In this lesson, we'll be completing 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. For this next lesson, we're going to be taking a look at a few files. First, we want to get started by uploading the file optical pick up. This is a continuation of the file we saw earlier in our lesson where we program some of the tool paths to cut this geometry. We were dealing mostly with tool pass for thin walls and spring passes. Now, we're going to complete this part by programming the rest of the features. We also want to make sure that we open two more files. We have a PDF drawing for this part, as well as an Excel spreadsheet file for process plan. We want to focus on process planning this part and figuring out what the rest of the operations need to be. The process plan has been started for us and it's identify the operations as well as the tools used in those operations. This process is not the same throughout all industries. Some places will require a more detailed process plan. Some industries won't require a process plant at all, and some will require a really specific one based on that industry. We're going to be looking at the process in general and understand the steps that are involved here. The first thing that we need to do, in this case, is identify the rest of the tool paths. We need to identify certain features on the drawing that may or may not require some additional assistance. Now the detailed drawing that we're looking at here doesn't have tolerance values on it, it doesn't have all the information that's, in this case, required for a high tolerance part. Things like GD&T notes for parallelism or flatness, but we do have some datum references. We can see on the screen that we have A, B, and C. And we want to make sure we identify these and help us understand when we're programming this part. What we should be referencing when we're doing things like drilling holes or maybe even putting it into a fixture or clamping it into a vise. So what we can see here is that our first reference is going to be this side wall. Our second reference is this longer side wall. And then the third reference is the bottom of our part. When we think about this in terms of holding it in a vice, we should be using the A, datum for our x reference, the B, datum for y reference. And the C, datum for our z reference, if we're dealing with the part that has tight tolerances. Now, our part in the way that we originally approached it was the fact that the four bolt hole pattern is actually drilled and tapped already in the bottom is feast and it's bolted down to a fixture. With this in mind, we've already got it clamped down to a fixture plate which would be our C reference and our A and B references are based off of rough stock. So those aren't going to be really good references either. When we have parts that call out critical tolerance values in reference to these datums, we need to be aware of that when we're creating our coordinate systems and when we're creating our tool paths as well. Because we don't have those references here, we can focus on a few more things. In this case, some of the areas we still need to finish off or going to be the top of this mounting boss in the circular region, the eight pockets as well as drilling and tapping this whole. So the notes on the drawing that are going to help us with those are going to be first off this note in the upper left-hand corner. And this tells us that the diameter of the counterbore is 375 and the distance down is 0.125. And below that we have a quarter 20 tapped hole that's going down 375. When we look at these references and we take a look at the drawing and the section view, you can see that this whole doesn't go all the way through. It does have a drill point on it and the total height of it from the bottom is half an inch. So if we think about these as we're looking at the part here, they're going to help us identify a couple things. First off, the specific diameter and depth of these features if we didn't have the CAD model to go off of, as well as specifics about like the chamfer. We can see that the chamfer on this section is 0625 and it's a square chamfer. And then we have the one on the smaller pockets is actually going to be a 0.02 x 0.02 or 0.02 x 45 degrees. So again, these details help us identify things like exactly what we should be using in terms of tools and geometry as well as any critical features. Let's go back to that process plan and let's take a look at the last couple rows and things that have not yet been identified. So if we take a look at the part and I'm going to go ahead and move this over to the right side of my screen. If we take a look at the part, we can see that we have are facing operation, which is number one in our process plan. Our contour which is the outside with the note external contour rough and finish, our adaptives which are clearing out the square pocket. Then we have contours to finish off that pocket. Then we have a contour for the outside upper edge for our lip. Then we start to clear out the circular pocket. We finish off the ID portion, we finish off the OD portion. Then we create a contour operation for that small pastor. So at this point in time, if we were to select set up one, go in to simulate and simply jump all the way to the end, you can see that the areas that still need to be machine or going to be the top of this boss here. We need to take it down to the appropriate level. Then we need to add the counterbore, the tapped hole, and the chamfer on it. Then we also need to handle those smaller pockets in the small chamfer on those as well. So with this in mind and knowing exactly what we've already done and what we still need to do, we can plan out the rest of our operations. So the next thing that I would do here for operation 12 would be to face the