The CNC Milling machine is a versatile and powerful tool to have in Maker space. It can work with multiple materials, wood, metal and plastics for both large and small projects.
– This is what you will need the knowledge and skills for
After reading this module, you’ll understand how a CNC milling machine works and how to turn a computer design into a finished piece.
Overview of learning objectives and competences
In this module, you’ll learn how to set up the machine, the software, start a job and how to post-process the finished pieces. You’ll also learn how to work safely around this kind of machine and be able to maintain the machine.
Required skills for this module
Basic computer skills and 2D conception skills learnt in module 4: 2D Conception (CAD)
What is a CNC machine?
In this part you’ll learn what a CNC machine is, what it is used for, the different types of CNC machines and how they work.
What is a CNC machine?
CNC milling, or computer numerical control milling, is a machining process which employs computerized controls and rotating multi-point cutting tools to progressively remove material from the workpiece and produce a custom-designed part or product.
Several methods are available under the general term CNC machining services, including mechanical, chemical, electrical, and thermal processes. CNC milling is a mechanical machining process along with drilling, turning, and a variety of other machining processes, meaning that material is removed from the workpiece via mechanical means, such as the actions of the milling machine’s cutting tools.
What this Module will focus on is a mechanical drill as a means of removing the material. This is in simple terms a drill attached to a table set to move in at least three directions, called the XYZ axis. Depth, width and height. The drill removes the material that is not wanted and at the end of the milling job we are left with the object we designed.
The XYZ axis refers to the length, depth, and height of the total work area. Traditionally and somewhat confusingly the X and Y axis can denote either length or depth. You have to check that in any individual machine of software you are working on.
The Z axis refers to the height of the work area. For example a machine with an XY axis of 500 mm and an Z axis of 200mm will be able to create an item half a meter on either side and a height of 20 centimeters. The maximum cutting area is different for each machine. The machine manufacturer will have those specifications available.
The CNC milling process utilizes computerized controls to operate and manipulate machine tools which cut and shape stock material. In addition, the process follows the same basic production stages which all CNC machining processes do. Taking or making a CAD file, converting it to a format applicable to the specific CNC machine, getting the machine ready and executing the milling job.
Milling is very fun and can help you create a number of helpful and exciting things, some examples are shown below.
This part will teach you the security precautions to take with a CNC machine.
As was mentioned in the introduction, not all CNC machines are the same. The examples given here are all focused on a Shopbot Desktop CNC machine. Just be aware that even if things might look different there are some universal commonalities in most of the CNC machines.
This big red button should be part of any large machine that has moving parts. It should only be used for emergencies. Stopping a job in progress is almost always better accomplished by some other means, either in the operating system or on the machine. This is as stated earlier only for emergencies.
This model CNC machine is a desktop version and does not have a large workspace so an enclosure could be bought from the manufacturer for it. This enclosure is connected to the machine so that if the doors open it will automatically stop the job and the job will not start unless the doors are closed. This serves a second vital role of reducing the noise and dust that is produced from the machine.
A machine of this type will produce a lot of noise and dust. They will often have a vacuum machine or ventilation system running along with it which increases the noise.
Safety measures for the operator of such a machine:
- Use ear protections at all times when everything is running.
- Wearing protective gloves is also a good idea since there are many opportunities of cutting oneself on the drill bits or getting splinters from the wood or aluminum material.
- Before starting a job, be aware of the location of the nearest first aid kit.
Setting up the Job
This part will teach you to use the design software, the output software and making a job to use on the CNC machine.
- Opening a Vector file or 3d file in a 2d carving software, in this case Vcarve.
- Creating the material and placing the job on the material in the software.
- Assigning operations/cut paths and selecting correct drill bits to individual parts of the design.
- Exporting the operations/cut paths into a file format that the CNC machine software can understand.
1. Opening a Vector file or 3d file in a 2d carving software, in this case Vcarve.
First, we open our carving software – in this case we use Vcarve, as this software is supplied with the Shopbot. This software provides basic operations that the use of this software can also be applied to the basics of other software and thus the fundamental concepts of CNC milling can be learned.
Vcarve is also great for designing jobs completely. Drawing up all the vectors and everything. That is rare, usually you design something in one software and then transport it to a milling, printing, or carving software.
