UNSW Making

CNC Router Basics

Everything you need to know about flat-bed CNC router machining!

For this learning module, you will need:

  • A Computer with Fusion360
  • Sufficient knowledge of a relevant CAD program
  • A Fusion 360 (or Autodesk) account
  • The burning desire to make cool things

Getting Started


The Basics

What even is CNC?

CNC stands for 'Computer Numerical Control'… if you have the urge to know more... keep reading. If that makes sense to you... Skip ahead!

CNC refers to the ability to move and manipulate various tools in 2-5 axis of motion using digital instructions. 3D printers, laser cutters, even soft drink vending machines rely on CNC systems, however when we use the term CNC we are mostly commonly referring to cases where a manual (NOT computer numerically controlled) version of a tool or process exists to compare it to. Examples include CNC routers, mills and plasma cutters. These types of CNC's are almost exclusively for subtractive manufacturing, where you take (cut) material away to make an object.

CNC Workflow-03.png
Meet the Family - CNC

Tormach PCNC Mills

The Tormach PCNC 1100 (dfl) and 770 (eng) are versatile CNC mills designed for individual users and small production spaces. They are lower in power than industrial CNC mills but have all the features, such as an enclosure, controller, accessories, and fixturing options allowing us to do precise milling to make complex small parts out of plastics and metals, including alluminium and mild steel.

Multicam CNC Routers

Our Multicam routers are large scale table routers commonly used to cut wooden and composite metal panels for the construction industry. They are powerful and large, but do not have the versatility and rigidity of a Mill, with limited fixturing, accessories and controller. With that in mind they are excellent for carving plywood, timbers and foams to make larger scale models, furniture, and full scale components for theatrical sets and architectural projects.

CNC anatomy v2-01.png

Gantries / Linear Axis

Gantries are the Linear movement system of a CNC. They either move the spindle, the workpiece, or a combination in 3D space to produce the complex, accurate outcomes we require. Commonly on CNC’s the first 3 Axis of movement are linear Axis.

On our Tormachs, the X and Y Gantries holds the workpiece and moves it left, right, back and forth at a fixed height. The Z Gantry holds the Spindle, moving it up and down. This configuration allows for more stability and accuracy but limits the working size.

On our Multicam, The X, Y and Z gantries hold the spindle so that it moves in all directions. The workpeice remains fixed to the bed. This allows for a greater range of movement (and larger work pieces).


This is the motor powering the cutting tool on the CNC. The spindle spins the cutting tool at an approximate range of 100 - 24000 RPM in order to remove material and mill the object.


The controller most commonly takes the form of a computer, or hand held control pad. This is used to execute the functions of the machine. It is the Human User Interface of the CNC.

Dust Extraction / Chip Evacuation

Dust extraction is used to remove loose excess material (chip) created during the milling process. This chip must be removed to create a clear and safe workspace and allow for the precise cutting of the object.

Flood Coolant Pump

The flood coolant pump is used to supply the cutting area of the CNC with coolant to help with the proper removal of chip and prevent the tool from breaking by overheating, or by hot chips re-welding to the tool. It is used when milling metals and some plastics.

Air Supply

Many CNC’s (including all of ours) require compressed air to facilitate functions on the CNC. On our CNC’s the tool changers and our Mist accessories both require compressed air.

Workpiece (Stock)

The workpiece, or stock, is the piece of material used make the object. It needs to be prepared with flat edges and fixed securely to the CNC bed, this is called fixing or workpiece hold down.

Below are some common accessories used for Workpiece hold down.

Fixturing Table

A fixturing table is a level surface with holes or slots that allows various jigs and accessories to be attached to.

Vacuum Bed

Common on table routers, vacuum beds use vacuum pressure to hold down a workpiece. For a vacuum table to work, the material needs to have a very flat surface to make maximum contact with the table, and it must be completely free of dust and anything that can cause a leak.


A wasteboard is a sacraficial piece of material to which the workpeice is fixed using screws. This is often used in combination with a vacuum bed.


Similar to vice, a chuck commonly has 3 or 4 Jaws which move radially, making them ideal for fixing circular workpeices to the CNC for machining.

Coolant Mister

A coolant mister mixes compressed air and coolant together to provide a jet of mist used in similar applications as the coolant pump. The smaller amount of coolant released is easier to keep clean, whilst the jet of compressed air can be used to blow excess chip clear of the tool.

