In this video, we're going to be learning how to use your Makera Carvera to cut one of these. It's an ice stamp tray that you place your block of ice onto, and it imprints some fancy patterns onto it. Designed as sort of the first step maybe someone would take after completing the example cutting projects that came with your machine. If you haven't completed those yet, that's fine, but it does help if you've done it, but completely fine if you haven't.

So whether you're an at-home maker with one sitting on your desk or a member of the public looking to use one at a makerspace, or you've maybe got one at work and you're just wanting to learn how to use it, this and the second part to this video will hopefully teach you everything that you need to go out and start making your own things. We're going to try and get you just dangerous enough here, so let's get into it. First of all, CNC milling is a subtractive manufacturing process.

You start with a big block of material, we call this our stock, and we cut away at it bit by bit till we have the part that we want. Compared to laser cutting or 3D printing, which is an additive process, laser cutting is subtractive as well, CNC milling is messy, it's loud, and it's a little wasteful because you're turning a good amount of your stock into just confetti that can't really be reused. So why would you want to do this?

Well, the biggest thing is versatility. You can make parts out of pretty much anything as long as it's soft enough to cut. Materials like PVC, you can't cut that in a laser cutter because that releases poisonous gas when you do it. Polycarb is a nightmare to laser cut as well, and it's a bit of a fire hazard.

Milling these things though, perfectly fine, super easy as well. How about making a complex 3D part out of aluminium or brass? Good luck trying to 3D print those materials. That's why, as a nice little beginner tutorial, we're going to go ahead and mill a metal ice stamp into a hunk of metal, which is really in the specialty for a machine like this.

And this also just makes for a great little easy project to get your toes wet. All right, first step, let's choose some stock. Now, most ice stamp trays are actually made out of brass because it has wonderful thermal and antimicrobial properties. You can happily use brass and follow along and just choose the brass settings, but please check that it does not have any lead in it.

A lot of alloys of brass do have lead in it, and you don't want your water to be touching lead. If you don't have confirmation that it's completely lead free or you don't know the exact alloy of the brass, use something else. That's why we're just being safe and using some of the Makera 6061 aluminium, which is a pretty good enough replacement.

Size-wise, you'd want your block to be at least 5mm if you're using brass and maybe 10mm if you're using aluminium. We're using a 100 by 150mm piece of stock here. If you want to use the exact bit of stock that we're using, you can find it in the written guide linked below.

Also, if you want to follow along with this guide and get the cutting experience but don't want to use either of these metals, you can just follow along with a block of wood or plywood or anything similarly shaped. Obviously, it won't melt ice, but it gets you the experience. Now that we know what stock we're working with, we can get an appropriate design file to cut.

We're going to be using MakeraCam, which is the software that generates the instructions for our machine, which we call G-code. Makera accepts either a 2D vector file or a 3D model. In this video, we're just going to be using a 2D vector file and we'll look at 3D models in the next video.

We have a file ready for you to go on a 100 by 150mm piece of stock of any thickness. You can find a link to that in the written guide linked below, as well as some tips to design your own ice stamp tray design files if you wish as well. If you haven't already, go ahead and install MakeraCam.

Now, this is not a free software, but you do get a copy of it for free with the purchase of your machine. You'll be prompted to enter some details through the retailer that you've purchased it with, but if you bought it through us or another retailer that's not listed here, you'll just need to flick Makera an email with your machine serial number and they'll sort it all out for you and get you access to it.

They are usually pretty quick with this though, and you can get a 15-day free trial in the meantime by just punching in any old email address, just to get started. You get full access to it. So, we're going to go ahead and open up MakeraCam, and then we're going to do some 3-axis machining.

So, the layout's pretty simple. We've got all of our tools and our import everything on the top here. We've got a preview of our stock in the middle here, and on the left here, we've got all of our features, and as we add each cut, you'll see them pop up here.

First things first though, let's set up our stock by punching in the dimensions of the material as well as what material we're actually going to be cutting. Then we're going to go ahead and import a 2D file, and we'll just choose the vector file that we have.

Now, we'll need to line up our file. It's already nicely been placed on top of our stock, but we'll just need to select it, hit transform, and then move it into the center either manually, or we can select the auto align, which does a pretty good job most of the time.

