In this video, we'll finish details on a part. After completing this step, you'll be able to used 2D Contour, 3D Contour, and CAM expressions. Infusion 360, we want to carry on with our coupler for CNC Mill. So far, we've only added one tool path which is a 3D Adaptive Clearing that allowed us to remove a lot of material from the part. However, we need to go back and we need to make some adjustments. The original model had a small filling in the bottom corner, so we need to make sure that the axle stock to leave was enough to account for that filling. So in our passes, I'm going to go back to my stock to leave in the axial direction, and add 0.015. And in the radial direction, I'll do 0.015 as well, that allows us to leave enough material on the sides and the bottom of these bosses. And that means that the tool can come through and it can add that filling when we're using a bull nose mill. The next thing that I need to do is finish off this face with that bull nosed mill. I can do this with a 2D Pocket toolpath but first I need to select the tool. Notice that tool number 7 still has some cutting data errors. It's telling us that it's missing some required data, so we need to go in and edit this tool. Undercutting data, we're going to go through each of these, and see what information is missing. You can see that it's missing the passes and linking information for a lot of these different cutting datas. And that's because, originally when we created this tool we went from a ball nosed mill, and we changed it to a bull nose mill. Now, these two different tools have different linking parameters. So one thing that we can do is we can modify all these parameters or if this is problematic, we can always go into the Fusion 360 library. And we can filter by milling, and bull nose mill, and find one that contains all of that data. So what we're going to do is grab a quarter bull nose mill, we're going to right click, and copy the tool, and go into our cam DFM, and we're going to paste the tool. I'm going to take the original one that has issues and I'm going to delete that, and then I'm going to modify the bull nosed mill we just copied 1st. I want to change it to tool number seven, and next I'm going to go into my cutter data, and I'm going to make it a four flute, and make sure that the corner radius is 0.015. We're going to say okay, and now we have tool number seven that allows us to use that cutting data that's already populated for us. We're going to use it with aluminum finishing, and remember that our machine configuration has a max rpm of 12,000. So this means that some of these are getting really close to that limit, but nothing has gone over the limit yet. For geometry, for my 2D Pocket, I'm going to select this face, and I want to use stock contours and rest machining. The tool that came before it was 0.25, with a corner radius of 0.125. In the passes, we're not leaving any stock and we're going to say okay, and allow it to machine that geometry, noting that it is giving us an error. It's empty based on the rest machining tool path parameters. It thinks that the material has all been removed because rest machining inside of a 2D operation is generally taking a look at areas where a tool could not get to. So if we just say okay, and allow it to generate this tool path. Let's go ahead and take a look at the cutting moves. It's machining this entire face, it's going around all the bosses, and it's using that to finish all the geometry over the opening. Because it thinks that that's already been machined and it's leaving the small filling around the corner. So everything looks pretty good there and it's enabled us to get that geometry and that data that we need. But now we need to finish off some additional areas. We've got this board here, that goes all the way through, and if we measure that we can see that it is 0.24. It's relatively small and it might be easier for us to machine from the other side. However, this board has to be machined from this side, as does this taper. We also need to machine the outside, so we need to consider what tools we have and when we want to perform these operations. Tool number five is a quarter inch end mill, tool number seven is a quarter inch bull nose, either will work just fine. However, I'm going to use the quarter inch end mill to machine the outside before moving on to the inside. We're going to do this with a 2D Contour and I'm simply going to select this bottom edge. And we're going to move on to our heights and instead of the selected contour, I wanted to come all the way down to this bottom face.O Inside of our passes, we need to make sure that we're not leaving any stock, so make sure that that's turned off, and all the rest of the settings will be as default. This means that it's going to come down, it's going to make a single pass around the part, and then it's going to retract. Next, we need to try to get into this bore. We've already cleaned out some of the material and we know that it's large enough that we can go in with that quarter inch end mill. So I'm going to go into a 2D bore using tool number five, And then we want to select our geometry. I'm going to use all the default settings, allowing it to go in and clear that material out. I do want to modify my 2D Contour. I'm going to edit and select a different tool, making sure that I am using tool number five. And then we'll say okay, allow it to regenerate, and then we'll move our 2D Pocket with our bull nose end mill all the way to the end. Keep in mind because some of these operations are model aware, it's going to take some time to recalculate. So now we've got our 3D adaptive, our 2D Contour around the outside, our boar on the