Drillings are one of the most common machined features, with many applications including threaded holes, oil galleries, cooling channels, tool access holes plus many more. They look simple, but there is a surprising amount to think about when designing a drilled feature. Follow our drilling best practices to get the most out of your design, and allow us to produce the highest quality parts.
Features of a drill tool
There are a number of basic principles we should always follow when designing a drilled feature:
Choose standard diameter drills
British Standard BS328 defines standard size metric drills. The minimum diameter is 0.2mm and maximum diameter is 25.0mm. BS328 defines the following available sizes:
Available drill sizes in BS328
We would always recommend designing drilled holes to this standard where possible. Any deviation to this standard would require order of a special drill bit and could be expensive and add delays to your project. Drill bits in BS328 are in stock and readily available to us, but any non-standard sizes need to be ordered specifically for your project. Lead times on these tools can cause delays to a project, so we recommend using standard drill sizes.
Understand maximum flute length
Maximum flute length of a drill bit for a given diameter determines the longest drilled hole that can be designed. The most common type of drill bit is a ‘jobber length drill’, which has a flute length between 10 -17 times the nominal diameter. Other types include ‘Screw machine length’, which offer a shorter flute length option, and ‘aircraft length drills’ which offer a longer flute length option.
As screw machine length and aircraft length drills are not normally kept in stock, you can avoid additional costs and lead time associated with ordering these specialty tools if you can limit designs to be machinable with jobber length bits.
Consider drill point in drill length
The selected drill point angle affects the drill point depth; smaller drill point angle means a larger drill point depth. The angle required will be determined by the hardness of the material you are machining into. Generally softer materials will have a steeper angle (e.g. Plastics = 90°) and shallower drill point angles are used for harder materials (e.g. Aluminium 118°). 118° drill point angle is common and is suitable for machining many different metals including aluminium, brass, cast iron, mild steel & stainless steel.
The drill point should be considered in any drilled feature design
The drill point length will need to be considered when including drilled features. Defining a drilling using a ‘Hole Wizard’ in CAD software usually requires the drill length as input, and the drill point length is calculated automatically, which means risk of breakthroughs can go unnoticed. In the example below, the drill length is 135mm in a 140mm workpiece, theoretically leaving 5mm wall thickness. However taking into account the drill point leaves only 1.1mm of wall thickness, and has a high risk of breaking through causing loss of function of the part.
Not taking the drill point into account could cause the drill to break through
Minimise use of chamfers
We often design drilled features with chamfers on the outer edge of the drilled hole. This is either to act as a lead-in for an object assembled into the drilled hole, or to break the edge and minimise the risk of burrs. Standard drill bits cannot produce chamfers, so they must be machined as a separate operation. This is easily achievable, but does require an additional tool to create the chamfer.
Additional tools and processes in CNC machining are expensive and chamfers should be avoided if possible. A chamfered drilled hole could take more than twice as long to machine as a drilled hole without a chamfer. This also means it can cost more than twice as much to machine.
A drilled hole with a chamfered edge takes more than twice as long as the same hole without a chamfer
Don’t thread the full hole length
There are two methods of creating a threaded hole: thread tapping and thread milling. In both methods, a plain hole is drilled to a given diameter and length. For thread tapping, a ‘tap’ tool of the same diameter as the thread you require is plunged and rotated into the drilled hole. A tool clearance called “thread runout” at the bottom of the hole is required, meaning the drilled hole is always a few millimetres longer than the threads. This process is very fast and simple; we always recommend designing a threaded hole to suit thread tapping.
Thread milling uses a smaller diameter tool than the hole required. The tool moves in a helical motion to create the threads. The benefit is that a much lower thread runout clearance is required. The drilled hole only needs to be 1-2mm longer than the thread. However this process is very slow and should be avoided wherever possible.
Left: thread rolling is very fast and simple operation. Right: thread milling is slow and not recommended
Avoid high-aspect ratio drilling
‘Gun drills’ for machining of high aspect ratio holes
In some cases, the design requires very high aspect ratio drilled features. An example of this is the oil gallery which runs the length of a V8 engine block. The feature can be 500mm long and is only Ø6mm. Any drilled feature with a length more than 10 times the diameter is considered ‘high aspect ratio’.
To solve this CNC machining problem, we can use a ‘gun drill’. These were originally developed for boring of gun barrels, which of course require a very long, narrow and straight hole. These drill bits are unique in that they have a single cutting edge and cooling channels that run the length of the drill bit. Drill aspect ratios can be 40x diameter on a standard CNC machine, or 100x diameter on a bespoke gun drilling CNC machine. Gun drilling requires bespoke CNC drill tools which are often not in stock.
We recommend only designing high aspect ratio drilled features in specialist applications, where no other design solution is possible, to avoid the use of bespoke tooling.
High aspect ratio gun-drill required to machine oil gallery in V8 engine block
Always drill into a perpendicular surface
4-axis and 5-axis machining give you the opportunity to design and manufacture drillings at angles to standard XYZ cartesian axes. This can be especially useful for fluid transfer galleries, including water cooling channels and hydraulic actuation oil channels. One design option could be to design a separate pipe to transfer the fluid, another is to drill angled features into the main part.
Drilling at an angle can cause problems as the drill tip is not the first point to contact the workpiece. The drill can slip, causing a widened hole at the top of the drilling e.g. A Ø13mm becomes Ø14.5mm and tapers down to 13mm. This will likely cause problems with the function of your part. You might also see a poor positional accuracy and poor surface finish of the hole.
Drilling at an angle to a workpiece
Our recommended best practice is to design a ‘boss’ feature around the drilling to give the drill tip a perpendicular surface to cut into. This removes the risk of the tool slipping, and ensures the drilled feature is of the highest quality and meets your specifications. A boss design is best for drilling of moulded parts such as castings, forgings and plastic mouldings, where the boss can be created as part of the moulding process.
A ‘boss’ gives a perpendicular surface for the drill tip to start cutting
For drilling into a forged billet, we recommend designing a ‘spot face’ feature. This is a milled pocket machined prior to the drilling to give the drill tip a flat perpendicular surface to drill into. For low volume machining, the spot face can be created with a separate milling tool, which of course requires a tool change and use of a second tool. For high volume projects, it might be economically viable to create a combined drilling and spot face tool to machine both features in one go, but be aware that this tool can then only machine a single drill length.
Spot face milling is an alternative design to a boss for billet parts
Drillings can be interconnected to create complex passageways for fluid transfer. Our recommended best practice is to maintain an angle between drillings >45°. Connected drillings with a low angle between them causes a sharp piece of material which cannot be easily de-burred. Burrs in these areas could come loose during operation and cause damage to the part. For example if the drillings are part of an oil system with a pump, the pump could become damaged by the loose burrs. A larger angle between drillings reduces the risk of burrs during drilling.
Interconnected drillings can be used to form complex passageways
We also recommend a best practice of fully overlapping drillings, so the full shank diameter of both drilled features interconnect. This, again, minimises the risk of burrs forming which would be very difficult to remove.
Follow these drilling best practices for the highest quality machined parts at CloudNC. Get in touch with our team to discuss your CNC machining project, and read more DFM tips on our blog.