From rLab Wiki
Revision as of 22:09, 7 April 2021 by Stever (talk | contribs) (Dealing with any problems, shutdown and clean-up: change to recovery proceedure)

Some of the tools at the Hackspace are potentially hazardous to use, for these tools members are required to have an induction before they can use them. Inductions provide the most basic information on how to safely and effectively use the simpler functions of the tools, we appreciate that some members may have professional experience on some of these tools and in this case please tell your induction provider and the induction may be very reduced and just cover any risks or procedures specific to rLab. Some tools have multiple levels of induction in order to cover more advanced uses of that tool without making the basic induction take too long, higher induction levels will introduce some of the more advanced features of the tools but as with all inductions are only intended to provide basic information on the capabilities of the tools and how to use them safely. Some members of rLab may be willing to offer more detailed tuition beyond basic induction level or offer guided practice sessions in exchange for beer money or assistance on their own projects.

For all tools you are only required to take level-1 induction before use, after that you may perform any task that you feel confident you can do safely, higher levels of induction may be useful to you in performing more advanced operations but are not required before doing tasks covered in them so long as you're confident of your ability to handle those tasks without risk to yourself, others, or the tool.

PLEASE NOTE : All induction providers are volunteers who are providing inductions to the best of their ability but are NOT qualified instructors. Inductions are provided on a best-effort basis but you and you alone are responsible for your safety while using the tools and for satisfying yourself that you can operate the tools safely. There are professional training courses available from various providers in Reading and the surrounding area if you feel they are appropriate for the level of work you intend to undertake. Reading these notes is NOT a substitute for an in-person induction.

Note for wiki editors : Please do not edit induction pages unless you are one of of the people that gives that induction

Induction Process

Induction for this tool is still being developed, at the moment the plan is to divide induction into 2 sessions. The first session will be classroom based and will cover how to design objects so that the Boxford can make them, and how to set up the CAM module in Fusion360 to generate code that the Boxford can run. The second session will be 1-on-1 and will be based downstairs and will cover actually operating the Boxford. There is going to be a charge for induction as the lab does not provide milling tools as a routine consumable. This is because it's easy for a clumsy operator to get through £200 of broken tools in an afternoon and that wouldn't be fair on other members. The cost is currently estimated to be around £30-£60 and will include some metal stock and a basic set of tools sufficient for most standard milling operations.


This induction will take a user through the process of defining an example tool path, checking it looks OK, and the safe operation of the Boxford to run the program. This induction will not cover designing an object, or the more advanced tool path options that Fusion360 can generate. It is considered a starting point for the user to be able to go learn more about the topic without putting the Boxford or other rLab users at risk.


Before you can take this induction you have to meet certain requirements. This is unusual for inductions at rLab as most do not have any prerequisites and are open to anyone. We've decided on this unusual course as the Boxford is considerably more difficult to use than most other tools in the space and requires a considerably greater knowledge of the process in order to get started. It's not something you can just walk up to and start work. At the moment the only workflow we have for the Boxford requires the use of AutoDesk Fusion360; there is a plan to add FreeCAD support in future but that may take quite some time. We will not be offering general tuition in the use of Fusion360 as part of this induction - we'll only be covering the detail of the manufacturing module but if you would like general help with Fusion then a number of our members are experts with it and are usually willing to teach. It is also going to be a requirement that you've had 3D printer induction and successfully designed something from scratch and printed it out. This is because quite a few of the skills and ways of thinking about manufacturing do carry across between 3D processes so making sure you are able to think and work in this way will save a lot of time later. You will also benefit significantly from having worked on a manual machine tool previously as in a lathe or mill.

Before you start

If you'd like to take the induction for the Boxford then the requirements before we start are :

  • Basic familiarity with Fusion360 and an AutoDesk account. You don't need to be an expert user but you need to be able to do basic designs and navigate around the Fusion interface without help.
  • Have designed something in Fusion360 from scratch, without importing any geometry or using the Mesh work-space as both of these can create issues for CNC operations.
  • Have a laptop capable of running Fusion360
  • Been inducted on the rLab 3D printer and successfully used it to print a design of your own making.
  • Be able to use the compressor
  • Pay an induction fee of £30-£60(tbd) which covers all costs of the induction as well as providing the material for your test piece and a basic set of tools.

First session

Principals of Milling

Slide deck for this presentation is File:Boxford induction.odp

(Open on slide-1)

A user aiming to use the Boxford needs to learn the following:

(Slide 2)

This induction is a work in progress. Questions or clarifications are welcomed so feel free to speak up if you have something to ask or add! The Boxford is also still being worked on so details are likely to change in the future as upgrades are made. Please check on the induction wiki page from time to time to see what's changed. If you've got ideas for upgrades for the Boxford then please let Steve or Toby know. We do already have a number of upgrades in mind but machine tools are expensive and so they won't happen unless the Boxford becomes popular and there's demand for improvement.

Topic Contents Reasons
Principles of Machining

(Slide 3)

  1. Milling machines like the Boxford work by pressing a rotating cutter into the block of material
  2. It shaves a thin strip off the material as it turns, forming a "chip"
  3. The cutter is advanced into the material steadily so that each tooth on the cutter removes a chip in turn
  4. The cutter is supposed to remove material by a "shaving" action, it's not scraping or shearing action
  5. Ideally things are arranged so that each tooth is removing a chip of the same size and thickness because that makes for consistent cutting forces but it's not always possible
  6. The cutter might have anything from one to several dozen teeth depending on size and shape, but 3 or 4 is most common.
  7. The shape of the cutter is designed so that the chips move away from the cutter and can be cleared out of the cut
  8. This method of removing material does impose some limits on the shape and type of cut that can be made which we'll get into later.
Basic grounding in how milling machines work
What materials can be used in the Boxford

(Slide 4)

YES NO Maybe...
Most plastics Wood Stainless Steel (slowly)
Aluminium GRP Titanium
Brass Carbon Fibre Tool Steels (Annealed)
Steel Hardened Steels
Bronze Chromed Steels

If you're not sure if your material can be machined, ask Steve or one of the other more experienced machinists

Some materials don't cut well or may cause damage to the machine
Cutter types

(Slide 5)

Cutters are available in thousands of shapes, the more important of which we'll cover in a minute but they come in 4 main types.

  1. HSS - High Speed Steel. These cutters are made of a special steel called high-speed steel which is mostly iron but has added Tungsten and/or Molybdenum to increase its strength and allow it to resist the heat that cutting metal generates. HSS is the weakest type of cutter that we normally use but it's also the cheapest and for standard metals it's generally fine.
  2. Cobalt Steel - These cutters are made of iron with a large amount of added cobalt and they're harder and stronger than HSS. Cobalt steel is more often used for drills than for milling cutters but we're covering it here because the Boxford can be used for precision drilling as well as milling. Cobalt tools are 3 or 4 times the price of HSS but also last 5 times longer. They're suitable for use with all the standard metals and also for use with some of the more difficult materials like stainless steel or titanium.
  3. Solid Carbide and Brazed Carbide - These cutters have edges (or the whole tool in the case of solid carbide) made from Tungsten Carbide. They are dramatically harder than the 2 steel types and can be used in all machinable metals. They're more expensive and more brittle than HSS cutters so they have to be treated carfully to avoid chipping or snapping. That said, if they're used properly they have a life span 10-20 times greater than HSS and can cut much harder materials. One downside of Carbide tooling is that they require very high cutting speeds to get good results and owing to limitations of the Boxford that can be a problem with smaller carbide tools.
  4. Carbide Insert Tools - Large solid carbide tools are VERY expensive; carbide insert tools are a way to get the advantages of carbide without the expense on larger tools. They have small Tungsten Carbide inserts which are held into the cutter to act as the cutting faces and can be easily replaced when they wear out. This means that they have a cutting edge nearly as good solid Carbide, but the inserts are cheap to replace and the cutter body lasts almost forever if looked after. Carbide insert tools are typically only available in sizes over 20mm and they have all the same advantages and problems as solid carbide when in use.

All of these cutter types can come with a wide variety of coatings applied to the surface which change their properties in various ways such as reducing friction, increasing wear resistance or changing what materials they can be used with. Covering all of the variations on coatings is WAY outside the scope of this induction but if you want more information you'll find hundred of pages online about them, or manufacturers usually offer guidance about what tool type and coating to use for what job.