Here we can see all the lines of our file, and the shapes that these vector lines form, the area inside, is what we're going to be milling out. This outer line here, by the way, you don't need that. That's just part of when I was designing it.

I said, this is how big our stock is, and I kind of drew it on the inside so I can see what it is. We're just going to ignore it. It's not important. Now, unlike the slicer software for a 3D printer, there is a bit of manual work required to produce our G-code, which is the machine instructions that will tell our carver how to move and cut out our piece.

We have the shape that we want, but we need to tell the software how we actually want it to cut along these lines because there are so many different ways that it can be done. Under our 2D operations tab up here, we have our bread and butter cuts, contours and pockets.

Pockets will machine away everything in a selected area, it will remove the entire inner area of that shape, while contours will just cut along the edge and leave any material in the middle. We want to completely remove all the material in these shapes, so we're going to go ahead and pocket this.

All right, we are going to be greeted by a wall of settings here. Now, thankfully, you don't actually need to touch most of these as MakeraCam will give you appropriate values for them. First of all, we have our cutting depth.

This is how deep we want to create this cut or this feature. We're going to start at 0mm, which is the surface, and we're going to make our cuts down to, let's say, 4mm. That's what we did on our test piece.

If you want to save some time, we reckon you can get away with 3mm on this ice tray, which is probably going to reduce your cutting time by about 25%. 3 or 4mm should be good enough for what we're doing here. Safe position is where we tell the machine how much to lift the bit up when it moves between cuts.

We can have this as defaults for now because we're pretty good, but let's say that our stock had maybe a little bit of a hill in the middle of that. We might need to increase this safe clearance height a bit just to get over that hill without accidentally cutting it.

Under tools, we're going to go ahead and select the tool that we want to use to perform this cut. Now, selecting the right tool is actually most of the difficulty in using your carver, but it's pretty straightforward.

So we're going to go ahead and add a tool, and here you're going to see all the bits that are in the ecosystem of Makera that you can buy. But for this type of cut, we're just going to keep it simple, and we're going to go to single flute metal, and we're going to select the 12mm one.

This one is 3.175mm wide and 12mm long, and it's the metal one, of course, because we're cutting metal. This one came with your machine, and if you set it up according to the instructions in the demo tutorial, it was going to be put in tool slot 4.

Down here, you can see all the pre-calculated settings for all the materials that it can cut, and we're just going to go ahead and choose it. And as you can see, down here, we've just gone ahead and punched those settings in for us.

Now, we're not going to touch these because if we increase it, we might push our bit too hard and maybe break something. The default settings are pretty safe as they're on the slower side, so they could possibly be bumped a little bit, but this slow speed setting gives us some really nice and clean results.

But it is also worth knowing what each of these means, so let's quickly go over them. When your bit cuts through your stock, it's going to do it in passes, or lines, like up and down, backwards and forwards.

And when it reaches the end of this pass, it's going to go ahead and move over a little bit and come back the other way. Step over, the first option here, is how much it should move over between each pass.

Our bit is 3.175mm wide, and our move over is 2mm, so there's going to be some overlap there, which is what you want. Step down is the same, but in the vertical direction.

It's going to cut out these pockets layer by layer, and this is just how thick each of those layers in each pass are going to be, how much you want to shave off the top each time. Feed rate is how fast the mill bit can move through the material in the X and Y direction, or horizontal across the stock.

Plunge rate is the same, but just vertically, how fast it can be shoved downwards into your stock. This is almost always going to be lower than your feed rate. Then you have spindle speed, which is just how fast the bit is going to be spun.

And then you've also got tool number, which is just what slot in the automatic tool changer the bit is loaded into. When we set up a machine, we just put it in tool slot 4, so we're going to leave it, but if you put it in any other slot, just punch the number in here.

Path strategy is pretty straightforward, it's just how it's going to move within our pocket to cut it out, and we're just going to leave it on offset, which is going to give us some nicer, cleaner cuts on the edges.

Cutting direction, we're just going to leave on the default of climb, and we're going to go ahead and enable ramping here. If we turn ramping off, the bit is going to move down to the next layer and then start moving sideways.

Ramping is going to tell the bit we actually can let you move down and to the left or right at the same time, like a ramp. When ramping is off, the bit will only move down and then left or right, it won't move both at the same time.