In this example we did create the design in Inkscape and porting it over to Vcarve is one of the steps that we teach. That file format is an .SVG format
2. Creating the material and placing the job on the material in the software.
First after starting Vcarve you have several options. Let’s start by starting a new Job. Then you are asked to define your material, here you select what type of material you are carving out of. The size of the material, length, depth and height, on the X, Y, Z axis(according to the milling machine you will be using for carrying out the job at a later point). You also select where zero is on the z axis, at the top or bottom of the material, to help you with setting the 0.0 later when measuring it on the material. Then you select where 0.0 is on the X and Y axis, to help you orient the material in the program and on the material later. This is to see where you are starting from on the job.. What the Axis are and how they work will be covered in part 4: Setting up the Machine. After you have done all this you click “ok”.
Your left side panel will change to the drawing panel. It is here that you can edit an already created design or in fact create a job from start to finish. It is not necessary for this tutorial as I had already made the design in Inkscape, a personal preference. But having the option to change individual parts of the job is always handy. Moving something around or changing the layout of the job without having to switch to a different software.
3. Assigning operations/cut paths to individual parts of the design.
Now let’s look at this simple pattern in the picture below. It is a cheese platter that was made to demonstrate different cuts and drill bits.
In this job we need to make a pocket cut, a type of cut that creates a pocket in the material. Of the four objects in the middle of the circle. Then we need to chamfer off the edge of the circle and then finally cut out the object with a straight cut that goes all the way through the material. With any cut we start by selecting the lines that we want to assign an action to. We can select multiple lines or objects by holding shift and clicking on them one at a time or holding down the left mouse button and dragging the mouse over the lines. When we have selected the lines then we look to the right of the screen and start setting the toolpaths.
In the picture above you see the Toolpath Operations. The first two are the Profile and the Pocket toolpaths and you do most of your milling with these toolpaths. Profiles are used to cut lines into the material and Pockets are used to remove all the material inside the object you select. Therefore, a Pocket toolpath cannot be open ended; it must loop back on itself and close up. Let’s start with the first path, we select the four objects in the middle of the circle and open up the toolpath menu.
Now we go over the settings one by one for this toolpath and for this job in particular.
Cutting depth: This simply sets at what depth to start cutting and at what depth to stop cutting. This is not affected by where you set your Z height, at the top of the material or the machine bed. The cut will always start from the top. Look at the small illustration on the left that shows the (D) and (C) for clarification.
Tool: The type of drill bit you use affects the type of cut you make, and changes drastically based on the bit. We are only going to go over these three most common types of bits here. The flat drill, ball nose, and V bit. As you can see the cuts that each bit makes on the wood are fairly different.
For this pocket cut we are making we could use all three bits and get similar results. I have selected the Ball Nose as that will give the edge of the pockets a nice smooth curve from the top of the material to the bottom of the pocket. A flat bit will leave sharp corners and while a V bit will give us a slope down from the top to the bottom it will also take a much longer time clearing the material out.
The types of drill bits and feeds and speeds for your project will be covered in Chapter 6 of this module.
Use Larger Area Clearance Tool: Here you would perhaps replace a smaller more detailed drill bit with one that can clear out a larger surface. Fewer passes over the material means less time. This does call for a change of drill bits and might affect the job negatively. In this job, if I select a large flat drill bit as the clearance tool it will carve out the material, but it will also ruin the edge of the pocket making the corners sharp, something we are trying to avoid in this job so we will simply take a bit longer and use one drill bit for this operation.
Clear Pocket: Here you select what type of cut the pocket is cleared out with. Both offset and raster are good, and the type depends on the object being cut. For instance, it is bad to cut against the grain of plywood since that will cause greater splitting and splintering. Climb and conventional is simply clockwise for counterclockwise.
Ramp Plunge Moves: This sets the drill bit to move gradually down into the material. Plunging the drill straight down and then moving sideways is not good for the longevity of your bit, or the surface of your material. It is not set here as the depth of the cut is simply 5 millimeters and the drill bit can easily handle that without any ill effects.
At this point you are ready to calculate the toolpath and save it. It is a good practice to name the toolpath something descriptive and helpful. For instance, the type and size of the drill bit and the cut being generated. Ball_Nose_Four_pockets, for the example we are using here.
Then you calculate the toolpath and are presented with a preview of your path. In the picture below the red lines are travel lines and the blue lines are cutting lines. As can be seen there are two blue overlapping paths on the cutting area. That shows that we are passing twice over the material to cut everything out. We set this in the number of passes section of the toolpath. So each passing blue line represents the drill bit moving over the material cutting away. The number of passes is set in the Tool part of Toolpath Operations.
Next we would select the outer circle line of our design and create a groove into the line so that the edge of the platter is smooth and sloping. We will use a Profile Toolpath for this. Let’s go over the picture on the left one setting at a time.