Selection of suitable tools is vital for getting good result

Cutter shapes

(Slides 6 - 14)

Cutters come in a huge range of designs (slide 6) that are all meant for different purposes. We're not going to cover very many of them today because we'd be here for hours but I am going to go over a few of the main types

Tool Slide Picture What's it for?
End Mill 7 Example End mills are the workhorse tools for milling. They're good at removing materials from the sides and tops of parts and larger size ones can remove a lot of material very fast. Their main weakness is that owing to the small dead spot right in the centre of the tool they don't work well if plunged vertically down into a workpiece, but there are ways around that with pre-drilling or adaptive toolpaths that we'll cover later.
Slot Drill 8 Example Slot drills are in many ways similar to end mills and can do many of the same jobs, however if you look closely at the face of a slot-drill you'll see that the centre point of the flutes is off-set from the centre of the tool. This makes it possible to plunge vertically down into a job and still cut properly. The downside is that the unevenness of the end makes it less effective at making smooth faces and more prone to vibration.
Ball-Nose End Mill 9 Example The rounded end on a Ball-nose end mill is used in situations where you want to produce a controlled internal radius on a cut. They're also used for more difficult situations where you're having to work at long tool extensions or the ability to clear chips from the cut is restricted, because without the small, sharp points of the previous two cutters they can be made much stronger. They can be used where you're trying to contour a 3D curved surface as using a ball-nose cutter doesn't leave sharp steps behind like the other two types.
Face cutter 10 Example Face cutters are milling tools with a very large width-to-height ratio that are used for rapidly machining a flat horizontal surface, they generally have little or no plunging ability but they can clear a large area rapidly. They're mostly used for preparing a rough piece of stock before other milling operations but when used this way you have to be careful as you're probably milling away your reference face. Why this matters will become clear as we go through the rest of the induction.
Chamfer cutter 11 Example Chamfer cutters are used to produce chamfers that prevent your part from having sharp corners. They can be had in a variety of point angles (and so chamfer angles) with the normal range being 45-135 degrees and 60 or 90 degrees the most common. There are many types of specific chamfer milling cutter, but in softer materials where you don't want to buy a special cutter, countersinks or center drills will also work.
Spot/Centre Drills 12 Example Centre drills and spot drills do basically the same job just using slightly different shapes. When you want to use a regular drill in a milling machine you have to deal with the drill trying to wander around rather than bite into the material cleanly. This is because all drills have a small dead-zone in the centre where there's little or no cutting action which tends to push the drill around. Spot and Centre drills get around this by having a very small dead zone and being very short and rigid. They're not good for drilling deep holes though so you normally use them to make a small indentation in the metal and then switch to a regular drill to make the main hole.
Jobber Drills 13 Example Jobber drills are the "standard" drills that you're used to using for everything. They don't have great life, and usually require a centre-drill to be used first when using them for milling but they are cheap and we have loads of them. Jobber drills are usually made of HSS but if you're doing a job with a lot of holes, or you're working in harder materials you can also get Cobalt or Carbide versions with dramatically longer life.
Stub Drills 14 Example Stub drills have the same geometry as jobber drills, they're just much shorter for their diameter. This allows them to be used in harder materials without deflection, or used without spot/centre drilling on regular materials.
Types of cutter dictate what sort of jobs can be run
Feeds & Speeds

(Slide 15)

Two of the most important parameters for using any cutting tool are called the speed and the feed.


Speed is how fast the cutting edge of the tool is moving through the work, usually measured in meters per minute. The speed is determined by the radius of the cutter, and the rotational rate (r.p.m.) - the larger the tool and the higher the r.p.m. the faster the peripheral speed of the tool through the material. This matters because every combination of tool material, tool coating and workpiece material has a specific speed at which it works best. At that speed you'll get the fastest, cleanest cut that's possible with that tool and material which will get your work done in the shortest time and with the nicest surface finish. It's relatively easy to calculate what speed you'll get from any combination of tool radius and r.p.m. but since Fusion360 will do it all for us I'm not going to get into that.

If your speed is too slow then the tool tends to bite into the work too hard. Instead of nicely shaving a layer off the work it starts pulling chunks off. This is extremely damaging to the cutter, dramatically shortening its life or even breaking it entirely, and results in a terrible surface finish. Too fast will result in heat build-up in the tool and the work and will start burning up the tool. At these higher temperatures there's a tendency for the material to start sticking to the tool which means it can no-longer cut efficiently, making more heat, which causes more sticking and so on. The usual warning sign for this is that the tool starts to push a mound of material ahead of it but in harder materials you'll get no warning at all and the tool will be destroyed inside the cut where you can't see it happening.

The Boxford will also impose some limits on the speeds you can run at. It has a maximum spindle speed of 3000 r.p.m. which is quite slow for a modern milling machine - most CNC machines these days come with spindles that can do at least 6000 r.p.m. and speeds as high as 30,000 r.p.m. aren't unheard-of in higher end machines. This can become an issue for smaller tools as they require a high r.p.m. to keep the surface speed up. At the lower end the speeds the Boxford can do are limited by torque. Typically the reason for using a low r.p.m. is that you're using a larger cutter and larger cutters normally require more torque to operate properly. Unfortunately the Boxford's available torque decreases with speed, making it easy to stall the spindle at low speeds. Although the controller will allow speeds as low as 100 r.p.m. you'll generally find there are issues with going much slower than 300 r.p.m. and preferably 500 r.p.m.

Deciding what speed you should use generally comes down to searching online for recommendations, then taking an average of the half-dozen different answers you'll get, then trying to guess an adjustment based on how good you think the Boxford is as a milling machine. For a general guide though, harder tools will result in higher speeds, so HSS will be slowest, then cobalt a bit faster, then carbide the fastest at around 3 times as a fast as HSS. Harder workpieces will normally result in slower speeds, so aluminium would need a very high speed, brass less, steel still less, and stainless or tool steels the slowest of all. Plastics are odd and usually require slower speeds than you'd expect based on hardness. They usually cut best with HSS tools instead of carbide.

If you're only making one of a part then you'll probably just go with your first guess for speed, but if you're making a lot of them then it would common to make one part at your first guess speeds, one at 10% higher speed, one at 10% lower speed. Whichever one has the best results becomes your new guess and you repeat the adjustment process until you get the best result you can.


Feed is how fast the cutter is moving into the material. It's normally measured in millimetres per minute. Faster feeds obviously result in higher material removal rates, but also higher loads on the machine and cutter. Slow feeds are more gentle on the machine but there is a lower limit to how slow the feed can be - go too slow and the tool stops cutting effectively and just starts rubbing the material away which results in a lot of heat and terrible performance.

In order to work out what you feed should be you start from knowing the r.p.m. of the cutter as we worked out just now, and from a parameter called feed-per-tooth which is measured in fractions of a millimetre. FPT is literally how far the tool moves into the work per cutting surface that goes past the work. You can also think of it as the thickness of the thickest part of the chip that's being removed. Working out what FPT you should be using is also a matter of online research and guessing. It depends on the tool material and work material, but unlike speed it also depends a bit on the diameter of the tool. This is because the FPT has a large impact on the force that's being applied to the tool and since smaller tools can withstand less force, it's common to use a lower FPT for them.

So in order to work out your feed you need to know how many teeth are moving past a given point in a minute, and how much feed per tooth you're using, the overall feed rate is then going to be :

Spindle speed (r.p.m.) x teeth on the cutter x feed per tooth (mm) = feed rate in mm/min

Note that this means the number of teeth on the cutter has a dramatic effect on the feed rate, a 12-tooth facing cutter will be advanced into the material a LOT faster than a 2 flute slot drill.

When deciding a feed rate it's also necessary to consider the "chip loading", which is how many and how large the chips being formed are. You need to be able to clear the chips from the cut, and how easy it is to do that will depend on the geometry of the cut. If you're taking a shallow cut skimming the surface off a block of material then getting the chips out of the cut is very easy so you can afford to have really quite high chip loads. On the other hand if you're milling out a deep, narrow slot (something you should try to avoid if possible) then getting the chips out of that cut will be dramatically harder and that's likely to impact the maximum chip loading you can afford to have.

Other factors you'll need to consider include the load on the spindle. For example if you're running at quite low r.p.m. where the spindle has limited torque available then if you try taking a large feed per tooth you run the risk of the cutting force exceeding the available torque and stalling the spindle motor. At the higher end of the speed range a cut with a high feed per tooth may exceed the total motor power available, which would result in the spindle slowing down and since the feed motors wouldn't slow down the tool forces would quickly rise enough to snap the tool. It's also necessary to consider the maximum travel speed of the machine. For most operations we recommend a maximum of 600mm/minute for travel moves and 300mm/min for cutting moves although this may change in future if the Boxford receives some of the upgrades we have planned.

You will come across the terms climb milling and conventional milling, climb milling is the preferred method to use when using CNC, Climb milling is when the direction of cut and rotation of the cutter combine to try to “suck” the mill up over (hence it’s called “climb” milling) or away from the work. It produces the best surface finish. you may be required to specify this in Fusion360

Because of the way Fusion360 works, in most cases you can set a surface speed and a feed per tooth when defining a tool and it will attempt to set suitable spindle speed and feed rate for you. The values it works out are usually quite aggressive as they're intended for larger, higher quality machines than the Boxford so it's always necessary to manually review them and often adjust them to stay within what's safe for our machine.

Feeds & Speeds are a fundamental concept. We have to cover it even if it is quite long and dull
Designing for CNC milling

(slide 16)

When you're designing something it's important to consider how it's going to be manufactured. You're familiar with 3D printing and that imposes limits on overhang angles and unsupported bridges - similarly with CNC milling you have to remember that every surface needs to be reached by a rotating tool. You can't have features on your part where the cutter cannot reach into, or where it's blocked by material above it, and having a part that has to be rotated in order to reach all areas dramatically increases the complexity of the machining process.

