In this lesson, we'll create a pencil toolpath. After completing this lesson, you'll be able to identify pencil toolpath requirements and create a pencil toolpath. In Fusion 360, we're going to carry on with our 3D finishing strategies. Now that we've taken a look at what's in this file, we want to start by programming a pencil toolpath to clear out the smaller fillet as it wraps inside of this pocket. This is a great example of where a pencil toolpath can be extremely handy to follow that fillet through its path. We're going to go to our 3D drop-down and we're going to take a look at the 3D pencil option. As we look inside of here, you'll notice that pencil shows a single line on the graphic. A pencil is really meant for us to take the correct size ball and mill or a rounded tool and wrap it through this fillet. Right now I've got an eighth inch ball and mill which is not the right size. We know from measuring that fillet that it's a quarter-inch diameter or an eighth inch radius. We're going to try it with this tool and see if it works, and then we'll figure out what we need to change. For our machining boundary, we're going to use the Bounding box option, but then we're going to use Avoid/Touch Surfaces using the Touch Surfaces option. I'm going to simply select the fillet and all of the areas that I want to cut, moving my way around the part until I'm happy with my selection. Then, again, make sure that I have Touch Surfaces turned on and I can move on to some of my other options. Inside of my Passes section there's many different things that we can take a look at. First you'll notice a new option that's shown, is called bitangency angle. Now the bitangency angle is something that is a little hard to describe. I'm going to go in and I'm going to turn on my tooltips because there's a great graphic when we use the tooltips that'll help us better understand what this option does. When we hover over bitangency angle we can see what that angle is actually describing is the contact area of the rounded tool as it's intersecting our geometry. The default value is 20 degrees, which means that it's going to try to keep 20 degrees in contact to the part. You'll notice that as the angle increases in the graphic from 45 up to 75 that it's using more of that tool while it's cutting. This is to determine the number of passes that are along a wall or a fold on our geometry. Once again, these tooltips can be extremely handy. Anytime you hover over a dialog box, you'll get information in a graphic about what this is telling you. As you're learning some of these operations, it's a great idea to keep that turned on. From here we have a couple of things that we can define such as the number of stepovers and the stepover amount. Right now it's 0.625, and I'm going to reduce that to 0.0125. I want that to be a little bit smaller. We're going to do a single stepover, so I'm going to have a number 1 in there. I'm not going to touch the bitangency angle or the overthickness value, but note that the overthickness value is the amount between the actual part radius and the actual tool radius. In this case, I'm just going to leave all these as default and say okay and see if we can get an operation. Inside of here you'll notice that it's empty. There's no passes to link. Again, I mentioned that really we should be using the correct size ball and mill in order to do this. But let's see if we can make some adjustments to the operation such as adding an eighth inch to the overthickness value. I'm going to add an eighth inch. I'm going to see if it can generate an operation. You see here it's calculating and it is able to go in there and actually make a cut. Let's turn on our passes showing our cutting moves and see exactly what's going on. You can see that it makes multiple passes and it's dropping down in this area here. What I want to do is do a quick simulation to see exactly what's going on. I'm going to play through and see where the tool is moving. Takes us down, it works its way around exactly where we would expect it to, and then it's going to work its way back, and again in the preview it showed that it had three passes, so it's going to go back through one more time before it finally finishes. Using that overthickness value was allowing us to use the smaller end mill. But I want to try it with the larger end mill. I want to pick something that's exactly the right size. In my library I don't have a quarter inch ball and mill. I have a quarter inch flat, a quarter inch tab, and a spot drill. I'm going to go into my Fusion 360 library, into my Sample Tools-Inch, and I'm going to start filtering by milling, and then I want to pick ball end mill. This will allow me to quickly and easily select the quarter inch, but again we have to remember that we need to pick the correct cutting data. All of the samples that I provided only have a single cutting data file, but this one we want to make sure that we pick the right one. Then I'm going to go back and reset my overthickness to zero, and then I'm going to say okay and allow it to generate this operation. Now we have a single pass, and you can see here that this is going to be likely a much better result using this larger tool in this case. You'll notice that it does start inside of that pocket and then it moves its way back around. While this is not likely an ideal situation, this is going to be okay, and you can see that we've actually cut all the way down to the underlying part. We can see because we have comparison turned on, turning it green or seeing some of that gray underneath means that we are cutting down to where we expect. This is a much better result, and now that we have this new tool in here it's automatically assigning it tool number 3, and that's because tool number 3 wasn't used. If we go into our machining library, you can see that tool number 3 is actually a number 7 drill. If we were going to use standard tools that are in our machine, we would want to make sure to fill a position that wasn't used. Inside of setup 1, tool number 3, I'm simply going to edit this tool, we're going to go to post-processor, and I'm going to set this as tool number 11. I'll accept it. It's going to update the operation. Now if I look at my tool library, there was nothing in that number 11 spot, and this will hopefully prevent us from having any issues with tools. Next, I want to take a look at creating a pencil operation on this portion of the design. Once again, we'll go to 3D, select a pencil, and this time we know that we need that larger ball end mill and we have one in the file already. If we select Documents and 3D finishing, you can see tool number 2 is a three-eighths ball and mill. We're going to select that. Under Geometry once again we're going to use the Bounding box option, not manually selecting an area to locate it, but we're going to manually use Touch Surfaces. Once we select all of these, we're going go to our Passes section. We're going to take a look at the stepover amount. I'm going to use a single stepover, leaving all the rest of the options as is for now, and allowing it to create that operation. Notice that in this case it does two passes. It's a little bit different because of the bitangency angle. We can likely make some adjustments and see if we can get a little bit closer to having that single pass, but ultimately the results look pretty good. One thing that we can do is we can allow it to go a little bit farther by using these Avoid/Touch Surfaces and allowing it to traverse out a little bit farther. If we increase the number of steps and maybe take the bitangency angle up to 30 degrees, we might be able to get a single cut or at least go a little bit farther out. Let's go ahead and take a look at the simulation and see where the tool is going now that we've made those changes. You can see that the tool is still cutting up high, and it's moving its way along that face, and it's coming back and cleaning it up. Once again, not a perfect solution, but sometimes these operations are going to take a little bit more work in order to figure out the sweet spot allowing the tool to maybe go outside of a boundary that we select, and if we use the Bounding box option or even a selection, we can try to select certain areas, and if we don't have a good selection, then we might be able to actually come back in and manually make a sketch to allow us to pick that area. Now that we've opened this up, let's do one more simulation and see exactly where the tool is going. Once again, the tool is riding a pi and then it's coming down low and cleaning it out. This has been a look at pencil mill and two different ways in which we can use it. With a smaller end mill and using some of that overthickness options to help us get closer, as well as using an appropriately sized end mill for whatever fillet we're trying to machine. These are both great options allowing the tool to both traverse in 3D, or in this case only in two dimensions, but allowing it to move back and forth in x and y. From here I do want to make sure that I save this before moving on to the next step.