Tool Holder, Collet and Collet Nut

The collet is what holds the cutting tool in the spindle, simliar to the chuck of a drill. The tool is inserted into the collet and tightened with a collet nut. Our CNC’s are equipped with air assisted tool holders so we can keep a library of pre-measured tools in collets that can be quickly and safely interchanged when needed.

Tool (Cutters, end mills, drills etc.)

Tools make direct contact with the workpiece and remove material to mill out the object. See the 'tools' section to learn more about the different types of tools we use!

UPADTED CNC Tool Guide-05.png

Module 1


All About Tools

End Mills vs. Drill Bits

Whilst they might look very similar, end mills and drill bits perform quite different functions. Drill bits are designed to plunge directly into the material to create cylindrical holes whilst end mills are designed to cut sideways. End mills have sharp cutting edges known as flutes that run down the tool, these flutes cut more efficiently when gradually ramping (sideways) down into the material rathen than plunging vertically.

CNC Endmills no title-04.png

End Mills

End mills come in a variety of shapes and sizes and it very important you choose the right end mill for the job you are doing! The type of material, the shape of the object and it's end use all play a part in determining which end mill should be used. Read on to find out all the things to consider when choosing an end mill!

Endmill End types

  • Flat end mills are used for clearing and finishing horizontal and verticals surfaces. These are the most common tools used on the CNC at UNSW
  • Bullnose end mills have a flat end, with a corner radius. Bull nose end mills tend to last longer than flat end mills and can be used to finish flat and verticals walls. Bullnose end mills however leave internal radii on all edges.
  • Ball end mills have a spherical end and are used for surfacing complex shapes. Whilst useful for curved surfaces, they leave peaks when used on flat surfaces.
  • Chamfer end mills have a V shape and commonly come in 90 and 60 degree angles. They are used to create sharp edges, cut mitres, and engrave fine detiails.
CNC Endmills-01.png
CNC Endmills-02.png

Endmill Flute Features

Flutes are the cutting surface of an end mill. These deep spiralled grooves allow for chip formation and excavation assiting in the cutting of the material. The number of flutes on an end mill determines chip size and surface finish. More flutes equals better surface finish, but means the tool runs at a higher heat and isn't suitable for all materials. Fewer flutes means greater chip size and more clearing capacity.

Helix Angle

Flutes with a higher helix angle pull the chip out more aggressively, which is useful for materials where chip removal is crucial (e.g. metals). For softer materials like wood, a lower helix angle (or a straight fluted tool) can produce a nicer edge finish.

Flute cutting direction

Flute cutting direction determines the movement of chip. You can visually identify the cutting direction by spinning the end mill clockwise and noting the direction in which the flutes move. When cutting wood, the edge opposing the chip direction will have the better finish.

  • Up cutters push chip upwards out of the way of the tool and the fixturing table.
  • Down cutters push the chip downwards putting less strain on the workpiece but can cause build up of chip.
  • Compression cutters combine both cutting directions, resulting in clean edges on the top and bottom edges, but given the complicated geometry are only used for specific applications. We generally use compressions cutters for plywood.
  • Strait cutters have no helix, no cutting direction and push the chips sideways. These are generally used for plastics.

End Mill Rules and Considerations

End Mill Size

The length and diameter of an end mill dictates the depth and detail that can be achieved. These factors can also effect the speed of a project. The larger the end mill the more material it will remove, and the less details it can acheive. The smaller the end mill, the less material it can remove (making it slower) and the more details it can cut.

  • Tool stickout (end mill length below holder) limits the total height of features that can be cut with the tool.
  • Flute length limits the depth of a single cut. If the tool engages material deeper than the flute length the shaft of the tool will colide with the material.
  • Tool diameter (in addition to limiting detail) is used as an indicator of the overall strength of a tool. We usually cannot cut into material deeper than 3 x the tool diameter without risk of snapping.

CNC Endmills-03.png

Internal Radii

Because all end mills are spinning cutters, they leave fillets equal to the radius of the tool on the internal corners of the object. Bull nose end mills will also leave a fillet on the bottom edges. Sharp internal corners cannot be achieved! This becomes very important when trying to make joinery, or complementary parts that fit together.

