CNC Machined Mechanical Dial Using Fusion 360 Manufacturing

I'm a student at Imperial College London who loves workshops and machinery. Working within a group of 4 students, one of them had recently torn their ACL while rock climbing. This person was a highly athletic person who's 1 mistake will cause them months of recovery. While talking with physical therapists and orthopedic surgeons we realized that one of the most difficult parts about injury your ACL was staying motivated during the physical therapy phase after surgery. Staying motivated and consistent with the training speeds up the recovery process and improves it.

That is why we went through the process of designing a mechanism that keeps track of a users knee angle throughout the day while also being able to provide small amounts of resistance during physical therapy. Right after surgery, the user's knee will be very weak, so being able to provide small amount of variable resistance means that as the user's knee gets stronger and stronger, the resistance can continue to increase based on the recovery progress. The solution that we've designed is a machined dial casing that sits on a brushless DC motor with an encoder attached the the users knee. As your leg rotates, it spins the outer casing which spins the motor. As the motor spins, the encoder keeps track of the angle and and displays it on the integrated screen and in the future will be able to send it via bluetooth the the user's phone. It is important that we credit part of our inspiration which came from scottbez1 and his DIY haptic input knob as seen in this video. Please do check out the video, it is truly amazing!!

The purpose of this Instructable is to help with the design, prototyping, and fabrication of the machined dial component using Fusion 360 design workspace and manufacturing workspace. When I went out looking for resources on how I could start CNC milling components there was no easy to understand guide that I felt truly helped me.

If you do decide to create a dial like this and use this guide I highly recommend reading through the entire guide first as understanding some of the later processes will help you in the earlier ones as well. In addition it's necessary to supplement this guide with whatever CNC milling machine you use as each one can be slightly different.

Reusable Supplies:

• 5-axis CNC mill
• I am using a Pocket NC V2-10 which is a very small 5-axis CNC mill which I am fortunate to have access to through my university. I will go through this guide with context to this machine, however most of it should work with other CNC milling machines
• It is possible with a 3 axis mill but the stock (that is what the material before it has been milled into is called) will have to be taken out of the vice and realigned on its other side
• 6mm & 1mm Milling Bits for Aluminum
• Depending on the size and design of your stock, other size bits may work, however for the size of my dial, these are the 2 bits that are best sized, You want a bit as big as possible that will fit for your component as it means it can take away material much faster.
• Hacksaw
• The machined component is still attached to the stock once complete, so to separate them, a hacksaw is the easiest way
• Ruler/Measuring Tape/Calipers
• Needed for measuring out stock and placement on the vice. Having a pair of digital calipers is an incredibly useful tool
• File
• After using the saw to cut the piece off of the remaining stock, there will be sharp edges which is good to remove.
• 3D Printer (Optional)
• A very useful tool for prototyping design before final fabrication process

Consumible Supplies:

• Aluminum Stock Material
• I used aluminum 6061 which is the most common alloy to use in machining and is what was available for me.
• The size of the stock material will depend on how big of a dial you want to design, and also critically, how big of stock material can the milling vice handle. The Pocket NC V2-10 can only hold very small work pieces so it is very size limiting. For this project I used a 63.5mm x 38.1mm x 68mm piece of aluminum stock material. A few important things to not about size
• 1. if your vice can handle it, it's always better to get a larger stock material and remove material, because you can't add back material to the stock. Also important because the machined finish of the aluminum is much nicer than the factor finish, so it is best to remove material from all the surfaces
• 2. The factory cuts for the material can be quite off so don't expect it to be exact. I ordered my material to be 68mm and it came as 69mm.
• 3. Having additional size is also important because you need stock material to be able to hold the workpiece in place
• Dykem (Optional)
• Dykem is a type of blue ink used in metal working that when applied to the surface of the metal dries. This is an incredibly useful tool for marking measurements on the metal surface. You can apply the dykem then take a knife to draw your line or point.