Cutting Depth is simply setting from what depth, and to what depth to cut. As shown in the illustration on the left It is possible that you don’t start a toolpath on the set surface of the material. For instance, let’s say I want to draw a simple illustration of a piece of cheese at the bottom of the pocket we just made. Then I would set the (D) of the cut at 5 millimeters and the (C) at around 7 millimeters. By setting (D) at 5, the drill moves down 5 millimeters below the surface of the object and then starts cutting. Until it reaches 7 millimeters of cut depth. This is so the drill doesn’t start drilling at 0 millimeter depth and drills through empty air. Remember there is nothing there because we just removed it in the previous pocket cut. Due to its shape a V-bit is meant to carve onto the surface usually, not to cut through it or clear out material. So we set the depth to around 2 millimeters.
Tool: We go into the tool library and select a V-bit. It will make the right type of cut into the material we want. We will look into the tool library a little later in chapter six. The number of passes depends on the tool and how deep we want to cut into the material. Since we are making a shallow cut 1-2 passes should be enough. The calculation for this is explained in chapter six.
Machine vector sets up where the bit follows the vector it is machining. Here we set it On the vector. This means that half of the cut is on either side of the vector line. So a 6 millimeter bit will have 3 mm on either side of the line. When we make the last toolpath, the one that cuts the object out of the material we will set that cut up so it will be on the Outside of the vector. Carving half of the earlier V-bit cut away and leaving us with a sloping edge.
Tabs set up a small connection between the object and the material it is being cut out of and can be removed after the operation with a knife or chisel. This prevents the object from being cut free completely and moving about which causes problems while cutting.
The last toolpath is the same vector as the last one. The outside circle. What we change is the type of drill bit we are using. Instead of a V-bit we would use a flat bit to separate the material completely. Leaving only the small tabs to secure its place.
Here the Cutting Depth is important, it has to be at least the same as the thickness of the material, and usually a little more, since the thickness of most softer material is never one hundred percent uniform. The material is 20 millimeters thick, so we set the depth a little more and cut down to 20.5 millimeters. This will cut through the material in all places and cut into the spoil board, which is fine as that is what it is for. Be aware when you save this tooltip the following warning will pop up telling you that you are cutting through the material. Just make sure that’s your intention and that you have not accidentally set the decimal point in the wrong place. It happens to everyone eventually.
Additionally, we set the Machine vector on the Outside of the line, carving half of the earlier V-bit cut away and leaving us with a sloping edge.
Lastly the Ramp, Leads, Order, Start At, and Corners are minor self-explanatory settings to the job. The Ramp is if you don’t want the drill to plunge straight into the material. Leads are to set the toolpath, so the cut leads into the line. Order is organizing in what order the cuts are done. Start at sets the starting points of the cuts and adjusts corners whether you have soft rounded corners or sharp corners.
Now we are ready with something like this:
4. Exporting the operations/cut paths into a file format that the CNC machine software can understand.
Previewing all the toolpaths gives us the opportunity to go through and check that everything looks as it should and that we are ready to save our toolpaths and export them to the format that works with your machine. The machine manufacturer will provide that information with the machine. On the right side of the screen, we see the toolpath save window. It is possible to either save it all as one big file or three different files. Many small files give you more control over for instance the order of the cuts and the timing. One big file is good if you just want to start a job and run it all the way through. You can see that I named them after the drill bits or their function. This way it is easy to see at a glance what a particular file is. In either case you will have to do a Drill bit change before and between all the operations as this job calls for three cuts and three different drill bits. If you save everything as one file, then the machine will pause after each part of the operation and walk you through a tool change. Also note that the order of the toolpaths matters as the job will be performed in order from top to bottom. Leaving cutting out until the end is considered best practice.
At this point you will have a file that works with your machine. That is ready to load into your machine so next we should get the machine ready so that we can start cutting.
Setting up the Machine
This part will teach you to start up the machine, affix material to the workplane, run the setup for the machine, install the design and start the job.
First of all, I will mention that we are using a Shopbot desktop version with its default software. All the examples in this chapter and in most of this module will refer to it. There are many different types of machines and software. They may have small differences, but they often share enough similar settings and traits that having learned one will help you operate a different machine or software.
A lot of steps go into
Starting up the machine
- Check the safeties, make sure that the dead switch is not active and that other automatic safety precautions like the doors on the enclosure are in the right position.
- Turn on the machine. This is usually a straightforward step, if you have followed step one.
- Start the computer and the relevant software, almost everything regarding the operation of the machine will happen on the computer. Aside from turning it on and off, all commands and setting adjustments are done on the computer in the Shopbot software.
