In this lesson will learn how to create chamfer toolpaths. After completing this lesson you'll be able to modify feature parameters, create a chamfer toolpath, and use Pattern to create multiple chamfers. Let's carry on with the file from our previous example. Let's talk about creating chamfer toolpaths. So we have two different sets of chamfers in this file. We have a rather large chamfer that's 0.0625, then we have a small one that's 0.02. We want to take a look at using the same tool for both of these and how we can manipulate the settings. I do want to note that there are two ways that we can go about adding a chamfer to one of our parts. We can have it already modeled, and then the geometry is going to account for some of these settings. Or we could simply add a chamfer to a sharp corner by inputting the values that we want to see in that chamfer. So this is great if we want to take a sharp model and simply just break the edges with the chamfer. But in this case we have some design chamfers, so we want to talk about how we can use it in these cases. We're going to start by going to 2D and down to 2D Chamfer. For the tool, we want to select our chamfer and mill. So we're going to select tool number five, which is an eighth inch 45 degree chamfer mill. Keep in mind that this mill is a rather small tool and it has a large holder on it. So we need to be mindful of its geometry and how it might collide with the part. Next, we're going to take a look at the geometry. And in this case, we want to make sure we select the upper edge of our chamfer. Then we're going to go on to Passes, and this is where we're going to define the actual chamfer. The chamfer width is going to be a value that we're going to input if we don't have a model chamfer. For chamfer edges that are on the model this is going to be an additional offset. So we're going to enter a value of 0 here for the chamfer width. The tip offset is how far down we want the tool to come. Because right now the tip of our chamfer mill is going to be resting on this contour. So because we have an eighth inch tool, and it's at a 45 degree, I'm going to enter a value of 0.0625. This tool is really too small for this specific geometry. It's going to just be barely big enough to cut this. For our linking parameters, we can use leads and transitions if we need to. In this case, we can add a horizontal and a linear lead in distance. And I'm going to add these in as point 0.05. And I'm going to do the same thing for my linear lead in distance, add it as point 0.05 and say okay. So if we take a look at this toolpath we can see that the blue line showing where the tool is is all the way at the bottom of this edge. And again, this is going to be the tip of our chamfer mill. To make sure that we did everything correctly, let's select set up one, go to Simulate, and navigate to the end of this toolpath. Then we'll jump back one and we'll play through it. So you can see that the tool comes in there. It is showing it's red, it's detecting that there is a collision. And this is because, again, the tool is just barely the right size for the size of this chamfer. Which means that it's touching a lot of non-cutting geometry on the tool. In reality we would want to have at least a quarter inch chamfer mill for this geometry, or potentially change the shape of the chamfer on the part. Now, if we designed the part, if we know that's it a noncritical area, we can reduce that from an 0.0625 down to something like 0.05, and the geometry would be perfectly fine. This is actually a good chance for us to do that by navigating back to the design workspace, selecting the chamfer and finding it in our timeline. Then we're going to right click and edit the feature. So right now it's 0.0625, and if we change it to 0.05 and say okay, we can navigate back to the manufacture workspace, and notice that all of our toolpaths are now marked with a red exclamation point. So if we go to Actions and Generate we'll recalculate all of these tool paths, and most of them will generate relatively quickly. Any of them that are rest machining will take a little bit longer. And now we need to make sure that chamfer mill tool path is going to be okay. So let's go back into Setup. Let's make sure that we modify chamfer one. We're going to come in here and change the extension of the tip because, again, this is exactly an 0.0625 deep chamfer mill. We're going to reduce this a little bit, and we're going to set this at 0.055. So it's going to be deeper than the actual chamfer, but smaller than the actual edge of the tool. So now, with those modifications in place, let's simulate, jump all the way to the end, come back one operation, and let's play through it again. So now you can see that the tool is not flashing red on the screen because the cut is completely within the cutting portion of the chamfer tool. Now let's go ahead and see how we can apply this to the smaller chamfer as well. We're going to go to 2D Chamfer. Again, we're going to be using the same tool. And for geometry we'll select the upper edge. Then again, in Passes we need to be mindful of our geometry. We're going to set the chamfer width to 0 because it is modeled in this part. And then the tip offset, this is going to be real important, because we're so close to the wall on this part we need to be mindful of how close we are. So I'm going to set this at 0.0625, which is the exact depth of my tool, and I'm going to subtract 0.02. This will allow me to keep the tool as far down as possible into that pocket and as far away as possible from the wall. There's also a chamfer clearance amount, which will ensure that the tool doesn't get any closer than point 0.0125 to the surrounding wall. Then we're going to say okay. Once it calculates will select setup one and we'll simulate it. Again, I'm going to jump all the way to the end, then I'm going to jump back one operation, and I'm going to play through. So the tool comes down, it's not intersecting any of the walls, and it moves its way back up. If we modify the parameters inside of here we can go in and we can add a small amount of linking. So again, we have a horizontal lead in. We can set this from 0 to be 0.05. And that way it'll allow the tool to enter the geometry, and you'll notice as soon as we do that, it's no longer cutting this back edge. It's not able to get in there and stay close enough to that wall and still cut that geometry. So even minor changes in the toolpath parameter can have an effect when we're this close to a wall. One thing we can do is we can reduce the clearance amount of the chamfer. So instead of 0.0125 we can make it 0.005, still leaving a small amount of clearance, allow it to calculate, and see if the tool is able to get into that corner. If it still isn't, we'll need to go back and manipulate some of our linking parameters. We can manually give it an entry position and say that we want it to enter over here. And we can reduce the horizontal lead in, giving it a much smaller amount, and then we can say okay. And now you can see we've told it exactly where we want it to start the cut, and now it's able to get back against that wall. So let's go ahead and select set up one, simulate it one more time, just to be sure that all of our settings are okay. Then we'll play through this. Noting that it is coming in in the spot we specified, with a small amount of lead in, and it goes around and it cuts that chamfer just fine. With the chamfer cut we can now create a pattern of it. So we're going to go into Setup, we're going to go into New pattern, and we're going to be doing a circular pattern. The axis is going to be again here, but notice in this case that we didn't preselect that chamfer toolpath. Nothing is preselected and nothing is showing on the screen. In order for this to work, we want to make sure that we preselect that chamfer toolpath, go into Setup and select New Pattern, and now we can still see it on the screen. We're going to, again, use circular. Just select one of our circular references. We're going to increase the number of instances up to 8. And again we do have this order by tool option. So if we were doing the chamfer as well as the contour for cutting that pocket at the same time, then we would be able to order it based on those tools. So now we have the circular pattern of that chamfer. Let's go ahead and select setup one. Let's simulate everything jumping all the way to the end. And I'm going to turn off the model, so I'm only looking at the stock on the screen. I'm going to rotate this around and just ensure that all the chamfers have been cut. So everything looks pretty good here. We've got the chamfer on the upper edge of that mounting boss. We've the chamfer on all of the different pockets. We've got all eight pockets cut. The last thing for us to do is going to be drilling and tapping that center hole. So let's show our model again. Let's navigate back to a home view and let's save this file before moving on to the next step.
