INJECTION MOULDING DESIGN GUIDE
The fundamentals of Injection Moulding
Find what you’re looking for.
Injection moulding is a formative manufacturing technology, i.e. material is formed from an amorphous shape into a fixed shape defined by a mould tool. Almost every plastic part created today is by injection moulding as it allows identical parts to be created in huge numbers, in a short space of time, and at very low cost per part.
The process works as follows:
1) A mould cavity defines the shape of the part.
2) Material (melted plastic) is injected under pressure into the cavity.
3) When the plastic cools it solidifies to take the form defined by the mould.
4) The part is ejected, and the process repeats from step 2.
Whilst the part cost is low, injection moulding has high set up costs, mostly from the cost to make the tools (using CNC) Mould tools range from a few hundred GBP to over 100,000 GBP depending on complexity.
The materials used for the tools varies depending on how many parts are to be made and the accuracy required. All thermoplastics (polymer’s which becomes soft when heated and harden when cooled) can be moulded. Some silicones and thermoset resins are also possible to mould.
The most common thermoplastics used are:
• Polypropylene (PP)
• Acrylonitrile butadiene styrene (ABS)
• Polyethylene (PE)
• Polystyrene (PS)
ADVANTAGES AND DISADVANTAGES OF INJECTION MOULDING
• Suitable for very high volumes >500 pieces
• Extremely quick to make parts (once running)
• A large range of materials available with diverse properties
• Very low part cost in large volumes.
• Excellent repeatability
• High tolerance
• Excellent visual appearance
• Can create very complex geometry
• Little or no extra finish required
• Low scrap rates
• High set up costs for tooling
• Long lead time relative to other processes.
• Expensive to modify design
Shown here are a number of the terms that will be covered through-out this guide.
Nominal Wall Section: The general thickness of the main part walls
Parting line: Where parts of the tool meet
Injection point: Where plastic enters the mould cavity
Rib: Used to give a part stiffness
Fillet: Rounds a corner to help plastic flow
Gusset: Stiffens a part, usually across 90 degrees between vertical and horizontal
A part is created by two or more tools moving together to create a closed volume, into which plastic is injected under pressure.
In a 2 part tool the cavity (A) creates the quality outer surfaces and the core (B) creates inner details.
There are often extra “cores” sliding into the cavity to allow more complex parts.
Raw plastic is fed into the hopper as pellets. Within the hopper these are mixed with additives such as pigment, and fillers such as glass fibres to adjust the properties of the final part The material is then fed into the barrel, where a reciprocating screw rotates, moving the pellets towards the mould and compressing them.
The friction created in this process combined with heater units wrapped around the end of the barrel raises the temperature and the pellets are melted Once there is enough melted plastic in front of the screw, the ram moves forward squeezing material through a nozzle into the mould cavity where it cools and hardens.
Throughout the injection process the tools are clamped tightly together. Once the plastic has cooled sufficiently to maintain its shape the tool opens, usually by the core and part moving backwards away from the cavity.
Ejector pins are then pushed through the core against the part, releasing it to drop free from the tool.
This process does result in a few witness marks on the part:
Parting lines: where the two halves of the mould meet.
Ejector marks: where the pins meet the part. Normally these are hidden on the rear.
The Runner System
Melted plastic enters the part through a network of channels in the tool called the ‘runner system’
There are usually 3 parts to this:
The sprue: The primary channel where material flows into the tool.
Runners: Smaller channels which guide the plastic to the gates.
Gates: The entry point to the part.
Gates are the point where the melted plastic enters the cavity. The position and geometry of a gate control the flow into the part.
The diagrams to the right show some of the common approaches:
1. Edge gates are the most common, injecting at the part line where the two halves of the mould meet. The runner system is removed manually after ejection which leaves a small witness mark.
2. Direct gates connect from the spur to the top of the part to reduce material wastage on runner systems. This is ideal for very large parts but does leave a visible mark on the part.
