Welcome to our second Carvera cutting tutorial. This video is going to be building off a lot of the things that we learned in the previous video. So check that out if you haven't, because you might be missing some important things. This time, we're going to be taking it one step further and carving out a 3D topographical map of the moon, or really any location that you want, on a material of your choice. We're going to be looking at bit selection, roughing and finishing passes, and adding tabs to your project. So let's get into it.

All righty. Starting off, let's choose some stock. We're going to be using some soft pine wood for ours, but if you have a spare block of brass or aluminium or even some ABS, feel free to use that. The idea is that you'll be able to choose the right settings for any material that you are using. Now, the model that we'll be using in our example here is of the Tycho Crater on the moon, which has some wonderful topographical features that look really good in an engraving. The model we're using is going to be designed for a piece of stock 20 millimeters thick and 170 by 170 millimeters, you know, wide in a square. But we will also have a version of this model designed for these different thicknesses and sizes of stock if it better suits your needs. So, pick the one that works the best for you. If you wish to make your own topography that isn't of the moon, you will find plenty of free online resources to generate custom topographical maps like this for pretty much any location on Earth. in the written guide link below. We will have some good free ones and some tips on getting good results if you want to give that a go. I'm just going to say the moon crater is pretty damn cool though.

All righty, let's jump into MakeraCAM and CAM this thing out. We're going to start by doing some three-axis milling. And as always, we're going to go ahead and assign our stock dimensions and materials first up. Then we're going to go ahead and import our model, which you can download from the written guide, which is linked below. Next, we're going to ensure that our model is nice and in the center of our stock and also sitting perfectly flat on the bottom. If we take a look using this box here to, you know, look at it from the side, we can see that it is not perfectly sitting on the bottom. To fix this, we're going to go ahead and select our 3D flat to be on the bottom. And then we're going to hit quick align stop. Now, if we look at it from the side, we can see that our bottom has been nice and aligned to the bottom of our stock. And also, as always, if we look at it from the top, it's nice and put it in the middle of our stock as well. Something we want to check here is that we have a nice rim of stock around our model. We have a little bit of breathing room. That'll give us, you know, some area to clamp down on and not worry about the tool getting precariously close to our clamps or anything like that. The models will give you have a 10 mm gap here, which is a lot of breathing room. It's probably a little bit on the bigger side, but it's fine. But if you've imported a custom model or any geometry or doing another one, you know, ensure that you have some breathing room. Now is when you want to set this up so you don't have to change it later. Now, we're going to need three cuts to make this piece. The first is going to be our roughing cut. This is going to use a big mill bit to remove a lot of the material, you know, really quickly and get us close to the surface of our final model, but it will not have that much detail in it. After that, we're going to need to do a finishing pass on it. This is where we get our little, you know, very fine engraving bit and get in there and carve out all the detail. The roughing pass gets us 90% of the way there and the finishing does that last little 10% where all the detail is. And then our third and final cut will be to actually cut out our model from the stock. So let's start with our roughing cut by selecting a 3D relief. And we're going to leave our cutting depths as usual. Safe positions we're not going to worry about because we have a nice flat piece of stock. We don't need to worry about retracting up our bit or anything. But we are going to need to assign a mill bit. So let's add a tool. And while we're here, let's talk a little bit about bit theory. Huh? How you like that pun? We're just going to go through all the bits on the list and basically explain what they do. because knowing what they do, you can choose it when it is appropriate. First things first, we have our flat end flute bits, also called milling bits or endmills. These are our bread and butter, the ones that you'll be using the most. The things that you need to