Maximum End Mill Engagement When Clearing

If an end mill is pushed into material too quickly, the load will be too high and the tool will break. Inversely, cutting too slowly causes grinding, friction, excess heat and heightened wearing of the tool. Ideally, the load on the tool should be constant and configured carefully.

When clearing, to avoid the tool breaking, we need to used slow, gradual passes that step down and over (radially) to cut the material.

It takes practice and experience to properly configure the end mill engagement when clearing. For more info you can refer to our templates and resources. You can also have a go at this formula:

The depth of axial engagement (depth of cut) of the tool multiplied by the width of radial engagement (step over, optimal load) gives us the cross sectional removal area of the cut. For Aluminium that area should be 20% of the size of the tool’s engaged cross section (the part of the tool engaged in the material), for plywood it can be 50%, for XPS foam, 100%.

Maximising Axial/Radial Engagement when Finishing

The quality and accuracy of a part will be greatly effected by how the tool interacts with the surface when finishing.

For the best verticals finishes, use the most of the flute length available, without engaging the end of the bit.

For finishing and facing horizontal surfaces have maximum engagement with the end of the tool.

For facing, avoid making contact with the centre of the tool and maximize the surface speed.

Using Dogbones v1-02.png

Types of End Mills

Select the right end mill for the job!

CNC Site Models-02.png

Further Your End Mill Knowledge

The Skinny on End Mills

This article from Make magazine focuses on the basics. Worth a read!


CNC Production Routing Guide

The best way to learn about tools, feeds and speeds is by experiencing it yourself whilst operating a cnc. Start with presets, templates then get a feel for it. In the meantime, Onsrud (a tool maker) made a great PDF about it. Click through and check out some of these headings:

  • Router bit anatomy
  • Cutting tool geometry
  • Tool material strengths & weaknesses
  • how to adjust real world critical variables affecting tool life
  • The dulling process of carbide
  • Feeds & speeds

Module 2


Brush Up On Your CAD Skills!

New to CAD? Learn some skills!

CNC Tool Guide-07.png

Check out our home made series on CAD for a general introduction to fusion. This is great if you want to learn the very basics of CAD, and expand in all directions in the future.

CAD learning modules
CNC Tool Guide-06.png

Our operators in the AML also made this handy list of CAD tutorials that focus more on learning CAD with a eye towards CAM and subtractive processes.

AML guide to CAD in Fusion 360

Already made your CAD file? Find out how to move across to CAM

Preparing files from other Software for Fusion 360 CAM

What files/models do I need to get started with CAM?

Depending on what you are making, you will need a mixture of 3D models and 2D Curves to properly generate your toolpath.

The 'Model'

The model, is the actual 2D or 3D representation of the thing you are trying to make. When you import it or open it in Fusion, it should be sized in millimeters, and at the exact scale you intend to produce it at.

Model File Tips

  • Solid models (imported as a STEP file) work best as they have defined edges and can be modified by Fusion most easily.
  • Nurbs based objects are next best (imported as a STEP or 3DM file) as they have the same defined edges, however cannot be edited in fusion
  • Whilst it is possble to import mesh based models (STL, OBJ, MAX, SKP), many additional processes will be required. If you can avoid using a mesh for CAM please do.
  • If what you are making is flat (2D, eg. shapes that need to be cut from a thin peice of plywood) a collection of 2D curves imported as a .DXF file or drawn directly in Fusion can act as your model.

✔️✔️ STEP, IGES, FDM: Solid Models, and designs made Fusion 360 are ideal

✔️ STL + DXF: meshes Combined with A 2D drawing for machining boundaries work too

✔️ DXF: 2D Shapes can be cut from a DXF file

STL = An STL mesh on its own is not enough, you will need to import a DXF for machining boundries

PDF= These files are full of extra data that gets in our way.

General Considerations

Always check your file for the following:

  1. 3D Models and 2D Curves should be scaled to the precise size of your final physical outcome in millimeters (mm)
  2. A corner at the boundary of your model/curves should be placed at the origin (0,0,0) of your workspace with the model placed in the positive quadrant.
  3. Models and curves should be aligned together (rather than sitting next to each other)
  4. Only relevant models and curves sitting within the stock boundary should be exported.
  5. Use layers to identify the different parts of your model and organize your 2D curves (roads, building pads, drilling holes, pockets, profiles etc.)