3. Tunnel/Sub gates inject below the parting line. There is no need for manual removal of runners as they are snapped off on ejection. This is ideal for very large volumes.
4. Pin gates inject material from the inside of the part in the Core or “B tool”, away from the visual surfaces making them favoured for appearance.
As with all mass manufacturing processes there are a few planning steps before committing to tool.
Is moulding the right process at this stage?
High numbers of parts should be intended, and tooling cost factored in.
Ensure that everything that is needed from the design is specified in detail before starting tooling. Changes to steel tooling is costly and time consuming.
Specify Material, and Properties
Every polymer has different flow rates and shrinkage, it always helps to know the planned material before tooling so the injection point can be designed appropriately.
Time to part with injection moulding is long. Times are quoted to samples, and there are often other time constraints, such as finishing, shipping, production sampling, assuming the design is complete. Ensure
Best practice design guides aim to help create complex shapes while:
• Allowing plastic to flow easily and uniformly around the part.
• Allowing plastic to flow easily and uniformly around the part.
• Allowing the plastic to cool quickly and evenly, resulting in a stable and accurate part.
These general tips will improve part quality, mould ability and cycle time based on known implementation and characteristics of the injection moulding process.
Note: Design guides are broken often and still result in successful moulded parts.
To do achieve this careful consideration and understanding of many parameters
is needed including;
• The part’s mechanical requirements,
• Mould flow,
• Temperature control within the tool,
• Polymer selection
• Filler requirements
• Adjustment of part geometry.
Uniform Wall thickness
Keep walls constant thickness, and avoid thick sections
If different thickness are required ensure the transition is smooth by blending or chamfering.
Transition over 3 x thickness difference.
Even wall sections allow the material to flow at a constant rate around the tool. Variable walls can lead to the part warping as the material cools. See table for recommended wall thickness
Allow as much draft as possible.
Recommended draft is >2 °
Increase draft 1° per 25mm height on tall features.
If the part is to be textured add 1-2°.
At the end of the moulding cycle, the cooling part needs to be ejected from the tool. Without draft, as the part shrinks it grips the vertical walls requiring greater force to push it off. This can result in a number of defects including ejector punch marks or drag marks where material rubs against the tool.
For this reason taper is applied at an angle to the movement direction of the tool. With sufficient draft on all surfaces the part quality will improve and the cycle
time will reduce.
Draft also helps with the CNC milling process to create the mould tools, allowing deeper features.
For interior edges apply a radius >0.5x Wall thickness.
Exterior edges should have a radius of Interior radius + Wall thickness.
As with wall sections, ensuring that the plastic can flow easily round the part is essential to avoid warping.
Sharp corners restrict the flow as they temporarily widen the flow path, and change direction quickly. This results in inherent stress within the part.
“Shell” Thick Areas
Avoid thick areas by evenly thinning outer walls creating a shell which follows the maximum wall thickness guidelines shown earlier in this document. Ribs can be added if more structure is needed.
Thick areas of a part will cool inconsistently, leading in turn to contraction at different rates across the part. This results in voids, warp, sink and stress points which lower the quality and performance of the part.
Use Ribs for Strength
Rib thickness should be 40 – 60 % of the primary wall thickness.
The height of a rib should be < 3x the thickness of the primary wall.
Ribs should be drafted >0.5 °.
There should be a radius of ¼ the primary wall thickness.
Ribs should be at least 2 x nominal thickness or ideally their height apart.
The requirement for keeping wall sections thin require consideration to introduce strength into a part. Ribs can be used to achieve strength and volume where needed.
It is important to consider the plastic flow and resultant material thickness when placing a rib. If the area at the base of the rib becomes too thick the plastic will cool slower and cause a visible sink mark.
Shorter ribs minimise ejection problems and also make it easier to fill the part.
Multiple ribs should be place no closer than their height from each other.
Use a bold San Serif font minimum 20 point. (5mm height).
