3D Modeling & CAD for Motorsport: Computer Aided Manufacturing
Watch This Course
$199 USD
-OR-
Or
8 easy payments of only $24.88
Instant access. Easy checkout. No fees.
Learn more
Computer Aided Manufacturing
10.41
| 00:00 | - CAM or C.A.M. stands for computer aided manufacturing. |
| 00:03 | It's the use of software and computer controlled machinery to automate the manufacturing process. |
| 00:09 | From this software, like Fusion 360, we can output files that define the tool path in a programming language such as G code which a computer numerically controlled, AKA CNC machine, can use to manufacture our designs. |
| 00:25 | We discussed this very briefly when covering output files and now it's time to take a closer look. |
| 00:32 | Just like the other topics in this section of the course, CAM is an advanced subject that requires a lot of extra knowledge so the intention of this module is not to teach you everything you need to know about CAM, but just rather an introduction to get you up to speed. |
| 00:47 | To be very clear, if you're getting the production of your designs outsourced, it's very unlikely you're going to need to complete any CAM work, even in a professional environment. |
| 00:58 | That's because this is mostly always done by the manufacturer as they're the ones with the skills and expertise in this area. |
| 01:05 | Not to mention, mistakes can be extremely costly in terms of breaking machines and tooling as well as the associated downtime. |
| 01:14 | It should go without saying that you'll need a good understanding of the machining processes to complete this work as well as all the information on the CNC machine and the tools that are going to be used. |
| 01:25 | That said, even if we don't use our CAM results to drive the machine, this process is still useful as it can highlight parts of our design that might not be ideal when it comes to machining and give us the chance to make modifications. |
| 01:38 | CAM can be used for CNC milling, turning and 2D cutting machines like laser or waterjet cutters as well as for additive manufacturing such as 3D printing. |
| 01:49 | We'll be covering 3D printing in its own upcoming module so we'll be just discussing methods that work by removing material for now. |
| 01:58 | You might have heard of G code as this is the most widely used of the many CNC programming languages to define tool paths and essentially tells the machine where to move, how fast to move and what path to take to get there, also known as the tool path. |
| 02:15 | In the past, tool paths have been written manually but with modern CAM software, we use various functions to define the tool paths and then this will be converted into G code or another post programming language. |
| 02:28 | This has been a time saving game changer as the models get more complex. |
| 02:32 | CAM functionality in Fusion 360 is accessed through the manufacturing workspace. |
| 02:38 | This is another key area of difference between free and paid versions of Fusion 360 with the paid version having significantly more CAM functionality. |
| 02:48 | This isn't actually common in CAD software, usually reserved for CAM specific software. |
| 02:53 | So to have access to it is a big advantage should we ever need to use it. |
| 02:57 | Let's look at an example using a simplified model of a roll centre correction spacer from a macpherson strut car which we want to be milled from billet aluminium. |
| 03:08 | Even with this being a simplified version of an already simple part, this is still a lengthy process as machining this part requires multiple operations, different tools and different setup orientations in the machine. |
| 03:22 | At the risk of overcomplicating this module and making it way too long and complex, we'll be just covering a few of the basic machining operations to get a general idea of the CAM process. |
| 03:33 | With the model open, we can navigate to the manufacturing workspace. |
| 03:37 | Here we can see we have a range of toolbars for each of the manufacturing methods. |
| 03:42 | In our case, we can stay on the milling toolbar. |
| 03:46 | The first thing we need to do is make a new setup from under the setup tab which automatically creates the material stock for our part to be machined from. |
| 03:55 | This is shown as the transparent box around the part. |
| 03:59 | If we look at the second stock tab, we can see that by default, the stock model is set to relative size. |
| 04:06 | This method is more suitable for machining parts out of relatively small areas of a larger stock which would be most common for 2D cutting operations like laser cutting or routing. |
| 04:17 | In our case, if we were planning on just making two of these parts for a vehicle, it would be more likely that we'd use a small piece of stock for each part. |
| 04:26 | For this, we'd want to change our stock mode to fixed size and enter the dimensions of this stock and then use the offset values to position our part within the stock. |
| 04:36 | For example, our stock could be 120 mm in width and 60 mm in depth which is just a bit bigger than our model. |
| 04:45 | But then use a 70 mm height for some extra material to clamp onto with a fixture so we can set the model position as centred in the width and depth but offset 2 mm from the top for the height. |
| 04:59 | Back to the first setup tab, at the top of the setup window, we can select the machine we intend to use to make the part. |
| 05:06 | As you can see, there's a big library to choose from. |