Inside, and our 2D Pocket with the bull nose mill that cleans up this top face. The next thing that we need to take care of is we need to take care of this taper. The taper can be done with a bull nose mill or a ball end mill. In this case, we're going to use a 3D tool path called 3D Contour and we're going to select a ball nose mill, and we haven't created one in our library. So we need to go into our filters and we need to filter by ball end mill, and we need to look for a ball end mill that's going to work. In this case, I'm going to take a look at using a quarter inch ball end mill with aluminum finishing and selected. That's a rather large tool, so I need to be aware of how much room I actually have. But let's go ahead and take a look at what geometry we can cut with this. The machining boundary by default is going to be a silhouette, but I want to contain the tool within this area. I'm going to allow the tool to center on the boundary and I've got contact only selected. We can also use A slope, to limit the slope from anything that is above 1 degree. And we want to go all the way up to 89 degrees, this will prevent us from machining the flat faces or the vertical walls. We're going to go into our parcel section to make sure that we're not leaving anything and then we need to take a look at our maximum step down value. This is going to be important as we want to make sure that we have a very small value, in terms of the step over to replicate that face, and I'm going to use 0.05. And then I'm going to say, okay, I'm going to allow it to generate the tool path, noting that the resolution is probably not fine enough for what we need. So we're going to make some modifications to those settings. Instead of the maximum step down of being 0.05, we're going to go to a 0.01. And now we're getting a little bit closer to that final shape. But let's note that it is going all the way into this pocket and we don't want it to machine that far. So let's make a few more adjustments, this time we're going to modify the height. Instead of the model bottom, we're going to use a selection which is going to be this edge. And will allow it to go past that edge a small amount by putting a minus 0.1. We'll say okay, and this will contain the tool a little bit better, allowing us to get a little bit closer to the final shape. We could also use other types of tools, we could come back with a smaller ball end mill or a bull nose mill. Or potentially even come in with a chamfer mill that can cut that very quickly and easily. Depending on the requirements for that geometry, whether or not it needs to be that large of a champfer, whether or not it has some sort of specific engineering requirement. It would determine what we would do in terms of its finishing geometry. For this design, it's pretty much a cosmetic feature and it's not a requirement for engineering. The last thing that I want to do is I want to come back and I want to chant for these upper edges. We have to tool paths that will work for this. We have a 2D Contour and we have a 2D Chamfer. The 2D Chamfer is a great tool path because it allows us to actually set a physical distance requirement between the tool and other solid geometry. 2D chamfer inside of a 2D Contour works, assuming you select a chamfer tool. We're going to go into our camp DfM library, and select tool number nine, and then we're going to select all the edges that we want to chamfer. These are going to be all the upper edges of these bosses and then we need to determine the chamfer geometry in the parcel section. 0.04 is going to be a little larger, so what we're going to do is we're going to modify this to be 0.02. The tip offset is going to determine how far down the tool is going past the chamfer. And then the clearance is going to be between the tool, and any other solid geometry, which in our case is not going to be a problem. We're going to say, okay, allow it to generate, and now we've chamfered those edges. You'll note that there's a small amount of material that's been removed on top and really we need to go back to a simulation to make sure that this is okay. But I'm going to go back in and make one small adjustment to the passes and I'm going to reduce the chamfer width to 0.01. And I'm going to reduce the tip offset 2.01 and say, okay, this is going to put a much smaller chamfer on the edge using a better portion of the tool. At this point, let's make sure we save. And then we want to take a look at one more aspect of the CNC programs. I'm going to go back into my 3D Adaptive and I want to take a look at the parcel section. When we modify values in the parcel section, we have a maximum roughing step down. And when we modify this value, the fine step down and the minimum step down both changed. If we hold down the shift key and hover over those dialogues, we'll get a preview of the cam expressions that are used to define those. We can also right click and edit the expression. In this case, math dot minimum is going to take the smaller of the two values. The tool diameter times 0.5 or the maximum step down times 0.1. So based on your tool diameter and based on the maximum step down value that is added here, it's going to determine which value to use. The same thing goes for the minimum step down unless we overwrite that value. So by default, the minimum step down is going to be based on a fine step down times 0.1. So it takes that 0.04 and you end up with 0.004. Cam expressions are extremely handy and can help you set up your programs to run a little bit smoother and with more optimum settings based on your specific tools and machines. Once again, let's make sure that we do save this before moving on to the next step.