worry about is the width of the bit, which is the first number here. Wider ones remove more material but have less detail. There's also the effective length of the bit, which is the second number here. This is the actual, you know, length of that sharp cutting edge that's on the bit. And then there's also the number of flutes. Here we have only single flutes loaded into our machine. This single flute means that the cutting tip only has one edge on it. As in every time it rotates, it's only going to take one, you know, scoop or chip out of our material. But you can also get two flutes which have, you know, two cutting edges and take two chunks out per rotation. Four flutes, eight flutes, and on and on. Why one flute? Well, flute theory could have its entire own video, and you should definitely go out and, you know, read a bit about it because it's pretty important to CNC milling to learn what the actual bits do. There's too much to probably answer in the runtime of this video, but long story short, it's more appropriate for the capability and power of this machine. It gives cleaner cuts and it helps with chip extraction, which is where we want to, you know, remove the little bits of material after they've been cut. You'll also see that they're divided into metal and non-metal bits. And this is just obviously whether they're designed to cut metal or non-metal. But the main difference is that the metal ones have a coating that help cut things like brass and aluminium. And they're also a little bit shorter. There's a common issue, especially when cutting metal, called chatter. Essentially, it's when the bit sort of wobbles around while it's cutting. This, you know, affects the quality of your cut and it's not good for the bit and it usually makes a horrible sound. So, metal bits are usually a little bit on the shorter end because a longer bit is easier to bend. Also, under your flat end bits are going to be corn bits, which if you look at them, they look like a cob of corn, hence the name. Now, if you followed the setup manual, you'll actually have one of these in tool slot three. These are really great for cutting composites. So things like carbon fiber and PCBs. The cutting edge just makes it, you know, really effective on cutting those. Under engraving, we have our single flute V bits. It doesn't have the V in the name there, but they are V bits. These are essentially just a V-shaped bit with a very small flat tip on the end. As you can see, we go from 0.1 mm to 0.5 mm. And that is just the width of that flat bit on the end. These are just our, you know, detailed engraving bits that we'll go through on our finishing pass. and really, you know, carve out all that little detail. And these also come in metal and non-metal bits as well. Under here, we also have our chamfering bits, which we, you know, used to add chamfers to edges. When we cut out the ice stamp tray last time, some of those edges might have come out almost sharp. Luckily, they didn't. But if they were sharp, we could be really fancy and use some chamfering bits to go over and just kind of take the edge off, almost as if we'd like filed down that bit with a nice 45° angle. And our last engraving bit is our soldering mask remover, which is specific to PCB making and removes a layer of solder mask. It's a bit of a niche one there. Then we also have our ball-nose bits, which are sort of like an engraving bit as well, but the tip is shaped like a ball, making them more, you know, suitable for carving curvy and kind of natural geometry, rounded shape geometry sort of deals. And again, metal and non-metal. And finally, we have our drill bits, which, you know, drill holes of certain sizes into our bits and also thread bits, which create standard sized bolt threads in our material. Super straightforward, super helpful to have that, you know, in the auto tool changer as well, so you don't have to do it manually. Now, that's all the bits. Some you'll probably never use. Not all of them came with your machine, but it's worth knowing what these bits are and what they do, so that if you need them, you can get one and put it in your machine and actually use it for a job. So, we're going to be doing a roughing pass on wood. So, we're going to choose a single flute non-metal bit. And I'm going to choose the 3.175 mm by 25 mil, which came in our machine in tool slot one. If you're cutting metal, you'll probably just want to choose the 12 mm metal version, which came in tool slot 4. These tool slots are assuming that you set up the machine as the instructions told you in the beginning. If you've changed them, you'll need to go back and, you know, put these in the slot later. So, let's choose our bit. Hit choose. And now we can go through