| 05:10 | For our example, we'll just choose an Autodesk generic three axis machine which we'll need to download the file for this in order to use it. |
| 05:18 | At this point, we need to set our work coordinate system. |
| 05:23 | We want to move the stop point to one of the top corners of the part so this can be easily located in the machine. |
| 05:30 | Then we need to set our X, Y and Z directions so the Z axis is in the vertical direction, meaning the base of the part sits in the bed of the machine and the X and Y axes follow the edges of our stock. |
| 05:44 | If this isn't already correct, we can click on the X, Y and Z arrows and change the positive directions. |
| 05:51 | All of these settings are essentially related to positioning our part in the machine and aligning it with the machine's own coordinate system. |
| 05:59 | Again for simplicity, we'll leave all the other settings as their defaults, however usually we'd want to consider the fixture used to secure the material to the machine's bed to make sure it's avoided and there are no collisions. |
| 06:12 | For our example, let's just assume the fixture is clamping on the sides of the stock and is lower than the height of the bottom of the model. |
| 06:20 | Let's start the machining process with a 2D adaptive clearing operation. |
| 06:25 | This is a roughing operation that removes stock material down to the face of the part. |
| 06:31 | For the tool, we can use a generic flat end mill from the library which comes set up with all the parameters. |
| 06:38 | In a real case, we would need to check and possibly change these to match our tooling or set up all our own tooling in our tool library. |
| 06:45 | Under the next tab, we can define the geometry we want to machine. |
| 06:50 | So for our example, we can select any horizontal faces or edges. |
| 06:55 | Let's select all the top faces including the step as well as the edges of the bolt holes, the bottom outer edge of the part and also the inner edge of the centre bore. |
| 07:06 | The next tab over contains our heights and the defaults are good for clearance, retract and top heights, however we'll need to set the bottom height to model bottom so the operation removes material down to that level. |
| 07:20 | Another tab over and we can control the passes of the operation, essentially how much material is removed each time to avoid too much stress on the machine and tooling. |
| 07:31 | This will depend on the machine we're using so in the interest of simplicity, we'll leave these settings as is for our example and click OK to finish our adaptive clearing operation. |
| 07:42 | We get this graphic of our tool and can use the simulate function to view how it moves over the part and choose to view the stock as well. |
| 07:51 | This gives us a good understanding of what material has been removed and what's still remaining. |
| 07:57 | The resulting tool path lines are colour coded, those shown in yellow are the linking moves, essentially where the tool is just moving between the start and finish points. |
| 08:07 | The green is the lead in or lead out path where the tool is moving towards or away from the cutting operation and the blue is the path where the tool is actually cutting. |
| 08:17 | For the two bolt holes, we can use a drilling operation with a 13 mm drill bit to match the size of the hole. |
| 08:25 | We can simply select the cylindrical inner surfaces of the hole under the geometry tab and then use the select same diameter preference so it automatically includes the other hole as well. |
| 08:37 | The bottom height for this operation is good as the default of hole bottom. |
| 08:42 | As I mentioned earlier, there are a few operations still required to machine the rest of the part, including more roughing operations and finishing processes, which will need to be completed with the part the other way up. |
| 08:55 | The part would be flipped upside down and fixed through the bolt holes or on the sides of the part to machine the bottom face and inside of the centre bore. |
| 09:05 | After all the operations are defined we can use the simulate function to check our operations again and then generate the tool path by using the post process function, ensuring we use the appropriate post processing language for our CNC machine. |
| 09:20 | This could be G code or some other language such as GRBL or G.R.B.L. which is popular at a hobbyist level. |
| 09:28 | There's a lot more that can be done with this software to create the most accurate and efficient process and there's a lot more that needs to be considered for this process to be implemented safely and effectively. |
| 09:40 | But that's outside the scope of this course so let's leave it there and wrap up some of the key points found in this module. |
| 09:46 | CAM software allows the user to generate code that's used by CNC machines to manufacture our designs. |
| 09:53 | Before we use CAM, we need to have a clear understanding of the machines and associated tooling we'll be using as well as the operations that would be required to produce our design. |
| 10:05 | We can then simulate the setup of the part in the machine in the form of raw material stock and then simulate the operations required to produce our design. |
| 10:15 | Finally, we can generate the code that can be used by the machine to bring our design to life. |
| 10:21 | Even if we don't use the code that we've generated to drive the machine ourselves, this process is still useful as it can highlight parts of our design that might not be ideal when it comes to machining and gives us a chance to make modifications before sending it to the manufacturer. |
