In this video, we'll create a tool library. After completing this step, you'll be able to modify user preferences to enable cloud libraries, create a new cloud library and modify tool parameters. Infusion 360, we're going to get started with a new untitled document. First we want to go up to our user preferences and make sure that we have cloud libraries enabled. You can find this in the general manufacturer section as a checkbox. Once we ensure that those are enabled, we're going to navigate to the menu function workspace. I'm going to change my default units. I'm going to set this two inch for this design, and then I want to go to Manage and Tool library. Inside of here, if we have enabled Cloud Libraries, we should now see Cloud and Local. Inside of a cloud, we're going to Right Click and create a new tool library. I'm going to call this one CAM DFM or CAM designed for manufacturer. Notice that, there's no data in here. Now, inside of the tool library we can either create new tools or we can copy them from the fusion 360 library. To do that we're going to get started by left clicking on the fusion library. Going up to the right, first we're going to filter by whole making. When we take a look at whole making, we want to look for a spot drill and then we want to identify an eighth in spot drill. We're going to select the eighth in spot drill and notice at the bottom we have a lot of different cutting data. This doesn't matter at the moment for us. Really we need to Right click and copy the tool, then navigate back to our CAM DFM library and paste the tool. We're going to select it, right click and edit. We're going to change the post processor data because we want this to be tool number one. It changes both the length and the diameter offsets as well. In the general section, the description eighth inch spot drill is still fine. In the cutter section, we can modify any parameters that we need. Inside of here, this has the number of flutes, the diameter of the tool and how far it's sticking out from the holder. You'll notice that, this is a relatively small tool and a large standard cap 40 holder. That's okay for this example but note that we do want to make sure that we replicate the holder based on what's actually holding our tool. There's information about the holder and we can select another one, such as a drill chuck if needed. And then there's cutting data which determines how fast the RPMs are and how fast the tool is going to be moving. In this case, I'm going to reduce the spindle RPM, which is a rather large number. I'm going to set this to 5000 RPM. When I do that, notice that it modifies some of the other values. Right now, it's set to feet per minute. You'll also notice that there are vertical feed rates. Since this is a spot drill, it's not going to be moving in the X and Y, it's simply going to be moving vertically. Right now the plunge feed rate is set to 21 and the feed per revolution is set to a relatively small number. We're going to set the feed rate to a smaller number. So this plunge value instead, it's going to be four inches per minute and the retract rate will leave at 21. Notice that when we change the plunge feed rate, it automatically changes the feed per revolution because this is linked based on the back end parameters. From here, we can accept the change and now we need to continue to populate our tool library. When we go back to the fusion library, you'll notice that everything is still a spot drill and that's because our filter is still active. We can clear the tool category and the filters and now we can take a look at milling or whole making and notice that it changes what we see in the library. We need to add some drills and taps before we get into our end mills. So let's go ahead and look for a number seven drill. We can do this by scrolling through the library or we can use diameter ranges. If we want to use a number seven, we can say that it's equal 2.201, and this brings up a number seven drill. Once again we'll copy and paste it into our CAM DFM library. Again, we'll have to clear the filters to see everything that's in here. Our number seven Drill, we're not going to make too many modifications but we do want to adjust the number two, two, two. We can also modify cutting parameters and give it to flutes. We're going to accept this change and then go back into our fusion 360 library. Now we want to look for a tap, when we take a look at this and we go to whole making, you can see that we have tap left hand and tap right hand. We're going to select the right hand tap and we want to find a quarter 20. We'll scroll down a little bit until we see a quarter 20, we will copy the tool and then we'll go back into our key MDFM and paste it. We're going to edit this tool in its post processor number, and this is going to be tool number three in our library, will accept the change, again, we'll clear those filters and make sure that we have tools one two and three. And we'll go back to our Fusion 360 Library. Now we want to find a flat end mail which will be in the milling section and will filter by flat end mill, in the sample tools inch section we're going to be looking for an eighth inch flat end mill. We're also going to do this for a quarter inch and a half inch, but we're going to do these one at a time. I'm going to copy the tool and paste it into my library, and then I'm going to go back, grab the quarter inch and we'll do the same thing for the half inch. Now I can modify their parameters and set their tool numbers, in the post processor section are eighth inch is going to be tool number four, our quarter inch is going to be tool number five. And then our half inch is going to be tool number six. Then we'll go into our filters and let's go ahead and clear all the filters to see what tools we have, right now we have tools one through six, a spot drill, a number seven drill, a quarter 20 tap, an eighth a quarter and a half inch flat end mill. Now that we have these in here, we can go ahead and modify some of their parameters. We're going to right click and edit the tool and go to cutting data, inside of here on the left hand side notice that there are various parameters based on what you're doing with the tool. If we go down