SOLIDWORKS Design Approach · Part 20
The shape the machine can actually release
Machining can only produce surfaces a tool can reach. Injection moulding can produce almost any shape in plastic — provided the part will come out of the mould, which is a design problem long before it is a tooling one.
Positioning
Why moulding, and where it wins
Machining is limited to surfaces accessible to machine tools — shapes without excessive complexity and without geometry that is hard to reach. Injection moulding is capable of producing almost any shape in plastics and polymers, and it does so cyclically: molten plastic is forced under pressure into a cavity that gives it shape.
The list of moulded products is long — bottles, toothbrushes, closures, vehicle components, wiring parts — and the industries using it span medical, consumer, automotive, health care and toys. Moulded part sizes run from the smallest components in medical devices to complete vehicle body panels.
That last figure is the constraint that governs everything else. Because the tool is expensive and slow to modify, part design errors that would be trivial in a machined component become extremely expensive here. Injection moulding rewards design discipline more than almost any other process.
Equipment
The injection moulding machine
Injection moulding requires a machine much as machining requires a machine tool, and with an appropriately designed mould that fits it, one machine can make a wide variety of parts. Machines come in horizontal and vertical configurations, with horizontal the common arrangement. The frame is long and relatively narrow, controlled electronically, and shows few externally visible moving parts.
The cycle
Making one part is called a cycle, and it has four stages in fixed order.
Clamping
The clamping unit secures the mould halves before any plastic is injected.
Injection
The barrel receives pellets from the hopper. A rotating screw slides axially, pushing pellets forward; at the heater zone they melt, and the screw drives the melt through the nozzle into the cavity, which it fills.
Cooling
The plastic begins cooling the moment it touches the mould. The clamping unit holds the halves tightly, pressing core into cavity firmly to prevent leakage.
Ejection
After the preset cooling period the screw retracts, the clamp opens, and ejectors release the part from the core.
Tooling
Classifying moulds
Mould designers design the tools; toolmakers make them, using precision machining techniques that combine turning, milling, grinding, EDM and polishing. Moulds can be classified along four independent axes.
| Classified by | Types | Design implication |
|---|---|---|
| Number of cavities | Single-cavity; multi-cavity | Multi-cavity multiplies output per cycle and demands balanced filling across cavities. |
| Construction | Two-plate; three-plate; side-action; stack | Side-action moulds use slides or lifters to form undercuts and add significant cost and cycle time. |
| Ejection | Pin-eject; stripper-eject | Pins push locally and can mark the part; a stripper pushes around the perimeter, which suits thin-walled cup-like shapes. |
| Runner system | Cold runner; hot runner; hot-to-cold runner | Hot runners eliminate runner scrap and shorten cycles at higher tooling cost and complexity. |
Core and cavity
The two halves of the mould. The cavity forms the outer surfaces of the part; the core forms the inner surfaces and the part normally stays on the core when the mould opens, which is why ejection acts on the core side. The surface where the two halves meet is the parting line, and where that line runs determines a great deal about the finished part — witness lines, draft directions, achievable undercuts and the cost of the tool.
Design rules
Part design guidelines
Successful moulded production requires two things: a good mould design and a good part design. Without both, parts will be defective. These are the part-side rules.
Wall thickness
Keep it uniform and as thin as function allows. Uniform walls cool evenly, which limits warpage and sink marks; thin walls reduce part volume and shorten injection and cooling time, which is most of the cycle.
Edges and corners
Avoid sharp edges and corners. Fillet edges and round corners — sharp internal corners concentrate stress in the part and are difficult to fill.
Draft
Apply draft to every wall parallel to the parting axis, so the part releases from the mould. Insufficient draft causes drag marks, ejection damage and sometimes parts that will not come out at all.
Ribs
Strengthen the part with ribs rather than by thickening the wall — which would violate rule 01. Orient ribs perpendicular to the axis about which bending may occur.