And obviously turning ramping on means it's going to move both at the same time, like a ramp. For soft things like plastic, you can leave this off, but we're cutting metal, so it's probably going to be a smart idea to enable it.

And again, the default settings are going to be good for us here. Sweet, those are our settings, so let's just go ahead and click this cube here. We can click on the top to get a nice square vertical view of our work area.

And then we're going to go ahead and ensure we have all of our cuts selected like so, and hit calculate. All right, we can go ahead and close out of this now, and you should now see these white lines in here.

It looks like a wall, but if you zoom in, they are actually individual lines, and these white lines just represent the tool path of your cuts. It's basically where the middle of the tool is going to pass over, and that is actually all we need to do.

We can go ahead and put that on our machine, but first, it might be a smart idea to go ahead and preview our tool path, just so we can catch any obvious errors or something like that and just double check that it's all safe and sound.

Now, that's all ready to go and put on our machine, but it might be a smart idea to preview the toolpath in MakeraCam first, just so we can catch any obvious errors or anything like that. So we're going to go ahead and preview our toolpath, select the toolpath we just created and hit preview.

I'm going to just angle it so we can see what's going on and I'm just going to hit play and maybe speed it up a little bit so we don't have to sit here for a very long time. That should be a good enough speed.

Sweet, that looks good. There's no obvious glaring issues like that and that looks like a nice final part to what we were envisioning. So let's go ahead and exit preview.

And first things first, we're going to go ahead and save our workspace. Now, this is not exporting G-code, it's just saving our MakeraCam workspace.

To create the G-code file, you need to go ahead and select export and select all your toolpaths that you've created and you want to include in this G-code file and just hit export and save it. And as you can see, that's going to be a .nc file.

Alrighty, that's us here. Let's head on over to the Carvera and bring our G-code along with us. First things first, safety.

This can be a dangerous machine, but as long as you respect it and you follow appropriate protocols and everything like that, you will have a safe time. When you stick your hand in the machine or anywhere near the spindle, ensure the machine is not running any G-code and that the E-stop is pressed.

This machine does not know the difference between metal and flesh, nor does it care. That spinning bin in there is producing quite a lot of forces as well, and there's always the risk that that bit snaps and it flies off at 100 kilometers an hour, or maybe your stock gets thrown somewhere randomly.

So ensure that that lid is down and you're wearing safety glasses when cutting. Also, you probably won't be using it, but it does have a 2.5 watt laser module in it for engraving purposes.

When using this laser, the machine is a class 4 laser and can cause instant eye damage. We're not using it here, so we won't have to worry about it, but just worth knowing for the future that there are some safety precautions needed when using that feature.

Also, it's worth noting that by default, this machine will likely keep operating even if you open the lid. The interlock is disabled by default.

If you want to change this behavior, you'll find it under the settings tab. So when your machine cuts, it's going to try and rip your stock off the bed and throw it somewhere, which is not very optimal.

So that's why we're going to need to clamp it down. There isn't really just one correct way to do this. As long as you have enough clamps to hold it down and ensure it doesn't budge anywhere, that's all you really need.

Ensure you don't over-comically tighten the bolts. Just make sure that they're firm enough to hold it all down. Also ensure that your stock is sitting nice and flush with your corner anchor bracket.

That bracket there is how your machine knows where your stock is actually sitting on the bed. We're not going to do it in this tutorial, but if you need to mount it somewhere else that's not in that corner, you're going to need to go ahead and use the included probe kit to manually tell your machine where the stock is.

But because we've got our anchor bracket, slide it in there, machine knows where it is. Now we're going to go ahead and open up Carvera Controller, which you should have set up when you followed along with the demo things that came with this.

If not, just go ahead and install it. First things first, let's connect to our machine. We have ours connected via USB, so we'll go ahead and connect to its COM port.

Next, let's go ahead and open up our file. You'll need to select Upload File and then navigate to it on your computer, select it, and then hit Upload and Select.

It may take a couple of minutes for it to get fully uploaded, so just be a little bit patient. Once that's complete, you should be able to see these green lines here, which are our toolpaths, which is going to get cut, as well as all the G-code commands that will be running on the left here.

Everything looks good here. We've got the right file, so we're going to go ahead and start a G-code task. And we'll be greeted to some very important settings here.