📏 mm

📐 (0,0,0)

✂️ Delete Scraps


Machining Boundries

Machining boundries define the areas on your model where your different toolpaths will be generated. Sometimes you will apply a toolpath your entire model, sometimes to a specific section where a certain strategy is needed.

Machining Boundry File Tips

  • DXF files are the only supported file format for importing machining boundries
  • Machining boundries are 2D regions, so you can use a 2D plan/projection
  • Organize (and import) your machining boundries in seperate layers to make selecting them easy
  • Make sure your boundries are trimmed closed curves.
  • If you have made your design as a solid model, you may not need to import machining boundries

'Stock Model' and 'Fixture Model'

A stock model is a 3D representation of your workpeice. A fixture model represents the mechanism you are using to hold your workpiece down. These are only required when:

  • your workpeice is NOT a rectiliniar prism or cylinader (they mostly are)
  • you are doing a 'flip mill' or 3+1 axis opperation

3D Models = Volumes

If you have a more complex project and a 3D model is required, consider the following:

Nurbs based models and Solids

Nurbs based and solid models are much better than mesh based models. We strongly suggest designing your model in Fusion 360, SolidWorks, Inventor or Rhino.

  1. Fusion 360 files can be shared directly with the operator
  2. Rhino, SolidWorks and Inventor models should be exported as .STP files


Whilst solid models are better, meshes can work. They will require the exporting of additional 2d machining boundaries (see below).

  1. Revit models and models made in mesh editors should be exported as a mesh (.STL)
  2. If you have imported a mesh from Revit or other program, but have opened it in Rhino to make some small revisions do not attempt to convert a mesh file into a nurbs object (the MeshtoNurbs command), make your changes in rhino and export the file as mesh (.STL)

2D Drawings = Machining Boundaries (Curves)

Curves can be used to send 2D shapes to the CNC to create profiles, pockets or drill down to specific depths.

When used in conjunction with a 3D model, curves are used to describe the different areas for which a different machining approach would be necessary. Whilst the 3D model is the ultimate shape we are cutting, the curves allow us to use different tool path strategies to move the tool across the surface. Below are some rules to take into account when preparing your 2D curves:

  1. Organize curves into separate layers based on the areas that they correspond to: Eg, ‘roads’, ‘building footprints’, ‘model boundary’
  2. Ensure curves are closed, and that no extraneous curves or duplicate curves are exported.

Module 3


All Things CAM

What is a Toolpath?

A toolpath is a collection of strategies or operations that direct the movement of the CNC across and through your material to reveal or cut out your shape. It is how we define our approach to cutting your project and there are many things to consider.

We make our toolapaths using Fusion 360. If you skipped over the CAD basics in Fusion 360 and have drawn your file in another CAD program, now is the time to jump across to Fusion!

Fusion 360 v2.jpg

Fusion 360 is a cloud-based integrated CAD, CAM and CAE software. It is free for students, educators and personal uses.

Download Fusion 360

LinkedIn Learning: Fusion 360 CAM

Available FREE for UNSW students, this course is ideal for those interested in preparing their designs for manufacturing on the CNC. They offer content from beginner to intermediate, well worth the look!

LinkedIn Learning: CAM in Fusion 360

Autodesk Fundamentals of Milling

From the creators of Fusion 360, this course is the best way to cover all things CAM for CNC milling.

Autodesk - CAM Fundamentals

Fusion 360 Cam Tutorial for CNC beginners

Whilst this video uses some different machines to the multicams at UNSW, its very approachable, and includes example models, and step by step versions of the tutorial.

Fusion 360 CAM tutorial for CNC beginners | How to

Fusion 360 Primer

This video comes from the makers of a few popular consumer level CNC kits, it provides a basic overview

Intro to Fusion 360 for CNC Users

Fusion Friday Series

Tones of fantastic Videos here presented in a casual way that focus on tips and tricks, ive chosen a very quick video looking at using a simple approach to tool pathing:

Fusion 360: CAM for Beginners! FF85 & FF102

Fusion 360: CAM for Beginners! FF85

Fusion 360 CAM Tutorial for Beginners! FF102

CNC Dummies for Routers

This is worth watching if your new to the basic concepts of CNC. It happens to use fusion 360 toward the end, but what it really provides is a broad overview of all aspects of CNC integrated fabrication.

CNC Dummies For Routers

So how did you go?