The first step to machine the dial is to design the dial. Our dial went through an iterative design process where we interviewed potential consumers about their thoughts on the looks and ergonomics of the design which is how we settled on this curved shape. It's important that you pick a shape that suits your needs or desires but also that it is designed for manufacturing. It is important to think about when creating the design where a 3 or 5 axis milling machine would be able to create that. That means not having any impossible overhangs or places to reach. One method in addition to carefully thinking about the design is to use one of Fusion 360s many integrated features known as Accessibility Analysis. This tool in Fusion 360, will show you whether part of your design is accessible from a certain direction by indicating accessible in green and inaccessible in red. This functionality is especially useful for 3-axis CNC machines.

Another tip that I highly recommend when creating the CAD is to use parametric modeling. During my initial design, the dimension requirements for the dial kept changing which meant I kept on having to go back and change the sizes one by one. To greatly save time, it is useful to use something known as parametric modeling where instead of defining each length of a line by a specific number, you can assign it a variable with an equation and base that on other variables and equations. You can then define all of these variables in Fusion 360 under modify parameters in the modify tab in the design workspace. There you can write specific value and write equations to different variable names and give them specific units. Then when you go to dimension your part, instead of writing our the number you want, you can just write out the variable name. If that dimension needs to change in the future, you can just change the value in the modify parameters menu. If you want to learn more about that within Fusion 360 there is a very good guide here

A rough guide for the process of designing the dial can be seen in the screenshots above which are in chronological order!

Design Stages

1. Sketch 1: Create a 2d sketch of half of the dials profile.
2. Revolve: Use the revolve tool to revolve the initial sketch face around the central point to generate the initial dial shape
3. Sketch 2: Create a new sketch on the same place as the initial sketch. You want to create an offset of the outside of the dial which you can do by selecting the outside profile edge and clicking P. This creates a projection of that edge on the current sketch plane. Then using the offset tool, offset the line to any distance you desire based on how deep and wide you want your hand grooves to be.
4. Pipe: Use the pipe tool on the offset line you just create in the previous sketch, Change the diameter of that pipe based on how deep and wide you want your grooves to be. Make sure the operation is selected as cut so that it cuts into the dial. (Also make sure they aren't too deep or else it might effect the strength of the dial)
5. Circular Pattern: Create a circular pattern of the pipe feature you just created. To do this select circular pattern from under the create menu, and change object type to feature. To then select the feature look at the very bottom of Fusion 360 to where the timeline is located, and click on the pipe feature on that timeline. Create as many or as little grooves as you want!
6. Sketch 3: Create a sketch on the top dial surface in correct placement for your chosen motor. We are using a brushless DC gimbal motor which has 4 holes on the top in a square placement.
7. Extrude: Extrude the sketch you just made to create the 4 holes
8. Chamfer: Select the chamfer tool, and select the top edges of the 4 holes you just made. That chamfer distance should be equal to the size of the distance on a counter sunk bolt. The chamfers are so that sounter sunk bolts sit flat on the surface.
9. Sketch 4: This 4 sketch is done to create that flat surface sticking our from the dial. This surface provide a contact point to the part of the stock being held in the vice, and it also provides the connection point from the dial, to the leg attachment band.
10. Extrude 2: Extrude that sketch so that you have a rectangle like the one seen in the second-to-last photo. It is important that when you create this extrude, you change it from "join" to "new body" so that this rectangle is a separate body from the dial.
11. Sketch 5. Create a sketch on the top or bottom face of the new rectangle body that has just been extruded. Using the slot tool, create a slot on the rectangle on the outside of the dial. The purpose of this slot is to be a place where the connection arm from the leg to the dial can be attached to.
12. Extrude 3: Extrude the slot sketch you just created so that it cuts through the rectangle body
13. Split Body: Use the split body tool and select the rectangle as the body to split, and use the inside surface of the dial as the splitting surface. This will split that rectangle body into 2 pieces and once it is split you can delete the piece that remains on the inside.
14. Combine: Combine the dial and the remaining rectangular piece into 1 body.
15. Sketch 6: Create a sketch from the newly merged rectangle to create a flat base plate as seen in the final image. This is actually a really important step. Even though you will cut it off after it has been machined, this base plate allows the vice to grip it throughout the entire machining process and still be able to machine all the parts without having to take it out of the vice. My design has a U shaped cut in that plate because of the way the viceing system works which I will explain more the importance of in the next section.
16. Extrude 4: Extrude the sketch you just made so that the width and length are the same size as your stock.
17. Sketch 7. Create a sketch of your stock size in the correct positioning based on where you want your dial machined out of the material after having measured the stock material with calipers.
18. Extrude 5. Extrude the sketch you just made to the correct dimensions of your stock material and make sure you select new body instead of combine. After the extrude you should have a rectangular body that surrounds your entire dial. This is your stock material, you can hide the body by clicking the body and pressing V on your keyboard

