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 for Boxford 260VMC is divided into 2 sessions, the first session will be classroom based and lasts about 3 hours. It 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 is 1-on-1 and is based downstairs and covers actually operating the Boxford, it will take between 2 and 3 hours. There is a charge of £45 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 covers some metal stock and a basic set of tools sufficient for most standard milling operations.
This induction takes 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 does 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. The full boxford introduction workshop uses all sections of this induction. The standard induction for people already experienced with milling machines skips the "Principles of milling" section. The mini-induction for people who already have experience of CNC machining skips the classroom session entirely.
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 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.
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. The account can be commercial, educational or hobbyist, but it cannot be the trial version. The hobbyist version of Fusion-360 is free but Autodesk do tend to make it more difficult to find. If you need help getting a suitable version then let me know.
- 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, it doesn't need to be fast but Fusion360 must be basically functional on it.
- 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 £45 which covers all costs of the induction as well as providing the material for your test piece and a basic set of tools.
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:
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 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.
|Principles of Machining
||Basic grounding in how milling machines work|
|What materials can be used in the Boxford
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|
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.
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 hundreds 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
(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
|Types of cutter dictate what sort of jobs can be run|
|Feeds & Speeds
Two of the most important parameters for using any cutting tool are called the speed and the feed. If you think of the cutter as a razor moving into the work and shaving a chip off, then the speed is how fast the razor is moving through the material, and the feed controls how thick a section it's slicing off each time it passes
Speed is 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. This is a situation where HSS tooling can help because it required much lower surface speeds than carbide. 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 keep above 500 r.p.m. if you can.
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 but you can also think of it as how far into the work each tooth of the cutter is being advanced. 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, work material, and 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 800mm/minute for travel moves (the machine will enforce this) 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) 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
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 :
|You have to design according to the process you will be using.|
--- Pause here for questions ---
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
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", "Inspection", "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|
|Setting up the machine||
Before we can use a specific type of machine we have to set up the definition of it in Fusion-360 so that it knows what it's abilities are
Everything starts with a setup so please go to Setup under the milling tab and select "New Setup", Setups define
In more advanced used they can also set
but our machine lacks these abilities so we're not going to worry about them
Settings and what to do
These are the basic settings to tell fusion what you're making and how it's arranged in the machine
This section is for telling Fusion the size of the stock that you're making the part out of.
Post Process Tab
These settings are for more advanced machines that have multiple work and tool offset systems, we can ignore them.
|Setting up the workspace|
|Planning and order of operations||
||Planning out jobs properly is critical|
Workflow for this part
For this induction we're going to divide the work as follows
|"Decking off" the stock||12mm 4-flute end mill||Because the part is thinner than the stock|
|Centre-drilling for the notches in the edge of the disc and the centre of the part||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 and the centre of the part||4mm cobalt 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 2-flute slot drill||We've done everything needed to prepare, now time for the main operation|
|Extra-operation - de-burr the edges of the part||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
|Setting up tools||
||The defaults are usually unsuitable so users must be able to make their own libraries|
|Telling Fusion what tools to use|
|Picking the rest of the tools||
||Getting all the tools set up|
|Choosing the order of operations||
and the decking off can happen anywhere before #3 but for convenience we'll do it first of all
|Need to choose the order of operations such that it's possible to machine easily|
Setting up tool paths
|Types of tool path||
||There are loads, users need to be aware of them|
Stock preparation is needed as you can't normally get stock the exact size you want
|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. This gives you a chance to check that the run-time for your toolpath isn't excessively long. Because of thermal limits the boxford can run programs up to a maximum of 1 hour long, after that it needs some cool-down time, generally around another hour, before it can operate safely again.
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|
||Setting up a first toolpath|
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
This new tool path should open in edit mode. 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.
On the heights tab, select "Drill Tip Through Bottom" as we want the drill to pass all the way through the work
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.
|Introduction to some of the basic milling options|
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
|Deburring is a useful safety measure|
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 https://help.autodesk.com/view/fusion360/ENU/courses/AP-TOOL-LIBRARY 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.
This second session will be 1-to-1
Safety and Start-up proceedure
||Keeping people safe!|
||Keeping the Boxford safe!|
|Setting up the machine||
||Getting the machine set up and ready to begin work.|
|Activating the CNC system||
||Basic operation of the CNC system|
Work and Tool setup
||Material needs to be fixed securely both for safety and to get good results.|
||Proper tool holding is essential to avoid breakages|
||The CNC machine needs to know the relative positions of its self and the work|
Generating, loading and running G-Code
|Generating your G-code||
||Getting the machining operation from Fusion onto the Boxford|
|Setting up the air-blast||
||Why the air blast is needed, what it does, how to set it up|
||A vital test to make sure you've not made a programming error.|
|Running the program||
||Making your first cut and what to watch out for.|
||Changing to new tools so that users can run a multi-path job|
Dealing with any problems, shutdown and clean-up
|Recovering from E-stop||
|Finishing and cleaning up||
||Leaving the machine in a fit state for the next person|