and start assigning settings. As we saw in our last video, all of our default speeds and feeds and whatnot are probably fine. So, we're going to leave them. And we're just going to ensure that the bit that we've selected is in the correct tool number here. If you're doing anything fancy or custom, change it now here. If not, leave it in slot one. Now, processing boundary. This is where we limit what it will carve. If we select model boundary, let's take a look at it from the top. It's going to use the edge of our model as the limit of what it's going to try and engrave. If we select material boundary, it's instead going to try and engrave all the way to the edge of our stock. And because we've got no model there, it's going to engrave it all the way down to nothing. We don't want this because we going to have clamps in the way there. So, we're going to select model boundary. And if you really want to get fancy, you can select a vector here and import a custom 2D vector and use that as the boundary. So you could import a circle shape here for example and only engrave you know the intersection between this model and the circle which is a really handy feature to know. We however are just going to leave it on model boundary because we don't want to you know engrave away our clamps and this is the model that we want to you know extract from our block of wood. We are going to do something here though. We're going to add a boundary offset of.25 mm. Now what this is going to do is it's going to take our model boundary and then add 0.25 25 mm to the edge and basically make our roughing pass slightly bigger. The reason that we're doing this is because after our roughing pass, we're going to come back in with a finishing pass. And when we do that, we want the roughing pass to be a little bit bigger. So, you know, the tool bit of our finishing path isn't rubbing against the walls of our roughing pass. If we made them the same size, it's going to rub. If we make the roughing pass slightly bigger by 0.25 mm, we're going to have clearance. Under path strategy, we're going to set it to parallel this time. We did offset when we were cutting out pockets, but parallel is probably going to give us a cleaner cut as it just kind of scans, you know, back and forth along like that. If you were cutting out something round though, maybe like a sphere or, you know, a egg shape or something, you know, something that has nice round geometry like that, you might want to try offset as that might give you a bit cleaner of a cut. So, we'll leave it on parallel. We'll leave it on climb. And now we need to set the tool containment. So, why are we selecting on boundary here? Well, this is going to be largely because of our finishing pass. Imagine this texture here is our engraving bit. The bit is, you know, 3.175 mm wide and then it kind of tapers down to a little tiny bit that we'll actually be engraving with. Now, if we selected inside boundary, our bit is never going to leave the confines of our model. The center of our bit, which actually does the engraving, is not going to reach the edge of our model. It's going to get close, but it won't actually get there because the bit needs to travel a little bit outside of the model for it to actually be able to get that center bit. Engraving the edge of our model. If we chose outside boundary, our tool can obviously, you know, move completely outside. So, we're going to be able to engrave that outer edge. But, this is going to try and engrave in midair. You know, it's going to try and engrave things that aren't our model, you know, all the way down to the bottom. So, we're just wasting time there. If instead we say on boundary where the middle of the bit is allowed to go to the edge of our model then our actual engraving part of our bit which is in the middle of the bit is allowed to go onto the edge of the model and you know we don't waste it and we actually get to the edge of our model. That's a little bit difficult to explain. The best way to actually see what's going on is to select inside and outside boundary for yourself and then preview the actual cut to see how that you know changes how your part's actually going to be cut out. Just go and experiment with it if you didn't understand that. It's something that you need to learn through just seeing it in action. We're going to leave ramping off because we're just cutting with softwood. If you're using aluminium or brass, probably enable it. And we can go ahead and hit calculate. Oh, we haven't actually selected our model cuz we deselected while we're doing it. Let's hit calculate again. And there is probably going to be a lot of, you know, pathing and geometry calculated here. So, this might take a hot minute.