Bosses
Support bosses with ribs connecting them to the nearest wall. An unsupported boss is both weak and a sink-mark generator.
Undercuts
Minimise them. Relocating the parting line or redesigning a feature will frequently eliminate an undercut altogether — and every undercut that survives requires a slide or lifter, with the cost that implies.
Wall thickness, ribs and bosses are one problem, not three. A rib that is too thick relative to the wall it joins produces a sink mark on the opposite face; a boss without ribs is weak; a boss thickened to compensate produces the same sink mark. Solving any one of them in isolation usually breaks another. Design them together, against a nominal wall thickness fixed early.
Workflow
The three phases of mould design
Industry practice separates the work into three sequential phases.
- Phase 1 — Part design The ordinary design work covered throughout this series, carried out with the moulding rules above in mind.
- Phase 2 — Prepare the part for mould design Mould designers evaluate the part thoroughly before it is approved for tooling, because they must be certain the corresponding mould can be made and will work. The evaluation comprises draft analysis, undercut analysis and parting line analysis. Draft analysis confirms the part can be ejected. Undercut analysis confirms it can be ejected safely. Parting line analysis lets the designer investigate several pull directions and select the best one. Flow and temperature analysis of the melt inside the core and cavity also belongs here, performed with specialist mould-flow software.
- Phase 3 — Mould design Creating the core, cavity, feed system, cooling channels, ejection system and mould base.
A part that fails draft or undercut analysis does not proceed — it returns to Phase 1. Treating the evaluation as a review to be passed rather than an analysis to be acted on is how tooling ends up carrying slides that a five-minute geometry change would have removed.
In the CAD system
Tooling split and shut-off surfaces
CAD mould design modules implement these concepts directly, and two of them are worth understanding in detail because they are where the work actually happens.
- Tooling split
- The technique that divides a block enclosing the part model into core and cavity. It uses the parting line, the parting surfaces and the shut-off surfaces to make the division.
- Shut-off surfaces
- Surfaces that close open regions with holes in them, so that core and cavity can be separated at all. A face with no holes needs no shut-off; a block with a central hole does — without one, core and cavity remain connected through the hole and the split fails.
- Parting surfaces
- The surfaces extending outwards from the parting line to the edge of the tooling block, forming the sealing face between the two halves.
The toolbar in a typical mould module is organised in four groups that map onto the workflow: surfaces, which provide the surface types used to build parting and shut-off geometry; preparation, which includes scaling for shrinkage and applying draft; analysis, covering draft, undercut and parting line checking; and tooling, which performs the split itself.
CAD systems support the three design phases and validate the geometry, but generally do not provide mould-flow analysis. Where filling, packing, cooling and warpage predictions are required, models are exchanged with specialist analysis software — and STEP is the appropriate exchange format, for the reasons set out in Part 17.
Shrinkage
One preparation step deserves particular attention. Plastics shrink as they cool, so the cavity must be cut larger than the finished part by a scale factor specific to the material, the wall section and the process conditions. The scale is applied to the model before the split. Omitting it produces a tool that makes parts uniformly undersized — consistently, and irreversibly, since the correction requires removing metal that was never left there.
Key takeaways
- Moulding produces geometry machining cannot reach, at very low unit cost and very high tooling cost — which is why part design discipline matters most here.
- The cycle is clamping, injection, cooling, ejection; cooling dominates cycle time and is driven by wall thickness.
- Moulds classify by cavity count, construction, ejection method and runner system; each choice trades tooling cost against cycle and scrap.
- Uniform thin walls, filleted corners, adequate draft, ribbed and supported bosses, and minimal undercuts are the six part-design rules — and wall, rib and boss must be designed together.
- Phase 2 evaluation — draft, undercut and parting line analysis — is a gate that returns parts to design, not a formality.
- Tooling split needs a parting line, parting surfaces and shut-off surfaces for every hole.
- Apply shrinkage scaling before the split; omitting it produces a uniformly undersized part and an uncorrectable tool.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.