After creating your design I HIGHLY RECOMMEND creating a 3d print of the model to see if you are happy with the shape and size. It is so much faster, easier, and cheaper to create 3D prints of the model, then going through the entire process of machining your component. This goes for any metal working project in my opinion. If you don't have a 3D printer, any sort of physical prototyping is incredibly useful whether its paper, cardboard, clay, foam, etc. Whatever you have is good just to get a general idea of your design not through a. computer screen.

It is important to note that this is not the only way to create a dial like this but just the way I found to do it!

The next step after creating the design is to set it up for machining. For the Pocket NC V2-10 they provide the vice system as a cad model so that you position your model correctly within the vice. Most larger and higher end CNC milling machines wont have you do this as this step is not necessary for machines that have probing functions. That means that the machine can figure out exactly where the stock material is within the machine, however with the Pocket NC, you have to position your stock inside the machine relative to where you position it in the CAD inside the vice.

It is now important to note that the U shaped cutout in the base section of the model that is meant to be held in the vice exists so that the milling bit is able to get under the entire dial while also not hitting the grub screws which vice the stock in place. Without the U shape, the 6mm milling bit is too large to go under the dial and machine it out so the U cutout in necessary. This could easily be removed in larger machine by just increasing the base material height, however the Pocket NC has a very small work area, so if I had increased the hight, then the tool wouldn't have been able to reach the very top of the dial.

Once you have positioned the dial within the vice (step not needed if your CNC machine has a probing feature) you can finally go to the Fusion 360 manufacturing workspace! If you click on the design in the top left, the click on manufacture you get the the new workspace. By default it should being you into the milling section, however at the very top bar you can see theres also a turning, additive, inspection, fabrication, and utilities section.

The next thing to do is in the browser tree on the left side, right click Setups and click New Setup. This will begin the process for the machining setup. This is a very important stage which will differ between different CNC mills and so I will discuss for the Pocket NC mill and try to talk about general info. In the setup menu there are 3 tabs, Setup, Stock, and Post Process. The first thing is to go to the setup tab and make sure the opperation is milling. The Work Coordinate System sounds confusing but is just the framework that defines the location of the tool and the workpiece. The orientation defines what orientation it is going to be in when in the milling machine, For most milling machines X and Y are the horizontal plane movements side to side, and the Z axis is the up and down. It's important to set these based on what orientation the stock will be in the machine. The origin is where you set the zero point as. On the pocket NC the origin is a specific location defined in the vice CAD, but for machines with probing the origin is often someplace you set it on the stock material. That can mean when you probe the stock material for its location, you can set a corner as the origin, and then in the setup, you select that same corner as the origin. Then you select your model which is the CAD of the dial you just designed, and then optionally you can select a fixture. You only need to check the fixture if you have the vice of the machine in your CAD. When you select the fixture bodies, that is a sign to tell Fsuion 360, that you don't want to machine these so it helps with the collision avoidance.

The next tab is the stock tab where you define the size and placement of your stock material. Since we made a body that is now most likely hidden to define the stock, we can change the mode from Relative, to From Solid and then select the solid that we created to represent our stock under models in the model tree.

