In this lesson, we'll complete a process plan for milling. After completing this lesson, you'll be able to modify a process plan and identify critical datums on a drawing. In Fusion 360, we want to begin by opening the supply dataset optical pick-up. You'll notice that there are several operations already in here including some facing, contouring, adaptive, as well as a bore operation. We've created most of these in previous lessons but we're starting with a new file and we want to begin to understand how we can modify this based on a detailed drawing and creating a process plan. In addition to this, we also want to open up our optical pickup finishing drawing and this is a PDF file, as well as our process plan sample which is a spreadsheet. Taking a look at the detailed drawing, you'll notice that we have more information than we had previously when we started inspecting this part. You'll notice that there's information about the diameter of certain areas, especially this counterbore in this tapped hole. You see here that it's a 375 hole and it's going down an eighth of an inch before it goes to a quarter 20 tap that's going down three-eighths of an inch. We can also see information about the quarter-20 through holes which we pretty much assumed based on the measurements that we had from an earlier lesson. One thing as we're looking at this detailed drawing is we'll note that it does have some G, D, and T information. It has datums referencing A, B as well as C. While it has these datums, it doesn't have any feature control frames which are dictating a specific tolerance to a location of a hole or the size of a feature based on these datums. While it does have some information on it, it's not a complete picture of any tolerance or references that we need. We do however see that it does have aluminum 6060-T6 in there. Now looking at this, this is likely an error that we would see on a detailed drawing, somebody manually typed in the material rather than bringing it in directly from properties on the part. As we look at this, we have some information but again, it's not a complete picture. Everything we've done so far has been pretty good referencing this, but I do want to take a moment to understand a little bit more about what these datums might be telling us for our part setup. When we see datum references on a drawing, these are going to typically help us control a specific tolerance for location-based features. For example, if the distance from this edge to this hole, this 0.313, had a feature control frame, it would likely be referencing a tolerance based on this datum A. What this does tell me is that when I'm setting up my coordinate system for this part, if I have this information at the start, I would set up my x coordinate on this A wall, my y coordinate on this B wall, and my z would be based off the bottom of the part. If you remember when we started talking about this part in Fusion 360, we mentioned that the bottom was faced and the holes were tapped so we were using a fixture. But when we take a look at this, we have set our z at the top of our stock and this means that if there's any variation in what that top of the stock is based on how it was faced, we're not going to get a consistent thickness on the bottom of our part and likely some of the depths that we're dealing with coming down from the top are not going to be correct. When we take a look at this in Fusion 360, what we would want to do is we'd want to modify our setup and we would want to set our z coordinate based on the top of a fixture. This could also be true for setting it based on the location of a hole if we were using a hole location as a datum reference. We would want to set it on the fixture at that hole and then we would be able to control the tolerance values to other specific features. When we talk about tolerance values for things like wall thicknesses or parallelism, generally what that means is we need to tailor the approach of our operations to minimize the amount of deformation that's going to happen. This might be in the way that the part is held. If it's held on a vise or a fixture, the locations of those holes and how it's held might be critical to add, for example, a dowel pin, a tapered pin that would help make a firm location for where everything is because there's going to be some variation in the tolerances and the threads and the holes that are drilled in a fixture. But also when we're thinking about things like controlling wall thicknesses, we would want to take smaller finishing passes and not be as aggressive. The good news is that when we're using these adaptive operations, these are going to keep that consistent load on the tool so we're going to see less deformation than we would with, say, a pocket operation. We also want to take a look at our process plan and the process plan is not an industry wide thing. When we talk about process planning, generally what we would see is a list of operations, tools, setups, and any additional nodes that we might want based on these operations. The process plan would typically happen before we start creating these operations. We would see a detailed drawing, maybe we'd have a 3D model, and then we will begin to plan out how we want to machine it. You'll notice that inside of here, Operation 1 is listed as face and it's a tool number 10 a half-inch flat. If we take a look in the browser, we have a facing operation. Then we're doing a rough and finishing on the outside with that half-inch, then we're doing an adaptive clearing on this pocket. You can see here that rough and finish, external contour, then rough square pocket, adaptive clearing down to mounting pads. As we go down, then we're doing the adaptive clearing, again, going down to the base and finishing the floor. Then as we go down the list, you can see that these operations are all in line with what we've done. We're finishing the round pocket with the boring operation and then we have this last operation, the 2D contour which is a pocket pass through. But now we need to figure out what else needs to happen. In order to do that, I'm going to simply come down, select that last 2D contour, and take a look at what we have. Again, we're assuming the bottom is faced and these holes were tapped. This pocket over here is done. However, we still need to face down the top of this boss, we need to cut all the pockets in the base, and we need to chamfer their edges. We also need to do the counterbore and drill and tap that blind hole. If we go back to our process plan, these are the types of things that we would want to add in: Operation 12, in this case, the next thing that I would do is face the mounting boss. This is going to be Setup 1 and again, I'm going to use that quarter-inch flat. This is tool number 8 in my tool crib and if we want to, we can make a note but this is pretty self-explanatory. The next operation that I would do would be to counterbore that hole. I'm going to set this as counterbore. Once again, I'm going to use that quarter-inch flat which is tool number 8 and this is all going to be inside of Setup 1 because we're not re-orienting the part. In this case, I'm going to counterbore for mount and that's just going to be my generic note that's put in there. The next thing that I would likely do after we counterbore that hole is to take care of maybe the big chamfer on the outside or maybe drilling and tapping. In this case, we could also think about what else we can do with this quarter-inch flat. Maybe moving on to chamfering and drilling is not the right option right now because we can use that quarter-inch flat to machine out those pockets. The next thing in this case, we'll do the small through pockets and in this case again, Setup 1, carry on using that quarter-inch flat. Because we're making this process plan, this doesn't necessarily mean that we have to follow it 100 percent. We might decide as we begin programming the order of operations might need to change. In this case, I'm going to put a note in here to pattern that feature. You can also see that as we go down, some of the things are not being centered justified anymore so if we have to make any formatting changes, make sure that you just go back in and make the adjustments or changes so that way everything can remain centered. The next thing that we want to do after those pockets is start the chamfering operations. I'm going to start with my small chamfers and then move on to the big chamfers. Again, it's going to be Setup 1 and this time we're going to be using an eighth inch chamfer mill so I'm just going to put C-H-A-M-F and again, this is going to be in Setup 1 but this time it's going to be tool number 5 and this is all based on the tool library that we're using. I'm going to put information about the chamfer that we measured or that we pulled from the detailed drawing. This is going to be 0.02 and it's going to be by 45 degrees. Then I'm going to move on to the next operation which will be my big chamfer. This is going to be on that mounting boss and I'm going to try to use that same chamfer mill. Again, I want to minimize the tool changes so I'm going to try to reuse these as much as possible. Again, based on the detailed drawing, we can pull in that it's 0.0625 by 45 degrees. Next, we'll want to drill and this is going to be a number 7 drill. This is going to be used for that counterbore and this is going to be a blind hole. This is tool number 3 based on our tool library and I'm going to just simply put a blind hole in here. Next, we're going to tap the hole and this should be our last operation and this is going to be our 1/4-20 tap and this is tool number 4. I'm going to put in a note based on the detailed drawing that it's 0.375 from top of boss. This is important especially since we're doing a blind hole, we want to make sure that we don't take the tap down too far and engage an area where we haven't drilled. Now that we've created this process plan, it's really just a map of what we want to do in order to finish the part. There's really nothing else that we need to do with this process plan except for use it as a reference. But from here, let's go ahead and make sure that we save any changes in the design before we move on to the next step.
