CNC Mill Tutorial

This is the CNC mill. You can use it to make any projects for your classes or even for fun. I'm going to show you a typical way to set up your stock in the mill. Right now it's mounted to this block. These are called parallels. They're machined in sets so they're perfectly flat and square to each other. We're going to use these to help mount our stock in the vise. So before you put anything in the vise you want to make sure that it's clear of any debris. This just ensures that you have a flat surface to mount your part on. So we're going to put these parallels up at either end of the vise and then we're going to set our stock on the parallels. So the bottom edge is resting on top of these parallels and the edges are going to get squeezed in by the vise. I'm going to put my Mastercam Origin in the back left corner. Once it's in there like that I'm going to use this handle here that's just to the right on this rack to tighten this down into the vise. It's not necessary for it to be overly tight. Next I'm checking that these parallels are stuck underneath it. See how they can move? We're going to use this rubber mallet to hammer down the stock so that those parallels can't move underneath it. Now they're not moving. That ensures that the stock is completely flat in the vise now. Now that your stock is in the machine you're going to have to tell the machine where the stock is located. To do that I use the edge finder tool which is located in tool 4 over here. I want to bring it up into the spindle so I can use that. To do that I need to do an automatic tool change. The door of the machine needs to be closed for it to do this. Then I'm going to get into the correct mode or menu to move this over. These buttons here I call motor menu buttons. That'll get you into the correct mode in order to do a tool changes or to move the table around. This MDI DNC button, MDI stands for manual data input, will get you into their correct mode to move the tool. Because it's several tools away from where we're located now I'm going to type in the tool number. So a T for tool, 4 for the fourth slot. After you do this you press ATC, forward or reverse will do the same thing, and ATC stands for automatic tool change. Alright so now the edge finder is in the tool slot. I'm going to show you really quickly how to take the tool in and out. There's a button right behind this that you press to release the tool. When you press it the tool will drop out of the spindle so make sure you're holding on to it. This here is the edge finder tool. See how the tip of this can move back and forth? How this works is it's going to be in the spindle, it'll be rotating, and this will be wobbling around. You're going to bring your stock in close until it hits this edge finder and then it'll push it to go concentric with itself and it won't be wobbling anymore. At this point you're going to go really slowly and bring the stock in even closer until it bumps off to the right. That's when you have found the edge of your stock relative to the edge of this tool. You need to tell the machine where the center of this tool is over the edge of the stock because that will be the center of every tool in the machine relative to the edge of the stock. To do this you have to compensate for the radius of the tool which is 0.1 inches and I'll show you guys an easy way to do that. First you have to put the tool back into the machine. Hold it just like this sort of like an ice cream cone. Some tools have more to hang on to but in this case you can just rest it on your hand. You're going to want to line these notches up with the pegs and the spindle. The machine will grab onto the tool even if you don't have those notches lined up but you can risk throwing the tool if the spindle turns on so you want to ensure that it's lined up correctly. Also it will grab onto the tool if your fingers are in the way so make sure they remain underneath because it's going to grab onto this upper lip here. So line up the notches, press the button, when you release it it will pull it into the spindle. Just like that. Now that the tool is in the spindle we're going to need to move it into the location to start finding that back edge of the part. To do that I have to get into a different mode. I'm going to go right to this handle jog mode that will let me move the table and spindle around. Next to that handle jog is the increments at which you're moving it. We just start at this .01. That's about as fast as we move so we don't risk crashing the spindle into anything. Now over here you have your X, Y, and Z. Plus or minus doesn't matter but you'll determine the direction with this dial. So X moves the table left and right, Y moves the table forward and backwards, and Z moves the spindle up and down. So I'm just going to move it till the edge finder is right behind this stalk here. Now that the spindle's in a good location to start I'm going to start the spindle up moving. An edge finder works best at a thousand RPM however the door of the machine has to be closed if you're running at over 750 RPM. Because it's easier to see what's going on with the door open we're just going to run it at 750. To do that I type in 750 to this keypad and then I press clockwise CW to start up the spindle. Since this is already wobbling you don't have to flick it but if it was concentric to start with like that you just have to reach in and flick it so it starts wobbling. Keep in mind this is the only tool you're going to touch when it's spinning. Now that it's all started I'm going to bring it in in the Y direction. Since I'm close I'm going to go down one increment lower just so I have more precision. It's starting to go concentric now. Now I'm going to go slower until it just steps off like that. I'm going to stop the spindle here with this stop button right next to clockwise that started it up. Now that you've found the edge of that part you're going to want to tell the machine where that zero is. To do that we're going to want to switch into this work zero offset menu and work in this G54 line here. To switch to that menu you're going to press this offset button and that'll highlight this menu we're working in. We just zeroed it in the Y direction so I'm going to use these cursor arrows to make sure that yellow box is in the Y axis and in the G54 line. Now I'm going to use this part zero set button and that will zero it out where that tool currently is. So you can double check in this work G54 and Y that's all zeros now because we just zeroed it there. Now we have to compensate for the radius of the tool. An easy way I like to do this is to just bring the spindle up away from the part and then bring it over in the Y direction until that is 0.1 and then double check that the tool center is over the edge of the part and not further away. Now that I have this new zero where the center of the tool is over the edge I'm going to go back into that Y axis and re-zero that with this new position. That's how you compensate for the radius of the tool. The same process will be used for the X direction. We're just going to bring the