- Run a warmup routine(as shown on the picture below). It is best to start with this as it can take a few minutes. In the case of the Shopbot it takes 10 minutes. This action is taken to slowly start the drill and spindle. It is not good practice to start a job at a high or fast revolutions from a machine that has been turned off for any amount of time.
- Check the work area from your previous job. If someone else was using the machine, make sure that everything is as it should be. For example, no one left their ear protection in a place where it would block the movement of the Y axis.
- Clear the surface of any detritus, again the last person using the machine should have cleaned up after themselves but sometimes it is better to give an extra brush of the build plate as a small splinter or a discarded screw can tilt the material when you affix it to the build plate.
- Affix the material to the work area. There are a number of ways to affix your material to the build plate. The purpose of this is to simply hold the material down so that it does not shift or move with the drill when it starts carving into the material. Three common ways are:
- Screwing in directly. Simply grab a drill and fasten two or more screws to the material and stick it to the build plate.Make sure that the screws are not anywhere near where you will later start cutting the material with your job. This is a quick but dirty way of fastening your material and will damage the build plate over time with repeated holes forming in the build plate.
- Drilling holes in the material to place studs. This is a really good way if your material is routinely the same size. Simply drill two or more holes into the material. Drill the same number of holes in the equivalent places in the build plate. Place a wooden dowel into the holes in the build plate. Then place the material on the dowels and slide the material to the surface of the build plate. Since there is no downward force on the material you have to make sure that your build plate is clear of anything that can vary the Z height of your material.
- Clamping the material down. Like screwing into the material this is a quick way to affix the material. Simply get the appropriate clamps, slide them into the grill under the build plate and clamp the material down.
- Replacing the tool bit if needed. There are a bunch of different drill bits that can be used for jobs using a CNC machine. I will go over them in more detail in chapter 6. A job can often use more than one type of drill bit calling for tool changes both in the beginning of a job and in the middle of it. Additionally, when you change the drill bit in the middle of the job you will have to set zero on the Z axis again, as it is VERY unlikely that you placed the new drill bit at the exact same depth as the previous bit. In any case when changing the drill bit you have to first open the enclosure and loosen the clamp holding the collet that the drill bit is inserted in. After loosening the fastening, remove the drill and insert the new drill. Then tighten the screw on the collet again. Be careful not to over tighten the screw. Tighten it firmly but not too tightly. You can damage the collet if you tighten it too much.
Running the setup
- Zero the X,Y axis: Let’s start with the X and Y axis. Giving the command in the software the machine physically moves as far as it can to the zero point on both axes. The zero point on the Shopbot is the left and closest corner to the front of the machine.
- NOTE: Setting the Z axis is next, but it is not done until after we affix the material to the work surface (at least on this machine). This is because a CNC machine removes material during the manufacturing process to produce the object as opposed to a 3D printer which adds material to a part until the object is finished. In those cases, the Z axis starts at zero and goes up. In the CNC machine the Z axis starts at zero and goes down. So, the zero point on a Z axis is the top of the material that is being worked. Then the drill moves down into the material cutting out everything that is not part of the object
- Set the Z axis using a sensor: To set the Z axis you use a sensor that uses an electric charge to get a detailed measurement of where the top of the material is. When the command is given the drill lowers slowly until it touches the plate and an electric circuit is generated. The drill stops there and then repeats the process to double check the measurement. You can also measure the Z axis on the build plate directly but only if the software is set up to carve up from zero. Remember that you only zero the z axis after you have affixed your material to the build plate.
Installing the Design
Move the file from the design software to the control program using a USB memory stick or whatever method you use to move files around in your system. Then you go to the Shopbot software and go to File and Part Load File. The software will guide you through this process with checks that everything is in the right place and that you have already zeroed all the axes. Everything should be ready at this point so starting the job should be fine. Monitoring the job is a must and your machine should not be left unattended. By this time, you should have put on your hearing protection and switched on the hoover to reduce the amount of dust and chips that are created as a side effect of the work. Now just wait for the job to finish.
Now that the job is finished you have a bunch of options on what to do with the finished object.
Removing the material from the machine: How this is done depends on which of the methods you used to fasten the material to the spoil board. After you have removed the material, you should clean the Shopbot and vacuum up all sawdust and material residues. It is a good idea to remove the drill bits from the machine and store them in their proper place.
The material will most likely need some work. Remove the tabs that hold the pieces to the material with a knife or chisel. These areas will most likely need sanding. The piece that you have in your hand now is most likely in a rough state. Post processing work will be needed to finish the job. Sanding the objects is almost always required. The drill bit can create splintering around the cut areas and going over it with sandpaper of different grit to smooth out the area is a must.