First of all, we'll need to set our work origin. This is just another name for where the corner of our stock is sitting on the bed.

We'll tell the machine it's sitting in anchor one, which is where we've clamped it to, and because it's sitting flush in there, we'll say that it has an offset of zero and zero, as in it's sitting nice and square.

Now, when we designed our file and went through MakeraCam, we ensured that there was a gap big enough between where we're cutting and the edge of the stock. Because of this, we don't have to worry about accidentally cutting a clamp or something like that that's sitting on the edge there.

If you don't leave enough room here, you can increase these offsets from the anchor point to just give yourself a little more space. Then we'll go ahead and select scan margin, which will tell the machine to trace the outline of our cut with the wireless probe's laser pointer when it starts.

And then we'll select auto leveling. We'll leave it on the preset of a five by five grid of leveling points.

If you're using the Carvera's inbuilt vacuum system, you'll need to go ahead and enable it with the switch up there. If not, remember to turn on your external system.

Also, it may be a safe idea to empty out your vacuum system before cutting metal. If you have something like wood dust in there, which is very flammable and potentially explosive, you don't want to throw possible blistering hot metal fragments in there with it.

There's an accident possibly waiting to happen there. An even better option, and probably a little bit safer as well, is to set up and use a little air assist inlet on the back.

We aren't using it here, but I think it's a good idea on a job like this. If you are using it, you will need to remove or raise up the shoe to ensure that the air can blast on the tip of the bit.

Something to be aware of, if you turn on the machine and then hit the E-stop or you turn the machine on with the E-stop pressed, you will need to home the machine again before running the job, or you will get an error like we've got here.

And in the top right, you can just open up the machine controls and hit home, and then you can just start the G-code job again. When our job starts, it'll pick up the wireless probe and scan out that margin with the laser because we told it to do so.

This is always worth watching as it'll show the area that it will be cutting in, and you can just make sure that there's no clamps in the way of the cut, and you've actually got the right size stock and everything scaled nicely and whatnot.

Then it will go ahead and level our piece and make the adjustments that it needs, grab the 12mm flute bit, and then it will cut out our job, which should take a little over two hours.

Cutting metal is done with a lot of thin layers compared to something like wood, so it's far slower than our wood one, which only took about 20 minutes in our test cut. And we can now just sit back and let it cut.

Please, while doing so, ensure that you are monitoring it. Don't let the machine run unattended.

While you're cutting, you might get up to the curvy circular bit on here and notice that it is a little bit different to the shape of our original vector design. Partly why we chose this design was to demonstrate this fundamental issue with CNC milling.

You can't cut a nice, thin, sharp corner with a big, round mill bit. This is just an inherent flaw of the process.

You could use a thinner, smaller milling bit to get more in there, but you've still got a rounded corner in there. You're probably going to get more accuracy, but that will increase the cutting time as well.

It's not really a big deal here on our design because we kind of planned this rounded edges to be part of our shape. But let's say we wanted to cut a square hole in this block so we could fit a same size square block through it.

We would run into the same issue, right? We'd have a square with rounded edges.

To fix this, we'd have to use something called a dog bone. We're not going to cover them here, but it is something worth knowing and learning about for future projects so you can get things to fit together nicely.

After our two hours, the job is finished. Undo those clamps, and that is your first proper piece cut from start to finish.

Now, this will not be food safe straight off the mill. It will need some post-processing first.

That is a whole can of worms we're not going to be covering, but it's not a terribly difficult thing to do. And if you want to make it food safe, a quick Google search can help you find out what you need to do.

And after some processing, we have our ice stamp tray. Get some large ice cubes and let them sit on the tray for a little bit to imprint the design onto them.

A quick dunk in some warm water can really help speed this up as well. Now, that was a nice and simple project to get our toes wet in the milling process.

But this was designed to be an easy project. We used a simple cut with a simple model and avoided a lot of the complexities and the catches in this whole process.

We didn't add tabs, and we didn't even worry about coordinating multiple cuts or anything like that. There is a bit more to learn, which we will do in our second video, where we'll cut out a 3D topographical map into a material of your choice.

So go ahead and check it out. If you need a hand with anything we covered in this video, or you made a funky ice tray and you just want to show it off, feel free to head on over to our community forums.

We're all makers over there, and we're happy to help. Until next time, though, happy making.