In this lesson, we're going to export G code for the part. After completing this lesson you'll be able to, create an NC file from a CAM program, create an NC program in Fusion 360, and modify code using an editor. In Fusion 360, we want to carry on with our optical pickup. Now that we've created this entire machining set of operations, we have to get it out to a machine. There are several different ways in which we can do this and there are some new functionalities that will be coming in the future that will also simplify this process. But right now, we want to take a look at the actions that we have available. Under the Actions we have something called Post-Process, this is where it's going to convert this to a machine specific code and that data can then be loaded onto your specific machine. There's another option that we have located in the Setup drop-down called Create NC Program. This is also found at the very top level. This is a slightly different approach to creating that code, but we're going to take a look at both of them so that we can understand what the differences are. The first step in the process is to make sure that we have setup one selected and then we're going to go to Actions and Post-Process. From here, the next thing that we want to do is we want to pick our post configuration. The post configuration is going to be based on the machine type first of all and then a specific vendor. From here we can filter down through the list of vendors and I'm going to use a HAAS automation. Then from there you can take a look at the list of HAAS post that you have available. These posts can be stored locally or you can use posts that are from the HSM post library or you can even store them in the Cloud. I'm going to be using all the default ones that are loaded with Fusion 360 so that way we don't have to worry about any compatibility issues. But these posts again are very specific to your machine and controller. From here the information in the program setup and the program comment is going to be populated based on information inside of your setup. If you've left anything empty, this program comment likely will come from a previous program. In this case I'm going to reset this to optical pick-up and I'm going to use the 1,001 for my program number. Below this you can see that we have open NC file and editor as well as reorder to minimize tool changes. I don't like to use this reorder option because I always want to make sure that I simulate how the material is being removed from my part, but this is an option to readjust the order of operations based on the tool. Everything we see on the right-hand side, these are all properties of that post configuration that can be tweaked on the fly. For example, if you want to use a chip transport, if you have an auger that's in your machine and there isn't a code to turn it on, you can use this option to put the code in to turn that auger on. From here, the next step is to simply hit "Post," we have to select a location where we want to save our post and if there's already one with that number, we have to decide whether or not we want to replace it. If you're making several posts, you want to make sure that you do take a look at whether or not you're overwriting other data. Once we have posted it, it's going to open up in any of the code editors that you've chosen. For me it's opening up by default in Visual Studio Code, sometimes it'll open up in a text editor or sometimes if you have a dedicated post processor file, you might run in a specific editor. From here we can take a look at the code and see exactly what we have, at the top we have our comment and the program number, we have information about some of the options we may have set, and then we have the tools that are being used, a drill, a tap, chamfer mill, tool 8 which is our quarter-inch flat, and tool 10 which is our half-inch flat. From there it starts to initialize the program and then it begins by referencing the coordinate system. It starts our tool change, a spindle speed and it moves to G54, it's basically telling the machine that this is your coordinate system reference in relation to your absolute coordinate system. From there it'll start things like whether or not to turn on and off coolant, whether or not we want to reference a specific operation, so you can see here it's calling for absolute positioning and it's using some of the information that this specific host code is going to need. As we go down the line, once it moves to the next operation, we can see that gap for me on the right-hand side based on where the gaps are in the long list of code. You can see that we move onto a 2D contour, as we go down we move on to 2D adaptive, and you can see that the 2D adaptive has quite a bit of code because there are a lot of tool motions that happen for these adaptive operations. Then as we move into the next adaptive once again, it tells us exactly what that is. The 2D Adaptive 2, that information comes directly from our browser, so when we see that the 2D adaptive with a two after it this is exactly what we have here, and we can rename this to be more helpful when we're talking about reviewing that code. Now that we've seen how to use post-process, let's take a look at how to create an NC program. From here, the NC program will allow us to do several different things. Once again we're going to pick an output folder, we're going to pick basic information like whether or not we want to add a comment, and then we can go down and we can pick which machine and vendor we're going to use. For us once again, I'm going to pick HAAS automation. Next we want to make sure that we pick the correct machine, once again I'm going to use that pre-NGC. We have all the options that we can change such as using that chip auger and then we move over to the Operations tab and we decide which of these operations we want to post. If we want to take the entire Setup 1, we can simply select that and then we can post. One thing that's great about using the NC program is that it actually is going to save it in a folder inside of your browser, so this means that we can create the NC program and we can save it without posting it. There are warnings that's telling us that the work offset has not been specified so it's defaulting to use G54. We can right-click and edit this and make any changes that we want, and if we take a look at our settings you can see that we can go through, we can change any of our options, we can make adjustments to the operations, and then we can simply say Okay to save that NC program. From here I want to make sure that I do save this file but I strongly recommend that you get comfortable with both post-processing as well as creating those NC programs. Once you have a part that has multiple setups or potentially you want to turn on and off different operations, creating those NC programs can be a great and efficient way to do it.