Important constraints to remember :

  1. The maximum distances the tool can move are 240mm in the X-axis and 130mm in the Y-axis. In practice it's better to keep well under that until the limit switches are properly installed as going anywhere near those maximum sizes will risk harm to the machine. The maximum travel in the Z-axis is about 130mm but here there are additional constraints to worry about. The length of your longest tool will limit the thickness of your part as it has to be able to clear the features of your part and not collide with them. This does mean that you can get more Z-height by using short-shank tools at the cost of having to make more passes
  2. Overhangs are a problem. The conventional tools I've shown you here have to approach from above and have straight or inwardly tapering shapes which means that you cannot machine any overhangs without first rotating the work, which is tricky to do correctly and we won't be covering here. You can get outward tapering tools, usually called dovetail cutters although some have other names, and they will allow a limited amount of overhang to be machined so long as there are no other features too close to block the approach of the cutter.
  3. Cutting deep slots can be difficult as it's hard for the chips to get out. This doesn't mean you can't do them at all, but if there's any way you can avoid it then do so! Typical avoidance strategies are :
    1. Completely change the part design so it's not needed at all
    2. Provide openings into the slot that can be machined first to allow chips to escape
    3. Make slots wider so that you can cut them in several passes rather than all at once
    4. Advanced toolpath types that provide clearance.
    5. Using cutters that make smaller and easier-cleared chips
  4. Deep holes can be troublesome. The important number to consider is the depth to diameter ratio of the hole you want to make. If it's less than 3 there's no problem, that's easy; if it's 3 to 5 that takes a little more care but should usually be OK; 5 to 10 is difficult, drills used in that way are very prone to torsional vibration and the risk of breakage is high; over 10 are not really possible with standard drilling techniques - Talk to Steve if you have an absolutely unavoidable need to do this. You can sometimes get around deep-drilling problems by :
    1. Increasing the hole diameter. This improves the depth:diameter ratio
    2. Milling away material around the top of the hole before you drill it to make it shorter
    3. Counterboring : Making the top of the hole a larger diameter than the rest and forming it in 2 operations
  5. Curved surfaces will often require hand finishing. Some types of curved surfaces are fine, for example if you want to radius an internal corner by a standard amount then you can just use a cutter with that radius formed into it. The issue comes where you want a larger or complex curved surface, you CAN have this, but the CNC system will produce it by making a series of small stepped cuts using whatever cutter you have available. This will leave you with a trade-off - if you use a small cutter and make lots of tiny steps then you can get quite a good finish and it won't need much hand work at all but it will take a very long time to machine. Alternatively if you use a coarse cutter and large steps it will be fast to machine but require extensive hand finishing. If your curved surface is somewhere inside the part, make sure you're going to be able to get in there with tools to perform the hand finishing!
You have to design according to the process you will be using.

Generating CNC Programs

OK that's the basic introduction to milling so now it's time to get on to actually writing a CNC program. You should have all downloaded the example object we're going to use here File:Bandsaw Table Insert.f3d So please fire up Fusion360, create a new project called "Boxford Induction" and load the part into it. Also please bear in mind that I'm not an expert on Fusion so if you know of better ways to do things, please let me know so they can be added into this induction

Getting Started

Topic Content Reason
Getting started

Start by taking a look at the design, think about what tools will be needed to produce each feature of the part and what angles they can reasonably approach from. In the case of this part it's going to be possible for all the operations to be conducted by coming in from the sides and top, so we'll only need a single "setup" for the job.

Switch to the "Manufacture" workspace using the selection top-left of the screen and we'll start planning how to make the part.

Top left of the work area you'll now see the structure tree for manufacturing which is mostly empty. At this point the only things to check are that your units are set to millimetres and the correct model is loaded. Because some machine tools use inches, it's possible to design something in one unit system and manufacture it in another but we'll be sticking to millimetres for everything.

Along the very top of the screen are "Milling", "Turning", "Addative", "Probing", "Fabrication", "Utilities" Make sure that "Milling" is selected so that you'll have the correct set of operations available. If we get other CNC machines in future then those other tabs might be useful but for now everything we need is under milling.

Remember Fusions360's spot-help system, hovering over any of these options will give you a clue as to what that button does.

First steps getting into the manufacturing system
Setup Sheets

Everything starts with a setup so please go to Setup under the milling tab and select "New Setup", Setups define

  • What you're making (What model to use)
  • What you're making it from (What stock you're using)
  • Any fixtures you're using to hold it down
  • How it's oriented in the machine
  • How the machine axis are oriented
  • Where the work origin is

In more advanced used they can also set

  • What machine you're using and what it's abilities are
  • What tools you're going to be using
  • Where the tools are in the tool changer

but our machine lacks these abilities so we're not going to worry about them

Settings and what to do

Setup Tab

These are the basic settings to tell fusion what you're making and how it's arranged in the machine

  • Machine - You can define the capabilities of the machine you're working with in a machine entry in the library but we're not going to because it's not needed but if you have a complex part with lots of tools and paths needed it may be worth doing
  • Setup - Milling should already be chosen cause we were on the milling tab
  • WCS - Defines how the axis are arranged and where the origin is. Can't use defaults here because the Boxford arranges the axis in a non-standard way.
    • Under Orientation, pick "Select Z axis/plane and X axis" then pick a plane that's flat in the Z-axis and the X-axis arrow. Select "Flip X axis" because the X-axis is reversed on the boxford.
    • For Origin you need to think about having a point where you can put the origin that you can get to because it makes things MUCH easier if you can position a tool at the origin while you're setting up. That normally means selecting "Stock box point" so that you can touch-off on the stock somewhere, but in this case as the stock we're using is the same thickness as the model, "Model box point" would work just as well.
      • For this model a point top-centre will makes things easiest but picking the top of one of the corners is also a common choice that can work well for other parts.
      • You can define any arbitrary point as the origin, but picking a point on the stock that you can get to makes setting up the machine WAY easier.
  • Model should already be selected as it's the only body available, if you have multiple parts in a design you need to tell it which one you're trying to make.
  • Fixture is for dealing with more complex work holding arrangements, it's out of scope for this induction.

Stock Tab

This section is for telling Fusion the size of the stock that you're making the part out of.

  • Mode is how you're going to tell fusion what size the stock is, either absolute or relative to the model and what shape the stock is. There are 3 basic shapes it knows, box (cube), cylinder and tube, if you have a more complex bit of stock then you can model it separately and use the "From Solid" option. We want "Relative Size Box"
  • Stock Offset Mode is how you're specifying the size of the stock, relative to the model, The default is fine but more complex options are available if your model/stock is very asymmetric
  • Stock Side/Top/Bottom Offset is how much larger the stock is than the work, Fusion needs to know this because it restricts how the tool can approach the work without hitting things. Side offset we're going to set to 10mm which is larger than any of the tools we're going to use. The actual size the stock is doesn't matter too much IN THIS CASE, it just needs to know it can't have tools fast-approach from the sides. We'll set the top offset to zero because out stock is the same thickness as what we're making.
  • The "Dimensions" section will tell you how large Fusion thinks your stock is. This is as a check to make sure that the values you've given are reasonable.

Post Process Tab

These settings are for more advanced machines that have multiple work and tool offset systems, we can ignore them.

Now we've got that set up, it's a good idea to hide any origins or sketches from the model view or it'll just get confusing.

Setting up the workspace
Planning and order of operations
  • It's likely that your job will require more than one tool and more than one machining operation
  • You must consider how to divide your job into individual tools and operations
  • This is one of the hardest parts of efficient CNC machining as dividing your job up into operations in the proper order can have large effects on the efficiency of the program
  • Some operations HAVE to be done before others for various reasons
    • Removal of references - If an operation removes the reference surfaces that you were using to set tool positions then the removal of these surfaces will make setting up later operations more difficult or impossible. For example if you've picked the top surface of the stock as your Z=0 reference and you then mill away the top of that stock, especially if you do it in a way that doesn't leave a flat surface then it will make it much harder to set up later tools.
    • Making surfaces unsuitable for later operations - If you're shaping the surface in certain ways it may make it impossible or difficult for subsequent tools to engage properly with it. For example drills do not like entering sloping surfaces so it's often necessary to drill holes before you machine surfaces around them
    • Preparing surfaces - Some tools need a specific surface feature in order to make a clean entry into the work, so you might have to machine such surfaces into your part before the later operation, even if you're going to to machine them away again later.
  • Once you've worked out what operations you're going to do and in what order, you need to decide what tools you're going to use.
  • Tools must be suitable for the material that's going to be machined as some tool types and coatings are only suitable for use with certain materials. The tools you choose must be of sizes, lengths and geometries that are suitable for the job, not so large they can't get around the work easily, not so small that machining will take forever, not so long that they'll be too weak for the job, not so short the chuck will collide with the work.
  • It's usually best to choose the largest, strongest tool that's practical for any given operation as that will allow you to machine the material the fastest.
  • You might add some additional tool passes that aren't actually included in your original design, such as cleaning or de-burring the work.
Planning out jobs properly is critical

Workflow for this part

For this induction we're going to divide the work as follows

Operation Tool Why?
Centre-drilling for the notches in the edge of the disc 1/4" HSS Centre-drill We're going to drill those holes with a regular jobber drill and they tend to wander if we don't centre or spot-drill first.
Drilling the semi-circular holes in the edge of the disc 4mm HSS jobber drill Once the perimeter is milled, a drill won't be able to cleanly enter at this location so we have to drill it first
Cutting out the main body of the part 6mm Carbide single-flute end mill We've done everything needed to prepare, now time for the main operation
Extra-operation - de-burr the edges of the part 1/4" HSS Countersink bit Might as well de-burr it as best we can because it'll make it safer to handle. We can't de-burr edges before we've made them so this has to come last.

