In this lesson, we'll be exporting G-code for an entire part. After completing this lesson, you'll be able to create an NC file from a CAM program and modify code using the editor. Let's carry on with the file from our previous example, and let's export the code for our entire part. So that way it can be sent to a machine and, ultimately, cut. To get started, I'm going to make sure that I select all of "setup one". Then in the action section, I can select "post process." We can also do this by right-clicking, and selecting "post process" in the menu that shows. Inside of here, we'll have to first look for a post configurator. The way that we can do this is we can use some of our filtering options to first only look at milling. We can select a specific vendor. For example, we can navigate down to Haas Automation, and then inside of here, we have a couple of HAAS options. There are two that have an a-axis on them or a fourth axis. Then we have a HAAS which says "pre NGC," and then, we have a HAAS UMC 750. We're going to use the HAAS pre NGC, and this is going to be the post file that's going to convert all of our tool paths that we created in Fusion 360, and it's going to process them into something that a specific machine can use. Now, for the most part the code that gets exported is fairly universal. The way that G-code and M-code is read by many machines is the same, but there are a lot of nuances to what machines want to see. It could be very simple, like the way comments are displayed or the way lines are numbered, or there could be very specific examples like certain G-codes or settings that can only be used in a certain processor. So from here, we can manipulate things like the program number, which can be also created inside of the set up. You also notice the comment comes through basic part. Now, this is from a previous example, so we're going to modify these values to better reflect our part. We're going to do 50001 for our program number, and our part is going to be renamed to optical pickup. I do also want to note the box on the right-hand side. These are parameters that are directly in the post processor, that we can manually change here by affecting some of these settings. Things like built-in tolerance values, whether or not we're using a chip transport, which is an auger in the bottom of the machine. If there's an option to activate a fast tool change. If we want the home position of the machine to be centered and generally the home position will actually push the table forward and all the way to the left in the negative-x direction. Then we also have a lot of other options in here. We're not going to change any of these settings, but this is a great way for us to customize our post processor, without actually having to go into that post file and make those changes. We also want to make sure that we use the "open NC file and editor" option. Then we're going to say "post." It'll ask us one more time for the location of this code, and I'm going to navigate to the location of the data set with all of my files. And then, we're going to go ahead and save the program here. Once it's saved and the codes created, it will be opened because we had that option checked. Now we can navigate through the code and take a look, make sure there are no glaring things that we see in here that we might need to change. You'll notice at the top it has our program number, and in this case because we are using a HAAS controller, it starts with the letter O, then it's 50001, the comment for the part of optical pickup. Then notice that we're using high feed G1, feed rate of 500 instead of G0. Again these are settings that are specific to the controller. Then it shows you some tools. So it tells us exactly what each tool is. Tool Number 3 is a taper drill with a 118 degree tip. Tool Number 4 is our quarter 20 right-hand tap. Five is going to be the 0.125 chamfer Mill. Then eight is going to be our quarter-inch flat end mill, and 10 is our half inch flat end mill. As we go down the program or the tool path inside of our program, phase one. And then as we go down, we can see other tool paths, contour one. So this is where it's real handy for us to rename these something that is meaningful and makes sense. So if you're not the one that's running this at the machine and somebody else is, they'll know that this 2-D contour is actually for the outside of our part. So just keep that in mind as we look through here, that comments can be very helpful especially if you're not the one running the part. We're not going to dive too deep into this code editor, but there are plenty of options that we have in here such as find, and find and replace that we can use, such as in most text editing programs. We can also change the view, such as splitting the screen if we're going to view multiple codes. We also have some theme options that we can change. We can change the font size, and we can use the highlight option to highlight active lines if we're scrolling down through the code. There's some navigation options and, of course, there are some edit options as well, allowing us to again just go through the code and figure out specifics inside of our code and figure out if we need to change anything. Now, in this case, for example, if I wanted to make a change and I didn't have direct access to the Fusion 360 file, I could go in and manipulate things like the spindle speed. Let's say Tool Number 10 can actually run at little bit over 1500 RPM instead of 1100. We can make that change in the code and save it here simply by using the code editor. Because the focus of our course is not to talk about manually programming G-code, we're really just focusing on the top level of simply viewing the code and being able to navigate it in the editor. Once we're done here, go ahead and close this. It's automatically saved unless you make some changes. Then it'll prompt you to save that document and we can save it. Go back into Fusion. We shouldn't have to make any saves to our file, but if it prompts you to save, go ahead and do that before moving on to the next step.