All righty. And that looks pretty good. As always, we've added something. We're going to go ahead and preview the tool path to just double check that it actually did the thing that we wanted it to do. So, let's run this. And I'm going to speed it up because it is going to take forever. And that looks pretty good. Our roughing pass has, you know, gone through and removed 90% of our material. As you can see, we're starting to get, you know, what our crater actually looks like. But because the tool is so wide, it's really darn rough. So, we're going to go ahead and exit that preview. And we're going to go and add another 3D relief to add our finishing pass. Again, we can leave cutting depth and safe position just as we did before. But now we're going to go ahead and delete our flat end bit from this operation. And we can go ahead and add a tool. And let's come and have a look at our engraving bits. Now, all of these engraving V-bits are pretty much the same just with one major difference. And that is this first number here, which is the size of that flat bit on the end. It's the actual width of the tip that it'll be using to engrave things with. And this goes from 0.1 mm to 0.5 mm. And obviously again, the smaller the bit is, the more detail you're going to get, but it's going to take more passes, which means your job is going to take longer. The.5 mm is going to give you about five times less detail than the.1 mm, but it's going to be about five times as quicker. Now, your Carver likely came with only a 0.2 mm V-bit for metal. So, if you're carving metal, you're probably going to be stuck to that unless you've gone ahead and bought one. If you're using wood though, you will probably find a 3 mm bit and a 0.5 mm bit in your tool bit of kits. It's floating around there somewhere most likely. So, you can choose from either of these. However, you can also choose the 2 mm metal bit if you're using wood or plastic or anything like that. There's not really much harm in using a metal bit for non-metals. For my case here, because we're cutting out a very big thing, I'm going to choose the 0.5 mm engraving bit because this is going to take a long time. Engraving detailed models out like this is a very time-intensive job for a CNC mill. And even with the.5 mil bit on the largest model that we provide, this job is going to take 6 or 7 hours. So, I'm going to choose the big bit cuz I don't want it to take 24. So, I'm going to go ahead and select that and I'm going to assign that to tool number five. It's not in my machine right now. And I'm just going to set it there because that's the one I have free in my machine. And I'm just going to ensure that I remember to put it into that slot before I run this job.

All righty. Under our feeds and speeds, again, we can leave it all the same, except we are going to disable step down. Like so. What this does is that it tells our machine when we disable it, hey, don't worry about milling all the stuff above it. I just want you to go down to the final layer and, you know, really tightly hug that surface and remove our 3D model. which makes sense because we've already removed everything above it with our roughing pass and we're just going to take that last, you know, 10 to 5% off. Unticking this is essentially the button that enables our finishing pass. We're going to set our processing boundary to model boundary and now we're going to ensure that we do not set an offset on this. Remember how we made the roughing path slightly bigger? This is going to make this slightly smaller so you know our engraving bit doesn't, you know, rub against the walls of our roughing pass. We're going to keep it on parallel. We're going to set it on climb and we're going to ensure it's on boundary. Again, enable ramping if you're using metal. And we can go ahead and calculate. And this might take a hot minute because there is a lot of path and geometry that this needs to calculate. It might take, you know, 3 or 5 minutes to process this. All righty, that is done processing. And we're going to go ahead and preview our tool path by ticking both of them and hitting preview. And this time, I'm going to go ahead and display our tool. And we are going to run that. And let's fast forward that quite a bit. And we're going to have to watch our roughing pass unfortunately as well. I'm going to get a drink of water.

And the last thing we're going to do is actually go ahead and cut that out, which we're going to be doing with a contour. But first, I'm going to go ahead and hide these just so it's a bit easier to actually see our model and not that spiderweb mess that's on top of it. And we're going to need to go ahead and add a 3D contour. First things first, we're going to ensure that object is selected and then hit generate contour and actually obviously select our model and then hit generate contour. What this is going to do is if we look at it from top down, it's going to basically grab the footprint of our 3D model and create a 2D vector from it because contours need to follow 2D vectors in MakeraCAM. And this is now pretty much the exact same process that we did in the last video. We're going to start our starting depth at 0 mm, but we're going to set our end offset depth to.5 mm. This is going to ensure that it goes 5 mm deeper than our model. This is going to cut into our sacrificial bit of wood, but is going to ensure that our part is fully cut out. Safe position. We can leave that as usual. We're going to select