Setting up tools and choosing order of operations

Topic Content Reason
Setting up tools
  • Now the tools are chosen it's necessary to tell Fusion360 which tools we intend to use in this setup
  • This is done by adding the tools to the local library, it is possible to select tools on the fly from the standard list while creating toolpaths but it's better to create a specific set of tools for this part that you can tweak for it
  • Under the "MANAGE" drop down you'll find the tool library, open it
  • It will offer a selection of tools that are already available in the following sections
    • Documents - Tools that are defined for this specific model and setup, most of the tools you use should normally be here
    • Local - Tools that are specific to this computer terminal. This isn't very useful for us but in a production environment you would have all the tools loaded in a specific machine that your terminal is connected to defined here
    • Vendors - Vendor specific tool definitions supplied to AutoDesk by that maker. Unless you have that specific tool, from that specific maker, do not use these
    • Samples - Example tools that are close to what you might be using. The idea is that you copy tools from the samples section into the document or local libraries and adjust them for our machine.

The defaults are usually unsuitable so users must be able to make their own libraries
Defining tools
  • Defining a tool from scratch
    • Make sure you have the document we're working with selected because we're going to have these definitions linked to the document so they will export with it. That makes it easier to move your design around machines.
    • Click the "New Tool" icon top right of the library window
    • There are 6 tabs available to define the properties of the new tool
      • General - Give the tool some descriptive name so you can find it again
      • Cutter defines the shape of the tool
        • Type offers a selection of the more common tools, if you have something not on this list then it needs to be defined as a "form tool" in a different library
        • Pick Centre Drill
        • Number of flutes is 2 for this tool
        • Pick HSS for material
        • We don't have through-hole coolant option on the Boxford
        • Geometry - Define the shape of the tool, be careful to be accurate as if you set this wrong then Fusion will cut your part the wrong size. As you update these numbers Fusion will update the drawing of the tool so you can see if the values you've picked look reasonable.
      • Shaft tab defines any shaft extensions you're using with the tool, we're not so leave it blank
      • Holder defines what size of tool holder the tool is fitted to. In more complex designs Fusion will use this information to analyse if it's able to mill the part without colliding the tool holder with anything. There isn't a definition for the hold we have and it's not important for the part we're making today so please pick "Maritool CAT40-ER25-2.5" as that's close enough.
      • Feed & Speed - This is the important one! Here's where we define how the tool should actually be used. Many of the parameters in this page are inter-linked, changing one will change others. Let's start with the "Speed" part of feeds&speeds, in this case it's marked as surface speed. Typical surface speeds for various material and tool combinations are
Tool Speeds (m/min)
Material HSS Cobalt Carbide
Plastic 15 15 Not recommended
Aluminium 100 150 300
Brass 75 125 200
Steel 25 35 65
Stainless Steel 20 25 40
Titanium alloys Not recommended Not recommended 15
Tool Steels Not recommended 10 30
        • We can start by inputting the speed from this table into Fusion and it will calcualte an RPM. For a tool this small this rpm is likely to be higher than the Boxford's limit of 3000rpm.
        • These very high Rpms recommended for some tools are why you might choose to use HSS instead of carbide in some situations, the lower recommended speeds for HSS will mean that the rpm requried is closer to what the boxford can do.
        • If the recommended speed exceeds 3000rpm then over-ride it and put 3000rpm in the box, surface speed will be automatically recalculated.
        • Next we set the feed per tooth. We don't provide tables for this so it's up to your judgement to pick a suitable value. What is a suitable value will depend on tool size, cutting speed, machine quality and other factors. An FPT of less than 10% of the tool diameter is a realistic maximum for very heavy cuts.
        • For this tool we'll set 0.05mm as the FPT for milling, and 0.1mm FPT for plunging.
        • Fusion will generate feed rates for us. At the moment we're recommending 300mm/min as a maximum feed rate so if the calculated values exceed that then over-ride them
      • Post-Processor - We need to set coolant type to flood, everything else can be ignored as it's for machine that have tool changers and ours doesn't
    • The tool is now defined so click OK and you'll see the tool has appeared in the tool library for our document so it can be chosen for tool paths for this document.
  • Copying an existing tool
    • Copying an existing tool is an easier option if the Samples section of the library already has a tool that's very close to the one you need
    • In this case our next tool is a 4mm jobber drill, so go to the samples section and pick "Metric - Aluminium"
    • In that list you should find "Ø 4mm 118° - drill" Select it, right click, copy tool
    • Go back to the document section of the library, right click, paste tool
    • We now have that tool added to our library, but it will still have the default values for things like speed and feeds, so edit it to change them to more useful values
    • It will have defaulted to a drill-chuck holder, so over-ride that too back to the "Maritool CAT40-ER25-2.5" because we're going to hold it in the ER25 collet.
Telling Fusion what tools to use
Picking the rest of the tools
  • Now you know how to define tools, please also define the 6mm end mill and the 1/4" countersink that we're going to use for deburring.
  • There is a 6mm flat end mill in the samples section to copy, but please note that our 6mm is carbide and single fluted
  • The countersink you're going to have to define from scratch.
  • Once you're done close the tool library and we're ready to move on to defining tool paths
Getting all the tools set up
Choosing the order of operations
  • We need to pick the best order in which to do the 4 operations we've set tools for
  • Some choices are forced
    • Centre drilling must be done before drilling
    • Deburring has to be last as we can't deburr edges till we've made them
  • That only leaves one decision to make, milling the perimeter, and drilling out the side notches, which to do first?
  • If we milled out the perimeter first then the drill would be coming down onto an area that's been 50% milled away already, that would tend to force the drill off-course
    • Drills should only come down onto flat, complete surfaces, if they meet another surface while drilling then at best they'll be forced off course and make a non-round hole, at worse they'll break
  • So that only leaves us one reasonable choice for order of operations
    • Centre Drill
    • Drill
    • Mill perimeter
    • De-burr
Need to choose the order of operations such that it's possible to machine easily

Setting up tool paths

Topic Contents Reasons
Types of tool path
  • Along the top of the fusion window are 3 sections, "2D", "3D" and "Drilling"
    • 2D mostly defines tool paths that are mostly in 2 dimensions, I.E. there's flat area being milled out
    • 3D is for tool paths that are fully 3 dimensional, typically curved surfaces and other complex shapes
    • Drilling defines tool paths that involve a tool plunging straight down into the work.
  • Be very careful of any toolpath options with the blue-and-white spanner logo on it, these are paid-for options
    • They're intended to be basically micro-transactions for Fusion360, but they're "micro" only by commercial standards, these highlighted options can cost anything from £1 to £25 per use!
  • We will not be going over all the toolpath options today, there's more than 30 different types of tool path so we're only going to cover those actually needed for this job, the rest you can explore on your own or you can eMail Steve or Toby for help with them.
  • Be aware that what toolpaths are available and what they do change frequently as Fusion360 is updated, if you're loading an old design, or haven't used fusion in a while then take extra care to make sure that you're still getting the intended result.
There are loads, users need to be aware of them
Centre Drilling
  • Select the drilling toolpath option from the drilling menu to start a new drilling toolpath
  • It should come up with a window asking you to select the tool and the Feeds & Speeds
  • When you select the centre drill a transparent image of it will appear on screen and the Feeds & Speeds section will be filled in with values taken from the tool definition. A new toolpath labelled "Drill<?>" will appear in the structure menu on the left. At this point if something about the part demands it, you can over-ride the feeds and speeds set for that tool without having to edit the tool profile. Changes made here will apply only to this tool path and won't be copied over to others.
  • Set Coolant to "Flood" if it isn't already, so that the boxford knows we want to use coolant with this tool. There are lots of different coolant types that can be used in CNC machine but "Flood" or "Off" are the only settings the boxford understands.
  • On the second tab
    • Hole Mode - How you're going to tell it which holes to drill. Selected Faces is easiest, Selected points will require that you have holes that don't go right through the work. Diameter range will choose all complete cylindrical holes in a given range. Leave it on faces because none of our drill holes are complete on the model
    • Hole Faces lets you select all the faces that define the holes we're going to drill. Holes do not have to be complete, anything that fusion recognises as a cylindrical feature can be used. This is why it was so important not to import meshes when designing parts, if we had then fusion would be unable to recognise these faces as part of a cylinder. Please select both notches and the centre arc faces.
      • We're going to drill the centre even though we don't technically need to as it'll improve chip clearance later.
    • The other settings are for optimising the process, we won't get into them now
  • The third tab is for defining the various heights things will happen at
    • When you switch to this tab a transparent image of the holes to be drilled will appear so you can see what material it's planning on removing
    • They can all be defined relative to layers of the model, the stock, or each other.
    • Clearance height - How far up to start and stop the toolpath, the default is normally fine but you might set it higher if the part has a lot of tall features and you need to miss them when moving between toolpaths
    • Retract height - How high to lift the tool out of the work when moving between holes
    • Feed height - How low to rapid-move down before switching the slower speed for normal machining. Setting this too high can slow your tool path down a lot. It's common for retract and feed heights to be the same but they don't have to be
    • Top height - How high above (or below) the work the tool will be when it engages with the work. Usually zero but might not be if you're drilling a surface that you'll later be machining more
    • Bottom height - How far above the bottom of the hole/work to stop, or how far through it and out the bottom to go if negative
    • Drill tip through bottom - Whether to measure from the tip or shoulder of the drill
    • All of these can be left on default apart from "Bottom Height", set that to -2mm so that it drills right through the work and so that the cone part of the centre drill engages with the top of the work. Drilling through bottom like this REQUIRES that a sacrificial block be used under the part, or you're going to drill down into the table
  • Fourth Tab
    • Cycle defines the type of drilling operation that's going to be done. There's too many to go through now but spot-help will tell you more about them all. For now leave it on "Drilling - Rapid out" which will drill the holes as fast as it can in a single operation
  • Click OK and Fusion will generate a toolpath for this operation
  • When the toolpath is selected it will show a diagram of what it intends to do
  • Clicking on the toolpath in the structure menu on the left will let you re-name it to something useful
Setting up a first toolpath
Simulating a toolpath

If we want to simulate the toolpath so far to see what's going to happen then you can right-click the toolpath and choose "Simulate" and the simulation controls will come up. The "Display" option lets you choose what will be shown on the screen (it's a good idea to turn on stock) and the controls at the bottom let you run the simulation back and forwards at varying speeds. The "Stop on collison" option under the stock section is especially useful as it will cause Fusion to detect and throw an error if the holder or a non-cutting part of the tool hits the work anywhere (or hits the holding fixture if you've defined one).