to a low carbon steel or brass, you can see that it changes the feed rates. We're going to be using the quarter inch and eighth inch for finishing operations. So we want to make sure that we take a look at the aluminum finishing, right now, it's spinning at about 12,000 rpm and we're actually going to reduce this to 10,000 rpm. When I do that, it automatically changes some of the other values. And we're going to go down until we find the feed per tooth, we're going to change this 2.002. When we do that, it changes the cutting feed, because it's based on those parameters, we're going to accept those changes and we'll take a look at the quarter inch next. We're going to go to cutting data and once again, we want to take a look at aluminum finishing. Inside of here we're also going to change this to 10,000 rpm. We're going to take a look at some of the other parameters. In this case, we're looking at a feed per tooth of 0.004, and then we want to take a look at some of the values for lead in and lead out. You notice that these values are rounded right now, I'm going to set them to 120, and for the ramp feed rate, I'll do that at 120 as well. We can also modify values for things like the plunge feed rate, in this case plunge we're going to set to 30 and then we've got passes and links and these other values that we're using here. We can also modify various parameters for the tool itself. For example, if we want to increase it to four flutes and change how far it's sticking out of the holder. We can always come back and modify these later on as we're using them. Last, let's make some adjustments to the half inch end mill. Under the cutting data, we're going to go into aluminum roughing since this is going to be a roughing tool, we're going to modify to make sure that we're using 7640 for the rpm and we want to take a look at the FPT or feed for two. Right now it's set to 0.005 and we're going to adjust this 2.008. Everything else I'm going to leave as is but I do want to modify the cutter and note that it is a four flute and accept the changes. There are a few more tools that we need. So we'll go back into our filters for milling. We're going to look for a ball end mill, and this is going to be a quarter inch ball end mill. Once again, we'll copy the tool, go into our CAM library and we'll paste it, will modify its parameters after we find the rest of our tools. Now we're going to be looking for a face mill. We're going to take the two inch face mill sample, we're going to copy this tool and we're going to paste it into our camp DFM library. The last thing that we need is a chaff mill and this is something that we're going to have to make custom. So inside of here let's first modify our tools. The ball end mill that I grabbed, I actually want to be a bull nose mill. So if I edit the tool, I can go into the cutter section and I can actually change its profile and make it a bull nosed mill. I then need to make sure that I modify its parameters. This is going to be four flute, it's going to be quarter inch diameter but the radius value for the corner is actually going to be quite a bit smaller. We're going to get rid of all the decimals that are in here and we're going to set up the corner at 0.015. This will allow us to create a small filets on the bottom of any of the features that we machine with this tool. This is also going to be tool number seven. We do want to go into the general and we want to change the description since we did change it to a bull nose. So I'm going to change it to a bull nose end mill, and I'm going to put a note about the corner radius 0.015, that way when we're looking at this in our tool library, we know exactly what value it is. Any time it's showing up in our tool library like this, it's missing some required data, when we take a look ,and we go through everything looks okay in here. But in the cutting data sometimes you'll note that it might be missing some information. You'll note here that in aluminum roughing and finishing, it's missing some of the data, it's not specified. I'm going to turn these options off, which means that I'm going to be using the values that are inside of my tool path and not using the ones from the tool library itself. It still says that it's missing some data but that's okay because we're only going to be using it for some of the cutting data, not all of it. We're going to be focusing on the aluminum values for roughing and finishing. Lastly we're going to change the tool number for our face mill before we get in and we start creating our champ for mill. The face smell is going to be tool number eight and we're going to accept that change. In order to create a new tool, we need to hit the plus icon and determine what tool we want to create. In this case, we're going to be looking at creating a champ for mill which is under engrave slash champ, we're going to go to our cutter section and we want to define this as 45 degrees. I'm going to change the number of flutes to two, we're going to be using the inches and high speed steel for material, and then down in the diameter, we're going to set this at a 0.25 diameter. The shaft diameter is also going to be 0.25. Then we need to define the other values, in our case, the inclusive angle is 90, the taper angle is 45, all that will be fine. And we need to make the tip diameter a little bit larger, right now it's set to zero, which means it can be used as a grave tool, we're going to set it at 0.125, when we do that, it gives us a flat section at the bottom and it gives us the chamber on the side. Everything else is going to be fine in here. I'm going to reset this to tool number nine. Then we're going to accept it, noting that we can come back and make adjustments to these at any point in time. Everything looks pretty good, and since this is a cloud library, I don't need to make any saves, the document is unsaved because we change the units but that doesn't really have any effect on a tool library. We can always come back in, go to our tool library and make any additional adjustments needed. From here, make sure that you have played around with all the different various parameters and settings and search through the tool library and then we can move on to the next step
