In this lesson, we'll be creating a 2D adaptive clearing toolpath. After completing this lesson, you'll be able to; create a 2D adaptive clearing toolpath on open and closed pockets, inspect machining time and modify toolpath perimeters. For this next lesson, let's go ahead and upload the file, open and close 2D adaptive clearing. Again, we've already explored some of these toolpaths but we want to make sure that we practice them over and over again and take a look at some of the settings so that way we can understand how best to apply them to our own geometry. In this example, we're going to be taking a look at the 2D adaptive clearing toolpath for both open and closed pockets. We're going to start by selecting a tool and we're going to be using our Cloud library that we stored for CAD cam specialization and we want to use tool number 10, the half-inch flat end mill. Next in our geometry section, we'll be grabbing this large pocket as well as each of the smaller open pockets. You'll notice when we select them that the graphic on the screen changes a little bit. We're going to move over to heights and we're going to set the height to selected contours. This is going to take it down to the bottom of these pockets here because they're going to be at the same height that we need to machine. In our passes section, right now we have all the default settings turned on but you'll notice that the optimum load is set to 0.2, this is going to be based on the diameter of our tool. So right now we're using a half-inch end mill. So it's taking just below the radius value of that tool. We have some options here to turn on both way cutting and slot clearing but neither of these options will really apply to this specific example. I do urge you to try some of these and we will be exploring slot clearing on another example a little bit later in our courses. As we go down the list, we have multiple depths which we can turn on to make multiple step-downs for our path. However, again in this case, an adaptive toolpath really can take this in one cut without doing multiple steps. A traditional pocketing operation would potentially have two or three steps to cut this geometry. We're going to leave a small amount of stock on the wall and we are going to turn on feed optimization. What this allows us to do is make some adjustments to the feed radius distance and feed rate as we enter or exit material. So you can see that we have a directional change of 25 degrees, and what this does is it allows us to specify the minimum change allowed before the feed rate is reduced. So this allows us to go into areas and as soon as we get into a situation where we turn more than in this case 25 degrees, then it will start to reduce the feed rate because it's starting to engage more material. So again, the entire point of these adaptive toolpaths is to keep a consistent chip load which will increase the amount of material we can remove quickly as well as reduce the tool ware. We're going to go to our linking parameters but again, like in most of our examples, I've left these values stock. I like to do that because first, I know that it'll help me create a toolpath, then I can always go back and make adjustments. For example, to the lead in and lead out values, I'm not necessarily going to know where it's going to enter or exit a cut, so that way I leave these values in here and I can always come back and edit them if I need to. So we're going to say okay and allow it to create this toolpath. What we really want to take a look at and focus on is how it makes the transition between all five different pockets, the four open pockets and the larger closed pocket. So what it's doing right now is it's creating these cuts and you'll see that we have these rapid movements shown in yellow that are jumping between each of them. While this is selected, I'm going to go ahead and simulate it and I'm going to use my cursor at the bottom to manually drag through the timeline. I want to see how it's approaching this and what material is getting left behind in those corners. Then you can see it's coming in to take care of each of those open pockets on the side of my part and everything looks pretty good from here. Because we currently have our original part displayed, you can see exactly the amount of material that's left that 02 on the wall. I want to go back and I want to make a change to this toolpath. Inside of my passes section, I'm going to set the axial stock to leave which is on the floor. I'm going to reset that to zero and say okay. This allows me to come back with a finishing tool doing a potentially a rest machining to clear out the corners and then a contoured to simply clear out the edges where all that material is left behind. So this prevents me from having to come back and finish the entire bottom of the pocket as well. The next thing that I want to do is I want to come back into this toolpath and I want to make some more adjustments. So now I want to start to explore my linking perimeters. So right now the retraction policy is going to be full retraction. Which means that each time it lifts the tool up, it's going to go all the way up to my retract plane. However, we have a minimum retraction option. Again, Fusion 360 is great and the fact that you can just hover the cursor here and get a nice tool tip to tell you exactly what it's trying to do. The minimum retraction amount will move straight up to the lowest height where the tool is going to clear the work piece. So this is going to help us get to other geometry quickly without wasting the tool motion coming too far above the part. We're going to allow for rapid retract which will allow it to increase the feed rate as it's moving away from the part. The way this is going to work as anytime the tool needs to move around it's going to go up in Z first and then it'll move in X and Y. So allowing for that rapid retract, we'll save as cutting time overall. We have a maximum stay down distance and in this case we have one open pocket in the center and then we have pockets on the outside. So this data on this doesn't really help us but in some cases, this actually might prevent the tool from lifting up on the part and moving to another area. So it can be a very handy thing especially if you have complex pockets that you're dealing with in multiple areas inside them. We're going to leave this state down level set to least and we're going to leave the lift height at 0.05. So what this allows it to do is it pulls the tool slightly up and away from the surface as it moves back over to the next adaptive cut. So the reason this is nice is because this keeps the tool from continually re-machining the back face. So as we're making all these small cuts, we're actually going to be cutting the bottom face of our pocket but once it cuts the pocket, it doesn't need to go back and recall that pocket. So having a small amount of lift height even if we take this down to 0.01, will allow that tool to come just slightly up in the Z dimension than slightly back down as it starts to engage that cut again. We also have a non-engagement feed rate which we can increase. For example, if we set this to 50, that'll increase the feed rate as it goes between those movements. Let's go ahead and say okay and let it re-calculate this. What I want to explore now is going to be the change that some of these options make on the overall machining time. So if we right-click on this toolpath and we select machining time, we can see here that our total feed time is about two and a half minutes. We have a feed distance and a rapid distance and the rapid time right now is one second. So it's pretty minimal in terms of the rapid time considering how many small rapid movements we have and the jumps that we have between these parts. However, if we go back in and we make some edits to our linking parameters, if we set the non-engaged feed rate back to something like 25, let's go ahead and take a look at how that affects the overall time. So if we take a look at the machining time, you can see that the rapid time is still about one second. It's really not affecting things too much because we don't have that many rapid movements. So overall this part program is fairly quickly. There's not a lot of material that's getting removed and we're using a fairly large bits so it's doing it really efficiently at this point. So keep in mind that the best option is to start with a toolpath. Maybe leave some of the default settings. Have it generate. Take a look at what it's doing until you get comfortable, then you can go back and make some adjustments to these toolpaths by modifying their parameters. From here continue playing around with this toolpath making some adjustments, see what you can do in terms of speeding up or slowing down the cutting time, so that when you get some idea of what those adjustments make and once you're done with that, make sure you save the file and then we can move on to the next step.