Use raised (Embossed) text rather than engraved.
Raise the text by 0.3 – 0.5mm.
Ensure the text is perpendicular to line of draw.
The Tools will be created by CNC so for cost finish and accuracy it is preferred to de-boss the lettering into the tool which results in an embossed plastic part.
Boss diameter = 2.0 to 2.4 x Hole (Screw/insert) diameter
Bottom fillet = 1/4 Nominal wall section
Rib height= 1/2 Wall height
As with ribs, screw bosses require careful design to avoid thick sections at the base.
Ribs and supporting gussets are often necessary to give sufficient strength, whilst keeping the volume of material down.
Avoid merging bosses with side walls, as the sections become thick leading to sink marks.
If the position is needed in some cases features can be created as shown to even the wall sections.
Commonly parts are held together with screws.
Thread cutting screws for plastic are available, however inserts offer longer part life where disassembly or servicing is required.
There are 3 common types of insert for thermoplastics:
The insert is vibrated using an ultrasonic transducer melting the plastic, allowing it to be pressed into place. This allows short cycle times and low residual stress.
The insert is heated until it melts the plastic, and then pushed into place. This is a low cost solution, less suitable for volume manufacture.
Inserts are placed into the injection mould tool, usually by hand unless with large volumes. The plastic completely surrounds the insert on injection, bonding it securely in place.
Other types include, screw fit, expanding push fit,
Undercuts - Sliding Cores
There is often the need to create features which require an under cut, such as snap fits or holes perpendicular to tool movement. A common way to make undercuts is to use sliding cores.
Sliding cores are moving tool parts which move through or between the main tools temporarily creating a volume for the plastic to flow around, and then removed as the tools open.
The sliding cores need to be drafted in line of movement:
1 degree or more will be needed where the core meets plastic.
3-5 degrees is recommended where two parts of the tool slide together.
The use of sliding cores need to be carefully considered. Each one will add cost, and will introduce a part line with potential for flashing.
Discussion will be needed with the tool maker to ensure enough space is available for the core to slide, and enough material in the tool around the sliding core for reliability.
Avoiding an undercut all together is often the best option. This can sometimes be done by changing the way the two parts of the mould meet.
Shut-offs offer low tooling cost approaches to creating features which would otherwise be achieved by sliding cores.
A shut off is where two parts of the mould mate, preventing plastic from passing. It is used to describe where the moulds form a slot or a hole by this method, or
when a slide shuts against the core or cavity.
As well as the plastic guidelines the tool geometry needs to be considered. As the 2 parts move against each other, they will wear, shortening the tool life. Tool strength is also a consideration, and often features need to be adapted to keep enough tool material.
For this reason 3-5 ° draft is required between the mating tools.
Snap fits are often used to hold plastic parts together because they are quicker and lower cost to implement than screws.
Snaps inherently require a overhanging feature which is often undercut, however to keep costs low it is often possible to create snaps in line of draw using the partline
There are many ways to create a snap fit. The snap design will depend on a number of variables specific to your project including space available:
• Material choice
• Snap force
• Retention force
• Opening requirement
Lifters can also be used to create undercuts.
A lifter moves with the ejector pins but at an angle, so as the pins push the part off, the lifter moves outwards and away from the feature.
This can be quite cost effective as it is a relatively simple and automatic process.
There are however some constraints on geometry to allow for the moving tool parts.
Small undercuts can be designed to be safely ejected from a straight pull mould without the need for a side action. This gives obvious cost savings.
The basic principle is to allow the plastic to deform as it is ejected. The plastic choice is important. e.g. unfilled polyethylene is flexible, glass filled nylon would be too stiff. The feature needs freedom to deform – e.g. once the cavity has moved away. The geometry should be designed to allow movement and flex.
In the example (right) after the cavity is moved away the part is free to easily stretch “bumping over” the undercut feature.
Bottle cap threads and small snap features are often created using this approach.