In this lesson, we're going to set up a CAM program and tool library. After completing this lesson you'll be able to : Create a CNC Mill setup, demonstrate how to select a fixture and stock, and explore tool presets. In Fusion 360 we want to carry on with our 3D pocket sample. We already have the vice added and we've modeled the stock. From here we're going to navigate from the design workspace to manufacture. Inside of here, we're going to start in the manufacture workspace at the first tab under the milling tools. I do want to note that each of these has different toolpaths and operations at our disposal. However, all of them all start the same by creating a setup. We want to get started by creating a new setup. When we do this note that Fusion 360 is trying to create stock based on all the bodies and components in this design. We need to tell it exactly what machine we're using and what we want to focus our attention on. Inside of the setup notice at the top we have a machine selection. We can define or select a machine that gives us the ability to check against criteria such as the amount of travel a machine has, the number of tools it can hold, and so on. We're not going to be looking at that step for this example, but we do want to note that is what the machine option is. Next is the operation type and for 3-axis machining, we're going to be focusing on milling. Next, we have the WCS or Work Coordinate System. We're not going to set this up just yet because we want to define the model, the fixture, and the stock that we're using. To get started first we want to select the model. In this case, it might be hard to select because the stock is outside of the part, but if you move the cursor around in some cases you can simply grab the model. Notice now that Fusion 360 has redefined its stock based on our selection. Next, we're going to add a fixture. We have fixture and fixture attachment. In this case, we're just going to use fixture by selecting the fixed and floating jaws, the parallels as well as the upper portion of the jaws. This is going to allow us to check the collision or the tool position against the solid geometry that we're not intending to machine. Next, I want to go to the second tab which is our stock definition. Right now it's based on relative to the size and we can use this, and I want to make a note that currently this is set to metric. Even though the file was inch, when we come into the manufacture workspace it's going to default to the units in your user preferences. We can fix that after the setup so let's go ahead and change the mode to from solid and then we're going to select our stock body. From here we're going to navigate to the last tab which is going to be our Program NameNumber and our Program comment. We're going to set this as 40001. Then we're going to make the program comment of 3D pocket. There is a machine WCS offset option if we're going to machine multiple parts, but in this case, we're going to leave that set by default. Now I'm going to go back to that first or original tab and we're going to reset the coordinate system. Right now it's based on a box point but the orientation isn't correct. I'm going to reset this to z-axis, we can use a selection on our models such as an edge, because we have our stock modeled we can use the edge of the stock or we can use one that default axis. If I can't select it through my body, again I can always hold down the left mouse button and make a selection. Right now by reselecting the top face, it has reoriented our z normal to that top face. Now I'm going to reset the box point to be this upper left-hand corner which is against this stationary or fixed jaw on the vice. Now we have our x in the correct orientation in relationship to our vice, same thing with y and we have z pointing up towards the spindle on the machine. Everything else looks pretty good in here so I'm going to say Okay. Now that we have this setup, we can always go back into the model and expand this and we can hide the vice even though the vice is hidden, it's still selected in the setup which means that it will be used for checking the position of the tool and the holder against where our machining, to make sure that we don't have any collisions. Now that we have our setup created, I'm going to do a quick save and then I want to move on to setting up my tool library. In this case, we're going to go into Manage Tool Library and we're going to take a look at what we have. Right now in all section on the left-hand side, we have documents, which is our 3D pocket sample and setup1 that we just created. If we select this there's no data here because we haven't created any operations or selected any tools. We have a Cloud section and we have a local section. At the bottom, we have Fusion 360 library which contains a whole bunch of samples, such as sample holders, sample probes and sample tools, and both engine metric. Our focus is going to be on creating a new library in the Cloud. If you don't see the Cloud option, then you can always go back to your user preferences, navigate to the manufacture section and make sure that you enable Cloud libraries. I'm going to say Okay, and before I get back into my tool library, I'm going to quickly change my units to inch to make sure they match the design of the file. Then we'll go back into our tool library and you should see Cloud now if you didn't have it turned on before. You'll notice that I have one tool library inside of my Cloud but I don't have anything locally. The Cloud option is great if you use Fusion 360 and multiple different computers because every time you log in with your Autodesk account, you'll automatically see those Cloud libraries populated. In order for us to import a library, we're going to right-click and we can use a new library option to start manually creating a library either from sample tools or manually created once. Or we can select the Import option. I'm going to select Import Library. From here we need to navigate to the location where we have our library saved. For me, that's going to be inside of my lesson 1 datasets for machining 3 axis.tools. Once I say Okay we now have a new Cloud library called machining 3 axis and it contains all the tools that are saved inside of that library. You can see that we've got a spot drill, 3/16th drill, a number 7, quarter 20 tap, we have a chamfer mill, we have a ball end mill, we have some long finishing end mills, and then we have a facing mill. All of these are now contained inside of our library which means that we can select them whenever we start creating operations. Another thing that I want to make sure we understand are going to be the tool presets. Whenever we create an operation and select a tool we're going to need to make sure we understand those tool presets. By navigating back into our library and selecting a tool, for example let's go ahead and select tool number 8, a quarter-inch end mill. Right now under cutting, it's got default presets. If instead we go into the Fusion 360 sample library and we selected Tool, maybe we want to filter by a specific type such as milling, and then we want to filter by flat end mill. Then from here we'll select a quarter-inch. Notice that in the cutting data section there are a lot more presets associated with this end mill. We have aluminum for slotting, roughing, and finishing. Brass for slotting, roughing, and finishing. Then we have copper, low carbon steel, high carbon, plastic, and so on. What this does is it's going to change some of the values that are populated inside of this tool. For example, if we take a look at the difference between roughing and finishing, those differences are going to come into play when we talk about the feed rate. If we view the tool and we take a look at the cutting data, you'll notice on the left-hand side we have our presets and on the right-hand side, we can see the cutting data. If we take a look at roughing and finishing, notice that the feed rates for both vertical and the horizontal feed rates change based on these two settings. The roughing feed rates are slower than the finishing feed rates because the depth of cut or the engagement of the tool is going to be more on a roughing pass so you're going to run it slower. Keep in mind that these presets are important whenever we're populating a library based on sample tools from Fusion 360 or possibly from a manufacture. However, the ones inside of the Cloud library for machining 3 axis only have the default preset, there's only a single cutting data pre-saved inside of those tools. From here we can close, we don't need to save anything in the tool library because it's in the Cloud it's automatically updated. But any changes that we may have made to this design we want to make sure that we do save it before moving on to the next step.