The "Info" and "Statistics" tabs will give you useful information about the toolpath, how long it will take and how much work it's going to do.

It's also possible (and wise) to run a simulation on an entire setup or chain of setups once you've got all toolpaths defined. That will cause fusion to go through the entire machining process that it's planning and will help you see if there are any problems.

Simulations are invaluable for spotting issues

Since we're going to be drilling in the same places that we centre-drilled we can save time by creating a derived operation rather than starting fresh. Right click the centre drill toolpath and go to "Create Derived Operation; Drilling; Drill" and a new toolpath that's a copy of the old one will appear

Right-click; Edit this new tool path. Most of the settings can be kept the same because we're drilling at the same point but the tool needs to be changed to the 4mm Jobber Drill. Check that the coolant is turned on and that none of the feed rates exceed 300mm/min, if they do correct them.

On the geometry tab nothing should need to be changed as it's all the same as the previous toolpath, same for the heights tab.

On the cycle tab we're going to change to a different cycle. "Drilling - Rapid out" would probably work here, but it would be nicer on the tool if we helped it clear the chips more easily. Change the operation to "Deep Drilling - Full Retract" which will cause it to "peck drill" by drilling a little bit then pulling the drill bit out to let the swarf clear before going back in. The Pecking settings will define a maximum and minimum depth for each peck in this case please check that "Pecking Depth" is 2mm, "Pecking Depth Reduction" is 0mm and "Minimum Pecking Depth" is 2mm. Dwell tells the drill to hold at the bottom of the hole for a moment before coming out which is useful if you need a polished finish at the bottom of the hole, we don't care since we're drilling right though.

Click OK to complete this toolpath, and then give it a useful name in the same way you did for the previous one.

Basic drilling set-up
Cutting out the main part

To mill away the main part and cut it free of the stock we'll need to use a milling cutter. As the bottom face of the part is flat we can use a 2D milling operation.

  • The most suitable 2D milling operation for this is "2D Contour Milling" so select that from the drop-down menu and pick the 6mm End-mill as the tool
  • Feeds and speeds should have been automatically filled in, check them for reasonableness and make sure cooling is set for "Flood"
  • Under the geometry tab we need to pick which contour we wish to mill, in this case it will be the bottom outer perimeter of the model
  • Tangential extension isn't helpful here so ignore it
  • Tabs are useful! If we were to mill the entire model out of the stock at this stage we'd have it loose and risk it banging into the cutter, it would also move which means we couldn't then do the deburring pass. So turn on tabs.
    • Tab shape can stay as rectangular
    • Reduce the tab width to 4mm, this is a small, lightweight part, we don't need large tabs.
    • Tab height can stay at 1.5mm, we're going to mill down to 1mm below the bottom of the work to ensure that we cut it out cleanly. Tab height is measured from the bottom profile so we should be left with a 0.5mm thick tab which will work nicely here.
    • Tabs can either be automatically placed at set distances or you can manually placed points, use manual for this
    • Using the Tab positions option please position 4-6 tabs around the work where you feel is suitable.
  • The other options on this section can be useful for more complex jobs but won't cover them today
  • The heights tab works as before but please set a bottom height of -1mm from selected contours. This will mean the program will mill out well below the stock and into the sacrifical block to make sure it comes loose when we want it.
  • The passes tab allows you to set up a variety of options for making multiple passes when machining. This can be very important on larger jobs and ones where surface finish is important but we won't be using most of these options today
    • The only one we're going to look at is "Smoothing", this allows Fusion to smooth out small details of the design in order to make less small moves, making your program smaller and more reliable. A value of 0.05mm is reasonable for this but of course larger or smaller parts might want different values.
  • The linking tab controls how this toolpath interacts with others, how to lead in and lead out of the work if that's suitable for what you're doing, and how to use ramping and other entry strategies.
    • We're going to use a ramping strategy, this is a way to get around the problem that end-mills don't plunge well. Instead of plunging straight down then moving around the contour the tool will slowly spiral down into the work until it reaches the proper height.
    • For spiral toolpaths like this, lead-in is not needed as the toolpath starts above the work anyway, so turn off lead-in.
    • Lead out is still helpful so leave it turned in, the defaults should be fine
    • Turn on Ramp
      • Ramp angle is how steeply the tool will spiral down into the work. It varies from tool to tool but usually quite low values like 2° are more likely to work than steeper ones.
      • Maximum ramp stepdown sets how deeply the tool will move into the work before it makes a complete circuit around the job to clear away material. This interacts with Ramp angle and may result in extra passes being made if you set it too conservatively. In this case we're going to use 2mm, which is actually a rather shallow step-down but it will result in a program where you'll be able to see more clearly what it's doing when you're running it later.
      • Ramp clearance height is how far above the work the ramp will start, depending on what you're doing and how slow your feed is you might find this can waste a lot of time, so let's use 1mm.
  • The milling toolpath is done now so give it a useful name like you did for the others
Introduction to some of the basic milling options
Deburring pass

We now want to use the machine to remove the sharp corner that's left on the upper surface of the part. We can do this using another 2D contour type operation and a countersink bit. We don't need to design the chamfered edge in the model as there's a program specifically for doing things like this

  • From the 2D dropdown menu select "2D Chamfer" and choose the countersink bit, as before feeds and speeds should have been automatically set but check them anyway
  • When selecting the geometry, pick the TOP perimeter.
  • Heights shouldn't need adjusting as this time we don't care about the bottom surface, we're not machining near it
  • As before passes can be ignored as we're not making multiple passes but we do need to set the chamfer properties
    • Chamfer width what it sounds like, 1mm is a good choice
    • Chamfer tip offset controls how far up the side of the tool it will be cutting. Lower values result in less risk of scratching the part with the end of the tool but higher values will allow faster cuts and longer tool life. 2mm should work here, simulation can be used to check values to make sure you get the result you want
    • Chamfer Clearance is how far the tool is to be kept away from other sides of the work to avoid damaging them, 1mm is plenty.
  • Set up smoothing of 0.05mm as for the previous path
  • Setting a lead in and lead out in the linking tab is a good idea to get a nicer surface finish.
Deburring is a useful safety measure
Final Simulation

Now that you have all the toolpaths defined you can go to the setup, right click and simulate the entire machining process that you've programmed. Please do this, and look very carefully at what the tool is doing and what shape you are making. If you've got any problems, questions, or anything that doesn't seem right, now is the time to ask about it!

If your simulation looks good then we're done for this session, and it's time to arrange your one-on-one induction session downstairs with the Boxford.

Final sanity check

If you'd like a refresher on this then AutoDesk has got a tutorial on their site at It takes about an hour and covers all of what we've talked about here although obviously some operations are more relevant than others because of the different models in use.