The final tab is the post process tab which affects the G code fusion 360 generates. For the pocket NC machine, this can be left without making any changes however some machines might require changes so it is important to look at your machine guide.

At the top of the machining workspace you can see the 2D and the 3D toolpaths. If you click on one, it will open up a menu and there will be 5 different tab and I will go through briefly the importance of each one. This first tab is the tool tab. This is where you will select the tool bit that you are using. You can add tool bits into fusion 360 by going to the Tool library which is a button on the top under the manage section, where you can right click under local and create a new tool library (if your CNC is run by someone, they might already have a tool library they can share) and then at the top of the tool library there is a plus symbol where you can add new tools. Once you have the tools you can head back to the toolpath you wanted and select the bit you just created for the specific toolpath. Then you select whether theres coolant or not, the Pocket NC has no coolant so you can disable it but many machines do have coolant. Then you define the spindle speed and speed of your machine and tool bit. I can't recommend any settings because each bit, material, and machine will be different so it's good to check any guides that comes with your machine and tool bits.

The geometry tab is where you will actually define what part of your workpiece you want to machine. This will often selecting machining boundaries defined by sketches or edges. The tool will then be either contained within that boundary, or be keep outside that boundary. There are other options in this tab which can be important and you can learn more about them by hovering your mouse over them and waiting for a few seconds for an info tab to pop up

The heights tab is where you will define the maximum depth you want your cut to go. That is known as the bottom height and you can change it based on how deep you want. You can also change the top height which is the height where the tool will start machining. It is generally good practice to offset the top height a little bit above where you think it will actually need to start just in case the stock is not exactly flat, or not positioned exactly where it thinks it is, then the tool bit won't go ramming into the stock. The clearance and retract height define how far the tool comes up to then go to its next pass or toolpath. These can be important to make sure your tool doesn't collide with the piece.

The passes tab is where you will define how deep of cuts do you want your bit to make, and how much it should cut on the side as well. This tab can be quite confusing as there is a lot of options but the important ones to look at are the Optimal Loads, the Maximum roughing stepdown, and the fine stepdown. The optimal load is how much the bit will move the side when doing passes. For example if you have a 6mm bit and you set the optimal load as 6mm then then entire cross section of the bit will be cutting. If the optimal load is 1mm, the the bit will only use 1mm from the edge of the bit in each cutting pass. A lower load means the bit will experience less stress but also cut more slowly. The max roughing step down tells the software how deep do you want to go in each pass. If you have a cut where you need to go down 10 mm then most likely yo wont be able to cut the 10mm depth right away, so instead the max roughing stepdown tells the software how deep the bit should go. If you set it as 2mm, then it will cut away 2mm at a time and instead of cutting the 10mm in 1 pass it will cut it in 5 or 6 depth passes. These setting are very important so that you don't break the bit. One a curved surface, the roughing stepdown will cut away the material quickly, but it will leave it looking like a stair case. But if you use really small roughing stpesns to have a smaller stair case effect and smooth surface, then the machining will take too long, That is what the fine stepdwon is for. It will make a lot of the rough larger distance stepdowns and then come back again and between each large stepdown, it will make a lot of smaller passes. You can define this distance as smaller to have a nicer finish.

The linking tab is also slightly confusing as there is so many different options. Most of the options you can probably leave as defaults but one of the most important ones that you might want to changes is under Ramp, and change the Ramping angle and helical ramp diameter, For softer materials you can have a larger ram angle but for harder materials like aluminum you want a shallower ramp angle. A ramp is a helix that the machine does to get deeper into the material instead of going straight down. A smaller ramping angle will cause less stress on the bit.

That's all for the tabs under the toolpathing so you should have a general idea what to do! From my experience it can take many hours of trial and error to get things to work but there's some huge enjoyment when you finally get the toolpaths to look good. Some of the toolpathing will have 1 additional tab which is called Multi-Axis which can be useful if you have a 5 axis CNC but for this project it is not necessary as it also requires the machining extension.