edge finder over to this side and find off of this edge here. The only difference with finding the zero on this edge is that when the tool goes concentric and breaks off it's going to break off towards the back of the machine instead of towards the right like we did on this back edge. That's going to make it difficult to see if you're looking at it straight on. So what I like to do is when the tool goes concentric I stick my head in the machine and with one hand keep moving the dial but be looking at it from the edge so you can see it break off easily. Now that we're in position I'm just going to start the spindle up again, make sure it's wobbling, and then start bringing it in with a smaller increment. Now that it goes concentric I'm going to look in and make sure it breaks off. Right there it broke off so now I'm going to stop the spindle and then zero this new position in the X. So I'm going to make sure I'm highlighting that X axis and then part zero set. Now just to compensate for the radius of the tool make that 0.1. Now that you've compensated for this radius I'm just going to zero over that X in this new position. Now that you have both your X and Y zeros set you have to set the Z zeros for every tool you're using in the program. This just tells the machine where that tool is just going to start cutting into the top of your stock. So to zero in the Z direction you're going to have to change tools to one of the first tools you're using. So before I let it do an automatic tool change I always bring the spindle away from the part to make sure that it has clearance. Then I'm going to shut this door so it can do the tool change. Now get into the correct mode and then we're going to want to go to tool one. So T for tool, one for the first tool. To zero a tool we use this paper test. We're just going to put this down on top of the stock, bring the tool over and down until it's right above this paper, and then slowly move the spindle down. It's not going to be moving at this point. And move this paper around until you feel the spin the end mill dragging on that paper in the stock. Not so much that you can't move it but just a little less so you feel quite a bit of friction. Make sure you get in the correct mode to move the table and spindle around. Sometimes with the paper test it's necessary to use the very smallest increment. Now that I've found the top of that stock I'm going to tell the machine where that location is. Up here in this tool offset menu spindle is next to number one which is the tool that we're currently using. And then in this geometry column is where you're setting your Z zero. If this isn't highlighted with the yellow box just use the cursor arrows to get over to that box. Then press tool offset measure and that will zero that in this new location. This process needs to be repeated for every tool you're using in your program. A shortcut to switching just one tool ahead is to be in this correct mode and then instead of typing the next tool ATC forward will take you one tool in the next direction and ATC reverse will take you one tool back. I found that top of the stock. Now spindle is next to two because we're in the second two. Go ahead and zero that out. Now that I have zeroed all the tools that we're using you're essentially ready to start running your program. So before it runs I always bring it away from the stock. Now that everything is zeroed you're going to want to put the program into the machine. Your G code from your Mastercam file should be saved on a USB drive. To learn how to make this G code reference the Mastercam tutorial video. Insert the thumb drive in the edge of the machine and then to bring it up I'm going to use this list program button here. That'll get me into the correct mode. Currently I'm in the USB device. If I wasn't and I was over in memory you would just use your cursor arrows to come up to the top tab to move back and forth. I'm going to select my file. It should have the .nc extension not the .err. To bring this file up I'm going to press select program and that will grab that file. Before you run your file you're going to want to do a settings graph of it to make sure everything looks correct. To do that you're going to press the settings graphic button twice and then the cycle start green button to step through the file. It's going to show up on this screen here all of your tool paths. The X's mark where holes are being drilled. Dashed lines are rapid motion and solid lines are cutting paths. If everything looks correct on your program then you're ready to start running it. To do that you're going to press this memory button here. That'll get you in the correct mode to run the program and then you're going to press the green button to start it. You'll press the green button after it changes tools and waits for you to confirm and then you're going to want to make sure your thumb is ready over the speed hold button in case for some reason it does a tool path that doesn't look correct you could stop it. If it's heading towards the vise you can stop it. If it's going through one of your mounting screws go ahead and stop it. If you wanted to clear chips off the part or see what was going on go ahead and stop this button here. That'll just stop the table and spindle from moving around. The spindle will still be spinning so it won't let you open the door unless you use stop to stop the spindle. It's no big deal to press this button. The green button will just start it right back up from where you left off. If for some reason the part gets pulled out of the vise and is stuck on the spindle you're going to want to press the emergency stop button or for any other situation where you feel uncomfortable with what's happening. It's not possible to restart your program in the middle if you press the emergency stop so it's better to use feed hold but always know that that button is there for you. So now it's ready to run the program so just start green to start it up. Now I'm going to push the green button because it changed tools into the first tool you're using. Here you can see it's stepping through your g-code. Also pay attention to your spindle load here and this will report the feed rates and the spindle speed to you. Rapid motion is set to 50% on this machine max but if you feel uncomfortable with how fast it's moving between changes you can step this down to 25% or even to 5%. Now that it changed tools it's waiting for me to confirm. Also this green light will be blinking. I'm just gonna press the green button now to confirm that that's the correct tool. Now that your part is done you're gonna want to move it so it's easy to get out of the machine. Right now I've moved it to the center of the machine. Go ahead and open the door look in and double check that everything looks correct on your part before you take it out. If everything looks good go ahead and grab the compressed air. Close the door almost all the way on your arm so you don't blow debris into your face or around the shop. Go ahead and blow your part off and take it out of the machine. And there you have it a completed CNC part.