Second session

This second session will be 1-to-1

Safety and Start-up proceedure

Topic Contents Reasons
Personal Safety
  • The Boxford will throw chips, if you break a cutter it can throw razor sharp shrapnel, googles are compulsory
  • The compressor is required, and noisy, ear protection is strongly advised for all but the shortest jobs
  • Despite our best efforts the lubrication system does still put a small amount of oil mist into the air, respiratory protection is sensible if doing longer jobs
  • Milling cutters are usually (literally) razor sharp and must be handled with considerable care. Gloves are usually not possible as fine manual dexterity is needed, so you just have to take care and try to avoid touching the cutting surfaces
  • The Boxford moves and starts & stops it's spindle automatically. Although we recognise that sometimes it will be necessary to reach inside the enclosure while the machine is powered up, you must at all times remain well clear of the spindle and cutter. Long or loose sleeves pose a risk of serious injury and are to be avoided while using the Boxford.
  • The motors driving the table and spindle are STRONG, the force required to cut hard materials is very high so the motors have to be powerful, if you get caught by them or get any part of you trapped in a pinch-point, they can easily break bones.
Keeping people safe!
Machine Safety
You have been warned
  • The Boxford is a powerful machine but it's stupid, it has no concept of what might harm it and will cheerfully do what you tell it to even if that's destructive. Since the Boxford is dumb, you have to be the brains of the operation and think things through before you do them.
  • You have to make sure that only suitable materials are used in the Boxford, anything that's hardened, or that will produce abrasive dusts is not allowed, wood is not allowed because sawdust gets everywhere and absorbs all the lubricant on key surfaces
  • Right now the Boxford has no limit switches, we plan on fixing this in the future but until then there is nothing stopping you driving the table or spindle off the end of their lead screws and causing serious damage, you need to be aware of the travel limits and not exceed them
  • The Boxford has nothing preventing you from driving a cutter hard down into the table, wrecking both cutter and table. Please do not to this.....
  • Debris left around the table can get caught up between the table and the housing of the machine, resulting in damage
  • Objects left near the table can crush or cut important cables when the table moves
  • Workholding systems must not protrude too far over the edge of the table or they'll hit the enclosure.
  • The spindle will overheat if run at full speed for prolonged periods; monitor this while it's running.
Keeping the Boxford safe!
Cleaning up the machine
  • The machine won't have been left spotless but it should be clear of any large build-ups of swarf of objects inside the enclosure
  • Turn on the Boxford and its monitor
  • Drag the compressor out and get it filling up its reservoir while you're cleaning and the Boxford is booting up
  • If the machine is noticeably dirty or obstructed then you will need to clean it up before starting
  • Operate the one-shot oiler. If the handle comes back down too fast then check if there's oil in the reservoir. If it's empty it should be filled up with the ISO 220 Waylube from the bottom drawer of the black cupboards by the lathe.
  • Most of the machine just needs to be reasonably clean, but the area of the bed where you're working and the inside of the spindle need to be immaculately clean. Even the tiniest bit of swarf or dirt will upset your positions and risk breaking tools.
  • Set up the Air system
    • Connect the compressor to the Boxford using the air hose to attach it to the port on the right of the machine. Make sure to set the regulator on the compressor to zero before attaching the hose or it may whip around and will be much harder to seat on the connectors.
    • Set the regulator on the compressor to 5 Bar (0.5MPa, 70PSI)
    • Set the oil metering pressure (top regulator on the right of the Boxford) to 1 Bar (0.1MPa, 15PSI)
    • Set the air jet pressure (lower regulator) according to what material you will be working. Suitable pressure depends on how "gummy" the metal being cut is. Aluminium needs the highest pressure, brass the lowest; steel is similar to brass. The normal range of pressures is 2-4Bar (0.2-0.4MPa, 30-60PSI)
    • Empty the water drains on both regulators, this is done by pushing in the buttons on the bottom. Be aware they may shoot out some rather nasty rusty water all over anything you leave near them. The drains may have be emptied regularly while the Boxford is working.
Getting the machine set up and ready to begin work.
Activating the CNC system
  • Start Fusion360 and log in
  • Start CNC.js from the shortcut on the desktop
  • Log into Fusion360
  • On CNC.js the connection menu can be popped out from the left. It should indicate that you are connected on COM4, if not then tell it to connect
  • The Boxford will usually start up in alarm mode as a safety feature
    • To return to normal mode, check the E-stop button is released
    • Press "Reset" button at the top-right of the screen (status indicator top left should show "Alarm")
    • Press "Unlock" botton at the top-right (status indicator should switch to "Idle")
  • At the top of the menu section on the right in the Axes section are 2 mode indicators
    • MDI (Manual Data Input) means the machine is under computer control from the console
    • Keyboard means the machine is in direct keyboard control
    • The 2 sets of numbers next down on the screen are the machine and work co-ordinates
      • Machine Position represents where the Boxford thinks it is relative to the absolute limits of the machine. With no limit switches installed these numbers are essentially meaningless
      • Work position is where the machine thinks it is relative to the current workpiece. The numbers here won't be correct yet - we'll set them later
    • Below that are the motion controls, these buttons are used to move the table and head around and specify how it should be moved
      • G21 means the machine is operating in metric mode. It should not be put into inches mode or it's very likely to crash.
      • The distance number indicates how much the machine will move per press of the button or per keypress
        • 0.1mm is a good setting for this, as using speed mode (holding down shift) will move 1mm at a time and using slow mode (holding down alt) will cause it to move in 0.01mm steps
    • When in keyboard mode the arrow keys control the motion in X and Y, PgUp and PgDn control the Z-axis, holding shift makes it move at 10x speed, holding alt makes it move at 0.1x speed
      • Tap at the keys, do not hold them down, or it may move much more than intended and you'll have to use the E-stop button to prevent a crash.
  • The G-code box contains information about the currently loaded toolpath
  • The Spindle box controls rotation of the tool and operation of coolant
    • M3 starts the spindle rotating in the normal direction at the specified speed, M4 does nothing as this spindle does not support reverse mode, M5 halts the spindle
    • M7 turns on the air-blast chip-clearance system, M8 turns on the oil mist feed, M9 turns off both.
    • All these controls are locked-out when a program is running
  • The Probe and Macro options are not yet implemented on this machine and should not be used.
Basic operation of the CNC system

Work and Tool setup

Topic Contents Reasons
  • Work needs to be securely fixed down to the table
  • You need to consider where on the table you're going to mount the work as the tool will have to be able to get all the way around it without the work hitting anything or reaching the end-stops of the machine
  • Even very small amounts of un-evenness will result in an out-of-tolerance part. Very small amounts of movement while machining will ruin your surface finish or break tools.
  • If you're going to need any position reference marks on the stock then now is the time to add them
  • There are a number of ways that you can secure your work to the bed
    • Bolting directly to the bed
      • If your workpiece has holes in it, or if you can drill holes outside of the area to be machined then you have the option of using bolts to directly fix your work down to bed by using T-nuts in the slots on the table.
      • This is the most direct and potentially best way of fixing something down as it has the fewest number of elements between the table's motion control and the work.
      • If you do fix something down this way then extreme caution is needed to ensure that the tool will not collide with any of the fixing bolts, so it will usually be necessary to define them using the fixture function in Fusion360 so that it knows to avoid them.
      • Fixing work down this way will also mean that you cannot cut all the way through the material which will prevent you from drill through-holes or cutting the job free of the stock as the tool would wind up digging into the table.
    • Clamping bars
      • You can use the clamping bars to hold down your work by friction. This is the most common way of attaching work to the table as it's quick, has good security on mostly-flat objects and is quite flexible in approach
      • This is the method we'll be using today
      • The bars rest on the corners of the work, well outside the area that the tool is going to be moving around
      • The back of the bars rest on the step blocks in order to get them angled so that they're level, or preferably angled down onto the work
      • They must not be used angled up, they will not grip securely in that position
      • Bolts go through the openings in the bars and then fix them down onto the T-nuts that run in the slots on the table.
      • Having the bolt as close as possible to the work will increase the clamping force
      • Be careful not to tighten the bolt till it "bottoms out" against the bottom of the T-slots, if you do that it'll feel properly tightened but won't actually be clamping very well
      • When using the clamping bars you can place a sacrificial piece of metal underneath the work so that you can break through the bottom edge of the work and into the sacrificial piece without harming the table, this lets you cut material out from the stock, or drill through-holes.
      • Sacrificial pieces must be completely clean and de-burred before use
    • For objects that have a higher aspect ratio, the vice can be used
      • It bolts to the table using the T-slots
      • It has a plate on one side so that work can be reliably butted up against it, which makes for repeatable positioning if you're making more than one of something
      • Objects shouldn't over-hang the sides of the vice
      • To prop something up higher in the vice for better access, you can use the parallels to keep it level but propped up
    • For round stock that you need to machine, there are collet blocks
      • These are the same ER25 collets that we use for holding tools so I'll explain how to use them later
      • They're mounted on square or hexagonal blocks so you can rotate them in fixed steps to produce square or hexagonal features
      • They're normally held in the vice
    • Superglue fixtures can be used to hold flat sheet
      • For large flat sheets that you're going to be machining on top of a sacrificial block, you can use tape and superglue to hold them down. Check YouTube for videos on how to do this as it's too complex a topic to cover today.
Material needs to be fixed securely both for safety and to get good results.
  • The Boxford uses the Coventry EasyChange chuck system
    • These tool holders are removed by pressing in the brass button and rotating the collar clockwise (when seen from above) and wiggling the tool holder until it releases
    • The collar should lock into that position once the tool is removed, but it often fails to do so
      • If you get a failure to lock then you need to press in the brass button while rotating the collar and using the 2 drive lugs on the lower surface to stop the inner spindle rotating
    • Tools will automatically lock into place when pressed firmly upwards into the spindle. This lock should happen with a quite positive "click" and the collar rotating back to its resting position
      • Both the tool holder and the inside of the spindle should be checked for debris and cleaned if necessary. Swarf or other debris inside the spindle will result in poor tool clamping which will cause out-of-tolerance parts, bad surface finish and maybe tool breakage.
  • The main tool holders we use for milling are based on the ER25 collet system. There are also a few holders for other things such as a drill chuck, some plain drilled holders and one insert holder
  • For the induction we'll only be using the ER25 holders
    • The ER25 collet set is kept in the top-left drawer of the Boxford tool chest
    • The tool-setting block should be held in a vice to help you install the collets and tools
    • The internal taper of the tool holder and all parts of the collet should be well cleaned before use
      • They are not supposed to be oiled, but a quick wipe with a cloth that's just slightly damp with WD-40 will prevent corrosion
    • All collets have a size range written on them, for example 7-6. That means the collet nominal size is 7mm but it can clamp down a minimum of 6mm. Tools larger than 7mm must not be used in this holder as the 7mm nominal is a maximum and the jaws of the collet should never be spread wider to fit larger tools.
    • A tool stick-out of 20-25mm is normal in order to allow enough clearance around the holder when in use but still get a good grip on the tool. This is an approximate guide only and it's important that all tools are held securely. Never allow the collet to grip on the cutting area of a tool as that's sure to damage both collet and tool
    • The collets should be rotated into the retaining nut as it has an asymmetric flange designed to hold the collet. Under no circumstances should the collet be put into the holder and then the nut tightened on top. The collet always goes into the nut first and is then fitted into the collet holder.
    • The collet nut should be tightened firmly. The maximum allowed torque for an ER25 nut is 110Nm but in practice you're very unlikely to need anything like that much.
    • Once the tool is securely fitted into the holder, the holder can be inserted into the spindle which loads the first tool that's required for your program.
    • Start the spindle turning at 300rpm and visually check the tool is running straight, drills can be deceptive and look wonky when they're not but make sure the tool isn't wobbling, stop the spindle as soon as you're sure the tool is properly mounted
Proper tool holding is essential to avoid breakages
Setting offsets
  • At this point the Boxford still has no idea where it is relative to its work space, or where the work is within the work space
  • Having the machine locate its self within its work space relies on limit switches which are not currently installed so that's not possible
  • Even without absolute positioning it's possible to tell the machine where the tool is with respect to the work and that's enough to let it operate so long as you're careful with positioning everything within its working volume.
  • How to define this position will depend upon what sort of work you're doing
    • If it's a object with a substantial Z height or requires accurate positioning within the X/Y plane then the edge-finder can be used to locate the stock accurately
    • <how to use edge finder>
    • For situations requiring less precise location then you can scribe a reference mark onto the stock and then approximately line up the tool by eye.
    • Today we're going to be setting the X and Y positions approximately as we don't care too much about the exact position of the final object within the sheet of stock.
    • Using the keyboard controls we can move the tool down close to the stock and jog it around until the tool is as close to properly centred over the reference mark as we can get.
    • At this point we can define this position as X0 Y0 by pressing the "Zero out work offset" buttons on the Axes panel on the screen (the ones that look like a Google Maps pin and are in the "Work Position" column)
  • At this point we're only zeroing the X and Y axes as the Z hasn't been referenced yet
  • Now we slowly lower the spindle until it is very close the work. As it becomes close we insert a section of metal shim of a known thickness between the tool and the work and slowly adjust the spindle height until the shim feels a light resistance to being moved in between them
  • At this point the tool is the thickness of the shim above the work so we need to tell the controller that. Click on "Set Work Offset" in the work position column for the Z axis. This lets you input the current position of the tool relative to the work. As the tool is above the work it's position is positive so you enter a positive number that represents the thickness of the shim, I.E. for a 0.15mm shim, enter "0.15" as the current position.
  • In time we hope to automate the setting of the Z height using a touch-probe but this is not yet available. This will vastly speed up tool changes as the Z offset changes every time you change tool but the X and Y offsets do not.
  • We've now defined the centre of the top surface of the stock as position X0 Y0 Z0 - in other words the origin. This works in this case because when setting up the job in Fusion we specified the top-centre of the stock as the origin. If we had chosen to put the origin elsewhere then we would have had to work out how far from the origin the reference positions were and used the "Set Work Offset" function to tell the Boxford where the tool was relative to that origin.
  • At this point it is wise to move the tool up well clear of the work, for example by 15-20mm, so that when your program starts the tool is well clear of any obstacles and to give the spindle time to get up to speed before encountering the work.
The CNC machine needs to know the relative positions of its self and the work

