requirements in the guide from idea to product. The shrinkage itself is compensated by the toolmaker, who enlarges the cavity. Our job is to state the material clearly and avoid geometry that shrinks unevenly, such as large flat areas without ribs.
Test with a prototype before ordering the tool
A mould is hard and expensive to change once the steel has been machined. So we test the geometry first with 3D-printed prototypes. Fit, snap fits and assembly can be evaluated, even though a print never has exactly the same properties as a moulded part. More on the process is under product development and prototyping. Sometimes it also pays to order a simpler aluminium prototype tool for the first parts.
When the design is finished, the toolmaker receives a STEP file and a drawing. It shows critical dimensions, surfaces with finish requirements and where the gate and ejector pins may be placed. We do not run mould flow simulations ourselves, but we deliver clean data to whoever does the analysis. Enclosures are a common application – see electronics enclosure design.
Think about the markings too. The material code to ISO 11469, date stamp and cavity number go on a hidden face. We build them into the model from the start, so the toolmaker does not have to add them afterwards.
Guide values for injection moulded plastic parts
| Parameter | Guide value |
|---|---|
| Wall thickness ABS | approx. 1.2–3.5 mm |
| Wall thickness PP | approx. 0.8–3.8 mm |
| Wall thickness PA (PA6, PA66) | approx. 0.8–3.0 mm |
| Wall thickness PC | approx. 1.0–3.8 mm |
| Wall thickness POM | approx. 0.8–3.0 mm |
| Draft angle, polished surface | at least 0.5–1° |
| Draft angle, textured surface | an extra approx. 1–1.5° per 0.025 mm texture depth |
| Rib: thickness / height / spacing | 50–60 % of wall / ≤ 3 × wall / ≥ 2 × wall |
| Radii | inside ≥ 0.5 × wall, outside = inside + wall |
| Shrinkage | ABS and PC approx. 0.4–0.7 %; PP, PA and POM approx. 1–2.5 % |
Guide values for unfilled materials. The material supplier's data sheet and the toolmaker's experience take precedence over the table.
What we need from you
- 3D model in STEP or an existing printed prototype
- Function and environment: load, temperature, chemicals, UV light and food contact
- Preferred material or the requirements that drive the material choice
- Visible surfaces and requirements for finish or texture
- Expected annual volume
- Parts the part is assembled to: screws, inserts and other plastic parts
- Contact details for the toolmaker, if one has already been chosen
Typical projects
- Housing and lid for electronics
- Snap fits and clips
- Handle with ribs instead of solid material
- Jar with screw lid
- Lid with a living hinge in PP
- Wheels and rollers
- Cover with screw bosses and threaded inserts
- Redesign of a printed part for production
- Bracket in glass-filled PA
- Parts with a textured surface
What affects price and lead time
- How much of the existing geometry has to change
- Number of side actions and loose cores to be designed out
- Snap fits, living hinges and threads
- Number of parts that must fit together in an assembly
- Number of prototype rounds before ordering the tool
- Revisions after the toolmaker's feedback
What you get
- STEP for the toolmaker
- Draft angle and wall thickness check across the whole part
- Proposal for parting line, gate location and ejector pins
- Drawing with critical dimensions, material and surface requirements
- Prototype files and printed test parts
- Revision management after the toolmaker's feedback
Frequently asked questions
What draft angle is needed for injection moulding?
As a guide value, at least 0.5–1° on polished surfaces in the opening direction. Textured surfaces and deep parts need more. The toolmaker can give exact values for their tool.
How thick should the wall of a moulded part be?
It depends on material and size. For ABS and PC housings, about 1.5–3 mm is common, for PP and PA often slightly thinner. Most important is that the wall is uniform.
Do you make the mould?
No. We design the part, prepare the data and help you in the dialogue with the toolmaker. The tool itself is made by a toolmaker of your choice.
Can a 3D-printed part be redesigned for injection moulding?
Yes. We make the walls uniform, add draft angles and ribs and remove features that need side actions. The part often becomes both lighter and stronger.
What causes sink marks?
Thick sections that shrink more than their surroundings, often at ribs and screw bosses. They are avoided with uniform wall thickness, thinner ribs and cored-out sections.
Do I need a mould flow simulation?
For large or thin-walled parts and high cosmetic demands it is often worth it. The toolmaker or a specialist usually does the analysis, and we deliver data prepared for it.