not our metal bit. Let's choose something else. Let's go with the mill bit. That's the non-metal one that we've got in there. We're going to leave it in tool slot one. Leave all the feeds and speeds as usual. Strategy, we're going to set it to cut on the outside of this because we've already, you know, carved up nicely to this model edge here. So, we don't want to, you know, ruin that. We're going to set it to climb. Enable ramping if you're using metal. And we are now going to add tabs. When we add a tab, we'll be telling our machine to leave a little bit of material connecting the thing that we're cutting out to our stock. This ensures that it won't move around or be thrown into our milling bit or something silly like that. One of the first times I was using a CNC mill, I didn't add tabs and essentially it got all the way down to the final, you know, cut after, you know, a 2-hour job. And as it cut the bit out of the stock itself, the bit flew up into the milling bit, it broke the milling bit and more importantly, it left a massive gouge in my thing and I had to restart all over again. Tabs would hold that all in nicely and we just go through and remove the tabs manually later. So, we're going to go ahead and add some custom tabs. Now, the width and the thickness is probably fine enough default for most things that we're going to be cutting here. The idea is that you want to make them thick enough so that they are strong enough to hold our thing in place, but also thin enough that they're easy to remove by hand. We don't have to do a lot of manual work with a saw and a file to nicely clean them up. So, with custom selected, I'm going to select our 2D contour. And we can see it's selected because the dotted lines there. And I'm going to add a tab. And let's select uh one, two, three. or if I can aim for the line correctly. Five. Six. And I'm not going to add any to this side because I want a nice clean side here. If you don't cut and clean your tabs correctly, you can leave a little bit of a weird artifact there. It's a bit of skill to remove them. I'm just going to leave one side here free without tabs. That way I know I have a nice presentable side for this model. And again, here we can just hit calculate. And exactly like our previous thing, we've got our thing there. So, let's go ahead and preview this. I'm not going to preview all the ones before because I'm pretty confident that they're going to work. And let's just run this. Whack that speed to max. Very nice. And as you can see, we have our tabs there. Little bits of material left. Beautiful. All righty. We're ready to get this thing cut out. So, first of all, save it. Ensure you're saving along the way as well. And we're going to go ahead and export our G-code like so. Ensure we have all of them ticked here. We can double-check our tool slot numbers are correct. And we're just going to export that and get it onto our computer connected to our machine with Carvera controller installed. The process of getting this cut out is going to be exactly the same as last time, but we will just need to ensure that our tools are in the correct slots that we chose one and five, and whatever you assigned yours to. If you're using a bit from the bit kits that doesn't come with the black collar on it, you will need to use the collar tool to put one of these collars on the bit so it can be grabbed by the spindle. Then, in Makera controller, we're going to go ahead and open the file. Check that it all looks good and then start the cup. Ensure the material origin is set to 0,0. We can do so because in MakeraCAM we set this up so that it has nice boundaries for our clamps and everything like that. And then just ensure that you enable auto leveling. Then go ahead and run the cut, and then just sit back and watch. Reminder, this might take a while. We're using pine because it's soft and we can cut this out really quickly. If you're using aluminium, this might be quite a long job if you cut one of the bigger things. So maybe try and cut one of the smaller model sizes, but as you watch, you'll have your roughing pass go through, and then your finishing pass to get your detail and everything in there. And then you go ahead and cut it out with that final contour. Once it's done, you can use the included handsaw to cut off those tabs. And then you can go ahead and sand them down nice and smooth. A soft sanding block here will do wonders. And that is our final piece. Also, a fun fact, I think that crater is about 85 km wide. And that little mountain in the middle, that's from when a meteor hit the surface of the moon, and it all turned to molten rock. And just like water, the surface of the moon splashed back, which is pretty crazy to think about because you don't think about rock acting like water. Regardless, hopefully this video, along with the last video, has given you enough to go out and start making your own part. Makera on their YouTube channel, has a large collection of tutorials on most of the tools that you will find in MakerCAM. So, if you get stuck on something, chances are they have a video guide for it explaining all the settings, dials, and everything that you can turn. If you make anything cool with your Makera Carvera you want to show it, or any custom funky terrain that you want to share with us, or if you just need a hand with anything we covered in this video, feel free to head on over to our community forums and post about it. Until next time though, happy making.