Generating, loading and running G-Code

Topic Contents Reasons
Generating your G-code
  • The Boxford is controlled by a program written in a language called G-code
    • G-code is composed entirely of short letter-number codes that are very hard to read
    • G-code has several hundred(thousand) possible commands, many of which are almost identical but vary in subtle ways
    • For all but the most trivial programs it's very rare to write G-code directly; people almost always have a CAD program make it for them
  • The first step is to get Fusion360 to output the toolpath as a G-code file
    • This file has to be customised to the tool that's going to run it, in this case the Boxford
    • This customisation is done using a program called a post-processor
    • Because of the way CNC.js works it's normal to output each toolpath as a separate G-code program. More complex tools with automatic tool-change options will usually output the entire job as a single program
    • Select the toolpath you want to output, right click and select "Post Process"
    • The correct post-processor is already set up. DO NOT CHANGE ANY OF THESE SETTINGS
    • Click the "Post" button to output your G-code
    • It will ask you for a filename and location, we suggest making a directory with your name and putting your G-code files in that directory
      • Please remember that as with all shared PCs at rLab, YOUR FILES ARE NOT SAFE HERE. They may get deleted or altered at any time and without warning.
    • Fusion has now saved the G-code for your toolpath, running on this milling machine
  • The next step is to load your G-code into CNC.js so it can be run
    • Switch windows to CNC.js
    • Click the blue "Upload G-code" button in the top left of the main window and select your file
    • Depending how complex the toolpath is it may take some time to visualise it
    • Move around the visualisation and check that it's doing what you expect it to do
    • CNC.js is now ready to run your toolpath
Getting the machining operation from Fusion onto the Boxford
Setting up the air-blast
  • When a milling cutter is moving through material it makes a lot of small chips of the material
    • It's vital to remove these from the cut, if they're allowed to build up then they'll start to clog the cutter, soon there'll be no room for new chips and so they'll start to pack in tightly
    • If they're not removed then the cutter will be unable to continue cutting through the material and will start to get hot
    • Very rapidly, within seconds, the cutter will become so clogged that it can no longer remove material at all, and now when the machine pushes the cutter into material it cannot remove it will snap off
    • As heat builds up the chips will also start to stick to the cutter, dulling it's edge and resulting in more heating in a viscous cycle. Aluminium is especially bad for sticking, Steel is better, Brass almost never sticks.
    • For some metals and cutter geometries the action of cutting alone will be enough to keep chips clear of the cutter but in most cases additional help is needed
  • For these reasons the Boxford is fitting with an oil mist cooler, it does 2 jobs
    • A powerful air blast removes chips from the cut and cools the tool
    • A faint mist of oil added to the air coats the tool and lubricates it which helps make cutting smoother and cleaner
  • Before use the mist cooler needs to be correctly set up
    • Check the oil level in the mist cooler oil tank. The rate of oil consumption is very low and a full tank would last many hours of machining.
    • Ensure goggles are on, the cooler can throw chips and other loose material around with considerable force
    • Point the cooler in a safe direction in case anything is ejected when it turns on.
    • Turn on the airflow using the M07 command on the CNC.js control screen
    • Check that the airflow is at a level you'd expect and the nozzle is clear
    • Turn on the oil flow using the M08 command
    • If the boxford hasn't been used for some time then the oil feed pipe will be empty, in which case you'll need to prime it
      • Using the needle valve on the oil line just outside the main enclosure, adjust the oil flow till it fills the tube in a reasonable time
      • When the oil nears the mixer block at the back of the nozzle then turn it back down again
    • Using a hand or bit of tissue held in front of the nozzle, adjust the oil flow with the needle valve until the oil is just barely flowing.
    • There should be enough oil to make a test piece look slightly shiny after a few seconds. Be aware when adjusting that there is a considerable time lag between a change of valve position and a change in oil flow rate out the end of the nozzle
    • Once the oil flow is at a rate you're happy with turn off both oil and air with the M09 button on CNC.js
  • Now you need to move the nozzle into position such that it will direct the air/oil mist as much into the cutting zone as possible. Having it positioned higher up the tool will not get the proper effect but at the same time you also need to consider how the cutter is going to move relative to the work. You'll have to make sure that the nozzle won't foul on any part of the material as it's machined or on any of the holding systems.
  • Setting up the cooler is always something of a compromise and you'll never get it working perfectly for all parts of a cut but do the best you can
  • It might be helpful on some parts to split an operation into 2 or more tool paths so you can stop and move the cooler in between sections.
Why the air blast is needed, what it does, how to set it up
Air Milling
  • Air milling refers to the practice of having a test run of the milling operation without actually cutting any material
  • It can be accomplished 3 ways
    • Running the program with no material on the bed, this can catch some errors but runs the risk of still driving a tool into the bed if the program is wrong enough
    • Running the program with no tool loaded, this works well on thinner material but it can be a problem on large jobs where the chuck might try to move through space that should have been cleared in other operations
    • Running the program with tool and material loaded but with the tool in the air above the work, this is the one we're going to do today, it's especially easy to see if the program is doing what you expected, but does risk tool collisions with the material if your work is tall.
  • In order to make the machine operate in thin air we need to convince it that it's much closer to the work than it really is, we do this by adjusting the Z coordinate of the work offset
  • Using the keyboard move the tool up to a position of (0,0,25) - it's very important to remember this value as we'll use it to reset the position afterwards
  • Use the "zero out offset" button on the Z axis to tell it that this is the new zero, the machine now believes that the head is 25mm lower than it really is, so it's going to perform the entire operation 25mm above the material.
  • Move the tool up another 20mm from here to act as a safe start position
  • Put on your hearing protection if you're choosing to use it
  • Operate the Safety Goat
  • Close the machine doors
  • Press the "Cycle Start" button on CNC.js which is the "play" button next to the Upload G-code button
  • It will bring up an M6 - Tool Change warning, you can ignore this as we've already fitted the correct tool
  • Press "Cycle Start" again
  • It will ask for confirmation, position your hand over the emergency stop button, ready to use it if something goes wrong, then confirm you want to proceed
  • The Boxford will now start the spindle and air-blast and begin to execute the toolpath, watch it very closely as it runs to make sure that it's moving in the ways you expect, at the speeds you expect.
  • From time to time you may need to operate the water separator on the air line as it can fill up quite quickly under some weather conditions.
  • Once the toolpath is complete the Boxford will shut off the spindle and air and come to a stop
  • If it did something you weren't expecting then now is the time to look at the path in Fusion and figure out what was wrong and fix it.
  • If all went well then it's time to position the tool ready for the real cut.
  • Using the X0Y0 and Z0 buttons move the tool to where the machine thinks is the origin
  • At this point it should still be 25mm above the work as we fed in an incorrect tool offset earlier
  • Use the "Set Work Offset" function on the Z-axis to tell it it's real position, 25mm above the work
  • You've completed the test run so now it's time to run the program for real.
A vital test to make sure you've not made a programming error.
Running the program
  • The tool should now be at a suitable height above the work, so make one last check that the position shown on the CNC.js display and the apparent position of the tool match
  • Check that the tool is at a suitable height above the work to move to the starting position without hitting anything, move it further up if needed
  • Operate the Safety Goat
  • Close the machine doors
  • Press the "Cycle Start" button on CNC.js which is the "play" button next to the Upload G-code button
  • It will bring up an M6 - Tool Change warning, you can ignore this as we've already fitted the correct tool
  • Press "Cycle Start" again
  • It will ask for confirmation, position your hand over the emergency stop button, ready to use it if something goes wrong, then confirm you want to proceed
  • The Boxford will now start the spindle and air-blast and begin to execute the toolpath
  • As the tool begins to engage with the work you need to look very carefully and watch for signs of trouble
    • You're expecting to see a fine spray of chips coming from the cutter and being carried away in the air blast
    • Watch very closely for any signs that chips are packing up around the cutter
    • Watch closely for any signs of heating, or of a mound of material being pushed in front of the cutter
    • If either of these happen you'll have only seconds to hit the E-stop before your cutter and maybe your work is destroyed
    • If you have had to operate the E-stop see the section below about what to do next
  • From time to time you may need to operate the water separator on the air line as it can fill up quite quickly under some weather conditions.
  • Once the toolpath is complete the Boxford will shut off the spindle and air and come to a stop, it will not automatically move back to the origin.
Making your first cut and what to watch out for.
Changing tools
  • Now the first toolpath is done you'll need to change to the right tool for the next tool path
  • Ideally move the tool back to X0Y0 using the button on CNC.js but you don't have to if that would cause the tool to hit something
  • Using the Z move keyboard controls move the spindle up so you can get the tool out, be aware it may stick in a bit and come out suddenly, leave enough room so that you won't bang the tool or your hand into anything when it moves suddenly
  • Once the tool is removed you can use the tool-setting block in the vice to release it from the collet
    • Examine the tool carefully, use the microscope if you need to get a better view, the condition of the tool will tell you a lot about how the cut went
    • If the tool is still clean and sharp that suggests the cut went well
    • If there are signs of dulling of the tool edge or points then you need to consider how rapidly this damage occurred. All tools wear over time and will fail eventually but if tools are showing significant wear after less than an hour of use that suggests a problem with the toolpath that could be better designed
    • If there are large chips or chunks missing from the cutter this suggests that the toolpath is seriously defective and needs urgent attention. You should not run this toolpath again until you can make corrections. You should also examine your work carefully in case there are fragments of the tool lodged in it, if there are and they're not removed they're likely to destroy the next tool that's used.
    • (HHS and Cobalt tools only) If the tools is showing signs of changing to a blue colour near the cutting edges that suggests too much heat in the cutter, likely as a result rubbing or over-gentle cutting.
    • In any event if the tool is significantly damadged, it should be thrown away. Do not leave bad tools in the lab where they might cause problems for others
      • Dulled milling cutters cannot be (reasonably) resharpened, HSS, Cobalt and brazed carbide tools should be thrown in the normal bins, Solid carbide tools and carbide inserts should be put in the waste carbide container by the lathe. Blunted HSS/Cobalt drills should be put in the dull-drills pot to be re-sharpened.
  • Remove the collet from the ER25 chuck and clean it carefully, you need to ensure that there's no trace of swarf left from the cutting operation. The compressed air line that hangs on the side of the boxford that may help you with that.
  • Check what tool you need next by looking at the next toolpath in Fusion
  • Select that tool and a suitable collet to hold it, and fit it to the ER25 holder using the same procedure as you did for the first tool
  • Clean the spindle and install the new tool into it
  • You'll now need to reset the work offset as it will have changed with the new tool
    • The X and Y offsets shouldn't need altering as they're set for the center of the tool which is common to all tools
    • The Z offset definitely will need to be reset, so you need to move the X and Y axis so that the tool is positioned above an area of the workpeice that you haven't yet milled.
    • You can now reset the Z work offset as you did for the first tool
    • If there is no area where you haven't milled then this will be more complex.....
      • This is one the situations that you should try to avoid when designing a part, changing the order of operations will often let you avoid it but sometimes there's no choice
      • You'll need to find a flat milled area that's large enough to comfortably touch-off on
      • Check fusion and determine how far below the zero plane your touch-off surface is
      • Touch the tool off on the work using a shim as before, but this time you'll need to put a different value into the work offset, it'll be ({shim-thickness} - {distance below Z0 plane}), this is likely to be a negative number.
  • Move the tool up to a safe position so that it won't crash when it moves to the start of the next toolpath
  • Post-process, export and load the next toolpath as you did for the last one.
  • Operate the Safety Goat
  • Close the machine doors
  • Start the cycle as you did for the last toolpath, not forgetting to position your hand over the emergency stop button, ready to use it if something goes wrong.
  • All toolpaths must be closely supervised with a hand near the E-stop the first time they are run. Once they've been proven safe then you can relax a little for subsequent runs. You still have to remain next to the boxford and be ready to act if there's problems, but it's not required to hold your hand over the E-stop the whole time.
Changing to new tools so that users can run a multi-path job

