In this lesson we'll create a Closed 3D Adaptive Clearing Tool Path. After completing this lesson, you'll be able to: create an adaptive clearing tool path, analyze tool path machining time and modify tool path parameters. For this next lesson, we're going go back to our 3D pocket sample file. We want to navigate to the manufacturer work space, and we're going to go into our model, and we're going to expand and hide the stock body as well as the vice. Then we want to navigate back to our home view. We're going to be focusing on clearing out the inside of this part by using some of our 3D adaptive clearing options. So we want to take a look at this geometry and remember that we have a 2D pocket inside of here, but if we consider that to be a complete plane, it'll actually cut off the top geometry of this dome. So we have to approach this a little bit differently. We can't simply come in and assume that it's a 2D pocket and ultimately mess up some of the other geometry. So let's take a look at using first the adaptive clearing option and how that handles this part. We're going to start by selecting our tool, and we're going to go into our CAD-CAM course two specialization file and use tool number 10, the half-inch end mill. We're going to leave all of our feeds and speeds from this tool, because it's a good idea for you to pre-program all the parameters into the tools that you're going to use. This information is going to start by getting it from your manufacturer. Your tool manufacturer will generally give you recommendations on their specific tools and the type of material you're using. You'll also have to factor in other things such as the machine you're using and its horsepower, the material that you're cutting whether or not it has good or poor machinability, and some other general parameters, like the type of coolant that you're using. The next tab we want to go to is geometry, and by default, it's going to automatically grab the stock contour. This is going to allow the tool path to calculate all the material that needs to be removed from the original stock. We have some options such as selecting a specific bounding box, we can use a silhouette or select geometry on the screen. However, we're going to allow it to use this stock and allow it to just simply do a roughing pass on the entire part even on the outside shape. We're not going to be using rest machining because we haven't done any previous operations yet, so will simply move on to the heights. Inside of here I'm going to leave the default retract, the clearance, and the top heights. However, I do want to change the bottom height. I'm going to use these selection option, and I'm only going to go down to the top face of one of these pads. This will keep the tool above this area and allow it to go down and leave a small amount of stock there. But ultimately on the outside, I want to come out and do a finishing contour on the entire part, and I don't want to have all of this geometry removed at the start. Next, we have our past as section, and there are a lot of different options in here. When you first start out, it's hard to understand and know what all of these options do, so my first rule of thumb whenever starting out is to try all the defaults, take a look at the tool path, to simulate it, and then make some adjustments to these options so we can see exactly what they do. We are going to adjust a few of these and we're going to talk about some of them. But again, there are many options and some of them will work better on certain types of geometry than others, and unfortunately one example doesn't cover all of the settings. Inside of here, we have some options to machine shallow areas which are going to be these small pocket areas around the dome. So we're going to have that option turned on. It gives us additional criteria in terms of step-down and step over, to control the tool motion. You'll see that right now the minimum shallow step down is 0.0039, and the minimum step over is 0.039. We can adjust these values if we want to change them, but again, I'm going to leave these defaults and just see how it looks. We have an optimum load and this is going to control how much material is engaged with the tool. So what this is saying is that we want to engage the tool a distance of 0.2 inches. We're using a half-inch tool so that's a little bit less than the radius of the tool, and this will give a consistent chip load wherever possible. We can use the "Both Ways" option. This will allow the tool to go back and forth while it's cutting, especially for a roughing operation, and this keeps it from jumping up and moving over and coming back to make sure that it's continually cutting in the same direction. We have a "Machine Cavities" option, which again, this allows us to go inside the pockets, and the strategy it does is it allows it to actually ramp and move up and down inside these pockets. This is something that we want to use for this type of geometry. We're going to set the default cutting direction to climb. But we could set it to climb or conventional. But remember we also have this "Both Ways" option, which allows us to go back and forth in climb and conventional milling operation. We have the maximum roughing step down, a fine step-down value and then we have a flat area detection. The flat area detection helps to detect heights such as this flat section right here, and it allows us to detect those heights and make sure that it is machining down to them if it can. So what that means is, if we have a maximum roughing step-down of half an inch, and that for some reason that flat is that 0.45 inches, it'll go down to that flat plus whatever stock we tell it to leave and it'll machine that flat area. So this really helps especially when you're dealing with complex pockets that have both flat and potentially curvature-type geometry. All right, as we're going down the