See how your CAM skills rate and assess your learning against the competancy checklist below!

How confidently can you;

  • Create, save and open your project in Fusion 360. Navigate the Fusion 360 browser to find your design, download and export an F3D file for sharing?
  • Navigate to the manufacturing tab in Fusion 360, create a setup, set the origin, select your model and size of your stock (workpiece)?
  • Load the Fusion 360 tool library and import the CNC basics tool library?
  • Import and load templates into your setup?
  • Edit the individual toolpath strategies to select machining boundaries, set heights and pass setting?
  • Create a clearing strategy?
  • Create a finishing strategy?
  • Simulate a toolpath, previewing the stock?


Module 3


All About Materials

CNC Materials-01.png

Choosing the right material for your project:

Material choice is an important part of the CNC process and will dictate some of the design choices you will need to make.

To find out more about what materials can be cut or what the specifications for these are, you can visit the DFL materials and pricing page.

  • If the material you want to cut is not listed on the page, you will need to provide an SDS (Saftey Data Sheet) and bring a sample to your tool-path consultation.
  • All materials must have a finished, flat, smooth face/s to fix to the CNC
  • Your material may need to be larger than your desired outcome in order to fix it to the CNC.

AML Material Guide DFL Shop

Preparing Materials for the CNC

Workpiece Hold Down

Using a Vacuum Table

Vacuum Tables generate hold-down force because of the difference between a vacuum under the part and atmospheric pressure pushing down from above. Every square inch of area exposed to that difference can have a force as much as 6.6kgs pushing down on it (the difference between 0 and sea level air pressure).

The hold-down force is proportional to that pressure difference and the surface area exposed, meaning that a larger work piece can have significant force holding them down whilst smaller pieced have much less force holding them down.

In order to maximise the hold down force on a smaller part, other areas of the vacuum bed can be 'blocked off' with a non-porous material such as plastic to help focus the vacuum on the other areas (see image adjacent).

Steps for using the vacuum table:

  1. Remove any dust, chips or debris from the MDF waste-board and the bottom of your material using the dust shoe attached to the CNC before placing your material on the bed. Debris and dust can cause an air-gap to form between the work pieces and the waste-board resulting in poor vacuum hold down.
  2. If your CNC has vacuum zones, close the valve on any zones your work-piece isn't covering. If you have large areas of waste-board exposed within the zone, use plastic sheets to cover the remaining area.
  3. Test the Vacuum by turning it on and performing a 'Push test'. You can check the vacuum pressure dial on the CNC, but given that different sized workpieces require different pulling forces, its best to test the suction by attempting to slide or push the work-piece yourself. If the vacuum hold down is sufficient, you shouldn't be able to move it.
  4. If you have tried the 'Push test' and you can still move the work-piece, you can attempt to improve the hold down by further isolating it using the following methods:
    1. Run the vacuum and note the current pressure on the vacuum pressure dial.
    2. Listen for a whistling sound around your workplace for leaks in your setup, this often occurs around gap between the material and the waste-board, or at the edges of the plastic sheet. It can also occur between the vacuum table and the waste-board itself.
    3. Use masking tape to seal off any cracks or possible air-leaks
    4. Check the the pressure dial to see if any improvement has been achieved, and do another 'Push test'.
  5. If you are still able to move your workplace after trying all of the above you will need to use an alternative hold-down approach.

Vacuum Hold Down CNC hold down-07.png

Using a Waste-board With Screws

In situations where your work piece cannot be securely held using the vacuum bed, you will need to use an alternate method of fixing. One of these alternative is using screws to secure the work piece to the waste-board.

If using screws to secure your work piece you will need to leave extra material around the perimeter of your design so that screws can be placed in the corners. There needs to be adequate clearance to ensure that the CNC bit will not hit any of the screws.

Thicker pieces of material (above 35mm) will require counterboring so that the screws can reach down into the waste-board. This is illustrated in the reference image below.

Hold Down with Screws
Using A wasteboard (with screws) v4_Page_1.png

Other Resources


Resources to enhance your CAD, CAM & CNC knowledge!

Get yourself trained!

If you want to learn and/or increase your skills in using the CNC machines don't hesitate to come and chat to a friendly Makerspace staff member. Make sure you complete the Badges that the UNSW Makerspace Network has for you!

Related Badges

Categories: Digital Fabrication
Tags: CNC