top of the boar. So under operation, I'm going to use just standard terms and I'm going to call this one face, Mounting boss. This is going to be in set up one because it's all going to be coming from the same side. And I'm going to continue to use the same tool that's already there. So this is going to be my quarter inch flat. This is tool number eight inside my tool turret and I can add any additional notes here If I feel like they're needed. The next operation is, we would continue on with that tool and we would do a counterbore. Now, there are a couple things that we need to be aware of here when we start to think about this specific geometry. Does it make more sense for us to drill that hole first so that way we have an entry point? Or can we actually just take that quarter inch end mill in there and create that counterbore? In this case, I'm going to go ahead and take care of that counterbore. So I'm going to simply call this counterbore, still in set up one, still using my quarter inch flat, still tool number eight, and we're going to go ahead and just add a small note here. Counterbore for mount. Then the next operation at this point is going to be, again, if we need to continue on with that tool, or if we want to induce a tool change. Since I want to keep that tool, I want to continue to move on. I'm going to go ahead and start machining out those small pockets. So I'm going to start with, Small through pocket. Still set up number one, I'm still going to continue to use that quarter inch flat until I need to do a tool change. And, in this case, I'm going to put a note pattern feature. So this is going to allow me to create the tool path for just one of those and pattern it eight times. Now at this point, we need to think about whether or not we're going to create a tool change. Is there another thing that we can use as tool on or should we go ahead and change tools? And if we change tools, what are we going to change too? So if we're going to add a pattern feature, it might make sense for us to start with the chamfer and mill. That way we can chamfer the small edges as well as the large edge on the mounting boss, then we can pattern that chamfer as well as the pocket. So I'm going to call this one small chamfers, And I'm going to do one after that big chamfer. These are, again, going to be instead of one and at this point in our tool library, we have an 8 inch chamfer mill. And then this is going to be if we reference our tool library. We can take a look and we can see that this is tool number 5. So we'll make sure that this is tool number 5. And I'm going to put a note of 0.02 x 45 and the one below it 0625 x 45. And again, we're going to reutilize those tools. And the point of this is to make sure that we're not having a bunch of tool changes unless we need it. I'm going to go ahead and make sure all in here is going to be centered, even though the formatting was set to standard, for some reason, doesn't seem to want to center the information. We'll spread this out so we can see everything. And now we have our small chamfer and our big chamfer. These are going to be, again, all in set up one and we're going to be using the eighth inch chamfer mill which is tool number 5 and then I've got some notes about the size of this chamfers. So at this point, the last thing for me to do would be to drill and tap that quarter 20 hole. So I'm going to call this one drill, I'm going to call this one tap. Both will be in set up one. The drill is going to be a number 7 drill. And the tap is going to be a quarter 20 tap, so we'll do a quarter 20. And if we take a look again at our tool library, we can see that we have a drill bit and we have our top, drill bit is number 3 tap is number 4. So inside of here, the drill be tool number 3, the tap will be number 4. For the tap, I'm going to go ahead and I'm going to put in a distance of 375. And, I'm going to put from top of boss, that way, I can remember exactly what the depth is. You can see that it actually tried to put that as a date in here. So we'll need to go back in and we'll put the inch designation, make sure that we have a -20, so now it's representing quarter 20. A lot of times when we be doing this process, we would either have something to reference in terms of the part or the detail drawing. In the best case scenario, you have both, you have the detailed drawing and you have the part to reference if you need it. In our case, we do have both, but if we just have the detailed drawing, we would look at it. We would take a rough guess at what the operation should be, and this document is essentially a living document. It can change, there's nothing that says that this has to be exactly how it gets machine as you start programming apart. You might identify some things that you can do differently. Maybe you can utilize a bigger tool on some other operations. For example, we could decide to face the boss at an earlier time. Maybe when we go in and we do the roughing for that pocket, we could come in and face it as well in an individual step. That way, we could use that half inch tool rather than the quarter. But again, the process planning can grow and change a little bit as we go but at least right now we've identified all of the geometry and all the areas that we actually have to machine. And now we can go back in and we can try to apply this to our part to finish off the rest of the tool paths. Make sure that you save this process plan and, again, it is just a sample. There's nothing that says this is exactly how you have to do it. It's just an example of a process plan and kind of information that you would typically populate in there. But make sure you save that, make sure that if you've made any changes to the optical pick up part that you save that as well, and then we can move on to the next step.