list, again there are more options we can order by depth or area. My recommendation again is to try the stock values, if you're trying to explore these tool paths, see what it looks like and then come back and make an adjustment to one or two settings. They recalculate relatively quickly and we can get a good idea of how it affects machining time, we can simulate it and see how it affects the material removal and surface finish of these operations., so there are a lot of different options we can play with. We are going to have stock to leave and we'll leave 0.02 in both the radial and axial direction, so that way we can come back and finish the floors as well as the walls of our pocket. We're not going to worry about fillets and smoothing options in this operation, so we're going to move on to our linking parameters. For right now, I'm going to leave all of the default settings on because I want to explore how some of these are going to affect our machining time. So we're going to say "Okay" and allow it to calculate. So once this operation is done, we can notice a few things right away. It is machining the outside and the inside of the part because we allowed it to basically calculate from stock how much material is there and how much needs to be removed. We also have a lot of yellow movements which are rapid movements. Now, in general it would seem like these rapid movements would greatly increase the machining time because there's a lot of non-cutting motion going on. However, we're going to explore what some of these changes will do in terms of affecting the overall time, and we're going to make that decision as to whether or not we want to keep all these rapid movements or maybe try to adjust some of the settings to remove some of them. So the first thing that I'm going do is go into simulate, and then I'm just simply going to play through this operation. I do have stock turned on, but I do have the tool path turned off. So this way I'm not looking at where the tool is going or where it's been, but simply the material that it's removing from stock. One thing that we can notice with this operation is around the curvature-type geometry, in this case our dome, you can see that it has these micro steps, stepping back up after it machines that pocket. So this is exactly what we want to see because it removes a lot of material and it allows us to come into a situation where we can do a finishing tool path and not have to remove a ton of material from that geometry, simply because we only had a 2D pocket operation. Let's take a look at this statistics in here and see how long it takes to machine. So the estimate right now is 10 minutes and 25 seconds. We can also see that information by right-clicking on the "Tool path" and going to "Machine time", we can see here 10 minutes and 25 seconds, the feed distance is 227 inches, and then we have a rapid distance of 57 inches. So this is great information because if we come in and edit the tool path, for example, we adjust the option to stay down level and we say stay down most, we say okay and recalculate this. We can see exactly what that does in terms of machining time, how it affects our rapid distance and our feed distances. Because in some cases, we'll have less feed time if we allow it to wrap it up and move over to another location rather than have to feed over to it. So if we take a look at the machine time now, you can see that we've added over a minute by allowing it to keep the tool down. What this does is, it actually changes the amount of rapid distance we have by reducing it, but if you take a look at the feed distance, it's changed that as well. So sometimes these options on the surface might seem like they'll help your programming time and they'll help you're cutting time, but ultimately it's a good idea to always make sure you go back and you check on those to ensure that they are having the desired result. In this case what I'm going to do, is I'm going to turn off this option for this "Stay down level" and set it to "Least". Inside of my passive section I'm going to order by area, allow it to recalculate, and see how that affects my overall program. So now that it's calculated it will right-click and select "Machine time", and you can see that this is actually reduced the time just slightly. Our total feed distance is reduced, our rapid distance is slightly increased, but the overall program time has reduced because those rapid movements are actually not really adding too much to the overall program. Keep in mind that this is a single operation. We don't have tool changes to deal with or we're not navigating to a lot of different areas, but there are many different things that can affect the overall program. For example, if we go into this operation and we take a look at the feeds and speeds, increasing the rpm and the surface speed of the tool, those are both going to adjust how long it takes for us to cut the part. Right now we're spinning this tool at a little bit over a 1000 rpm, but if the machine and the tool is capable of running at 5,000 rpm, and we can add a bunch more speed to the tool in terms of cutting into the material, then we can reduce that time quite a bit. So right now it's estimating that this is going to take about 10 minutes to rough this part, but ultimately with the right tool, the right machine, and the right setup holding this into the machine, we could ultimately rough this thing out in a minute or less. So there are many different ways that we can adjust the overall time it takes to machine these parts. If you're doing a one-off part and you're simply trying to program it, to cut a prototype, this isn't as critical as if you're trying to make a file for a production run. So just keep these things in mind as you start to program, and for right now, let's go ahead and save this file before we move on to the next step and explore some more tool paths.