The first toolpath is a 3D adaptive clear path. This is most likely to be the most common toolpath you use for most machined parts. It will automatically recognize your pieces and avoid it in 3 dimensions. This is also known as a roughing pass so typically you do another pass after this to increase the finish but for my application, most paths will be ok as the adaptive clear.

This first pass faces the backside to get it down to the level where the bottom of the dial is.

One really important feature to use in the Fusion 360 manufacturing is that once you've created the toolpath, right click on it in the tree on the left, and click simulate. This will simulate the tool path and you can speed it up and slow it down and see how it moves. This is also useful because at the bottom green bar, if there's any collision within the toolpath, they will show up as little red bars on the timeline and you can hover over it to see the problem and click on it to go to that moment in the simulation.

The second step uses adaptive clear again to clear out the inside of the dial. This also uses the 6mm bit and has a small fine stepdown because the top of the inside of the dial has a curve which I wanted to be smooth.

You can see a timelapse of that machining process in action.

The 3rd toolpath which still uses the 6mm bit is a very short toolpath. The purpose of this one was to clear some of the aluminum away from the vice screws and make sure that it is aligned properly

The next step was to create use adaptive clear again to remove the bulk of the material to generate the initial shape of the dial. It is important to use the simulations for each toolpath to make sure there are not any collision issues and the simulations are also useful because they give an estimated machining time. Especially when you are starting, you should be watching the machining process throughout the entire process, so its good to make sure the machining time is not extravagantly large.

Part of the machining process for this step can be seen in the timelapse.

This step also uses the adaptive clear to get rid of the rest of the bulk material remaining.

This next toolpath uses a Parallel toolpath rather then the adaptive clear. The parallel path is a finishing pass meant to create a good surface. You can see the importance of this in the images above. Without the parallel pass, and with just the adaptive clear you can see the steps phenomenon that I was discussing above, This step like feature doesn't look or feel as nice so the parallel pass goes over it up and over and then down, rather then in circles.

For this next path, we have to change from a 6mm bit, to a 1mm bit to be able to fit and clear the slot. This uses a adaptive clear process again

This 2D pocket toolpath uses the 1mm bit to create pockets on the top surface of the dial for the bolt holes

This is the final toolpath for this part which uses an adpative clear to create the hole chamfers for the bolt holes. it also uses a 1mm bit.

The post processing is an import part you actually export the toolpaths you have create as g code files so that the CNC machine can read and understand what you are trying to do. For the first machined piece of any part, I highly recommend exporting each toolpath individually as individual g codes, rather than the entire setup. If you export the entire setup as one g code, then the CNC machine will machine all of them, however if there are issues with the paths you have created it won't stop unless you force it to stop. If you export each toolpath individually you can upload to your CNC one by one to make sure each step works.

To actually post process you can right click on the toolpath and click Post Process. The post process setting will vary widely based on the machine you have but I have shown a screenshot of the settings I use for the Pocket NC V2-10 machine.

The first step of the machining process is to make sure that your stock is the correct size and then to place the material into the vice. During the machining process I recommend reducing the feedrate especially right before a new tool path. This ensures that you can watch what is happening and if anything goes wrong you can quickly stop it.One of the best ways to tell if something is going wrong is not only to see something wrong, but also if something in the machining process suddenly sounds bizarre, that is generally a good indication that something has gone wrong.

You can see a video of the end of the machining process with the 6mm bit. In total the machining process for this dial took ~12 hours, which I completed over the course of several days. However ensuring that your machining paths are correct and spending a lot of time checking them before starting the machining will likely save you a lot of time in the long run.

You can see part of the final ACL recovery product in the last image connected to the screen with the motor inside of the dial.

If you have any questions please feel free to reach out to me! I know there's a lot missing in the guide, there's just not enough space to go through everything and every setting so if there's something more specific you'd like to know I am happy to try and help!!