The options for what to do next are almost endless; is this a multi part project that needs multiple operations for many different pieces? Do you need to assemble the objects into a working whole? Plastics might need sealing with heat or some primer spray. Wood takes staining, painting and finishing. Whatever it is that you have decided to do for your design, the CNC milling is just a step in the journey of making something, a tool that will expand how you can create useful and fun objects.
Here we look at the types of drill bits most commonly used in CNC milling and how to set the speeds and feeds for those bits depending on the material being cut
First, we need to distinguish between drill bits and milling bits. So far, we have always referred to these as drill bits. There are however at least two main types of CNC router bits.
Drill bits: These drive into the material. They are the best choice for tasks that require material to be removed straight down through the workpiece. They are often used for pre-drilling holes for screws.
Milling bits (or cutters, carving bits, and end mills): These cut sideways across your material. They are designed to move across the surface of the workpiece, clearing away material so the object can gain 3D parts. Even though bits fall into these two main categories, other variables are always at play, flute type, number of flutes, and what type of shape is at the end of the bit, fishtail, engraving, V-bit, and ball nose.
There are also speciality bits, which have more sophisticated profiles for all manner of specialized applications. For example, boring bits, miter fold bits, round-over bits, and “veining” bits.
Next we should talk about some terms used to describe the bits.
A flute is the cutting edge of a bit. Having more flutes increases the strength of the tool, and it means you can have a faster feed rate, but it reduces space for chip flow. Thus, bits with more flutes tend to leave a smoother cut surface and require a faster feed rate to avoid burning. CNC router bits are mostly available in one, two, and three flute configurations. Generally, bits with fewer flutes remove more material per cut and require a slower feed rate.
Straight flute: A straight flute design means the cutting edge is parallel to the body of the bit. With this design, the material will not be extracted from the cut. A straight flute is cheaper to make and is mostly for wood and plastic materials. A straight flute produces a clean finish.
Spiral flute: A spiral flute is cut in a helix around the body (or shank) of the bit, making them ideal for wood, aluminum, and plastics. The up-spiral flute, for example, is useful for removing chips. There are three types of spiral bits: up cut, down cut, and compression. Their naming is to describe where the chips and material are pushed during the cut. So, an up cut spiral bit will push the material up and out of the material. They are preferable for cutting through the material. Down cut pushes the chips down as it cuts and is better for preserving the top of the material being cut. Compression cut is a mix of both and will leave both the top and bottom of the material looking good.
Feed rate: How fast a bit can move laterally through the material. If the chips that are coming from your cutting are unnecessarily large, reduce the feed rate or you may end up ruining the bit.
Speed rate: The speed of the spindle. It’s represented in revolutions per minute (RPM). Speed and thus feed rate will depend on the horsepower of the spindle. While a high RPM will generally result in a higher quality finish, it can also result in higher friction that will, in turn, increase the wear on your bit.
Higher RPM produces smaller chips, while higher feed rates produce larger chips. Overall, if the chips are too large, your bit will be likely to break, but if your chips are too small (like fine powder), you will be dulling your bit. It’s all about getting the right balance.
Feeds and Speeds
To calculate the feed, the relative linear speed between the tool and the workpiece, you need the speed RPM on the machine, the number of flutes on the bit, the material being used for the job, and the size of the bit. The equation for the feed rate is:
Feed Rate = RPM * chip load * number of teeth
RPM is the speed of the rotating element (either the tool or the workpiece)
chip load is the amount of workpiece material removed per revolution per cutting edge
number of teeth is the number of cutting edges the tool has, also known as the number of flutes
The chip load depends on the characteristics of the tool and of the workpiece material. For example a tool drilling a hole into a soft workpiece material will have a higher chip load than a harder workpiece material.
This is not a simple formula and thankfully many manufacturers of drill bits have a feeds and speeds calculator available online. Also suggested speeds and feeds are included in catalogs that come with the purchase of the software. Some research online is recommended here if you are not using the default settings that are suggested by the software or drill bit manufacturer.
Here we have the profile for the V-bit we used in the sample job earlier in this document. This is when we were selecting the right bit in the Tool section of chapter 3. These are the details that come up:
Here you can see the speeds (RPM), feed rate and plunge rate of the bit in question. These settings are in the software by default and using them at the outset is strongly recommended. It is here where you would add new bits to your tool library. A detailed description of your bit should be included by the manufacturer so that you can save it accurately here.