Dealing with any problems, shutdown and clean-up

Topic Contents Reasons
Recovering from E-stop
  • If you have had to operate the E-stop it will halt the movement of the machine instantly
  • As soon as the machine stops moving, you now need to shut down the spindle as otherwise it'll restart as soon as the E-stop is released
    • Press the "unlock" button that's top-right on the screen
    • Use the M5 button to shut off the spindle
    • Twist the E-stop to release it because CNC.js will not give you full manual control while it's still operated
    • On CNC.js press RESET, UNLOCK, and Keyboard to give you manual control
  • The first thing you must do after any E-Stop is determine WHY it happened, if you don't know what went wrong you won't be able to avoid it in future
  • At this point whether or not you can recover your work will depend on what caused you to press the E-Stop.
  • If the machine crashed, some part of the spindle hit the work or workholding then your chances of recovering your job aren't so good
    • If the tool was driven out of it's intended path and into a part of your work that you didn't want to remove then your work is scrap and you'll have to start again.
    • If the work has been moved on the bed, either sideways or twisted then you'll need to use techniques beyond the scope of this induction to recover it
    • If your part has no remaining flat and vertical surfaced for both X and Y axis then your work is lost, you need to start again.
    • If none of those apply then you may be able to fix this.
      • Likely the machine has lost position and all your offsets are now wrong
      • Unload the stub of the tool and dispose of it as per the procedure in the tool change section
      • Examine your work carefully, if a tool broke then it's highly likely that there's a fragment of it lodged in the work and you MUST remove it before continuing.
      • If you have a suitable edges that are flat and vertical in each of the X and Y axis then you can use the edge-finder tool to pick them up and recalculate your X and Y offsets
      • Alter your toolpath in whatever way seems suitable to make sure you don't crash the machine again, next time you might not be so lucky
      • Change to a new tool, set your Z-work-offset and load your updated toolpath as in the section above, then continue working,
  • If you used the E-stop because a tool broke then you probably can recover your job and finish it.
    • The X and Y position values are almost certainly still correct so they don't need to be adjusted
    • Alter your toolpath in whatever way seems suitable to make sure you don't break the next tool, there's no point loading tool after tool and breaking them all with the same faulty toolpath
    • Unload the stub of the tool and dispose of it as per the procedure in the tool change section
    • Examine your work carefully, if a tool broke then it's highly likely that there's a fragment of it lodged in the work and you MUST remove it before continuing.
    • Change to a new tool, set your Z-work-offset and load your updated toolpath as in the section above, then continue working
    • It's likely that you'll have to run your toolpath from the start which might mean the tool spends a lot of time air-milling before it gets to the point where it crashed last time
Finishing and cleaning up
  • Don't un-bolt your work from the bed until you're sure you're done, it'll be very hard/impossible to resume work if you've released it
  • Remove your work, holding system, and any tool from the machine
  • Clean and put away the chucks and collets
  • Clean the machine down carefully. Be aware that there'll be a lot of oil on the walls that will take some care to remove and you're likely to get it on you, also be careful of swarf as it may have sharp edges
  • You may have to use keyboard control to move the table to get to everywhere, take care not to get yourself or anything else caught while doing so
  • Any of the standard hoovers, henry or scheppach can be used to clean up swarf
  • We do not recycle swarf, it goes in the regular bins.
  • The inside of the Boxford does not need to be spotless, but we do ask that you clean it out properly
  • Once everything is clean close down CNC.js and be sure to sign out of Fusion360
    • If you forget to sign out then the next person to use the machine may be able to edit your designs and some of our members have a rather robust sense of humour......
  • Shut down windows on the PC. It will try to auto-reboot, so as soon as the screen goes black, turn it off at the main power switch, then turn off the monitor
  • Disconnect, blow-down and put away the compressor
  • If you encountered any major problems, the Boxford behaved in unexpected ways or there was any damage then please contact Steve directly or post to the mailing list
Leaving the machine in a fit state for the next person