1. Creating Tool Paths in Fusion 360: The process begins with the creation of two tool paths in Fusion 360 to guide the CNC machine. This includes setting up the workpiece in the software and programming the tool paths based on the design’s requirements.

2. Using G-Code: Fusion 360 generates G-code, the numerical code that directs the CNC machine’s operations. The speaker discusses the importance of setting up this code correctly to ensure the machine performs as expected.

3. Simulating the Cut: The software allows for the simulation of the cutting process, which lets users verify the path and make any necessary adjustments before the actual cutting begins. This is crucial for avoiding mistakes and waste of materials.

4. Defining the Workpiece and Material Setup: Detailed instructions are given on how to define the workpiece within Fusion 360, including dimensions and positioning. This setup is critical as it informs the CNC machine where to start the cut and how to orient the tool.

5. Selecting Tools and Cutting Parameters: Choosing the right tools and settings for the job, such as the type of cutter and the depth of each pass, is essential for the success of the operation. The tutorial includes guidance on selecting and setting these parameters in the software.

6. Post-Processing: After the paths are set and the simulation is satisfactory, the final step involves post-processing where the G-code is finalized and ready to be sent to the CNC machine. The speaker also covers how to save these settings for future use.

7. Executing the Cut: With all settings configured and verified, the G-code can be loaded into the CNC machine to start the actual cutting process.

Video Transcript

in order to cut something out with the CNC in the manufacturing workspace, we need to be able to create two paths for our tool to go through. As you can see here in this model, it will cut out these various slots in shapes, in contours in the model. And then we’ll have that actual part that we get from our CNC machine. But in order to do that, we have to do a few things in fusion 360 to make sure that we can create the G-code or the numbers that the machine needs to use. As we watch this simulation of the part being cut, you can see how the tool will go through and cut everything out in a specific path. The CNC is only following numbers made of the G-code exported in the post process of fusion 360. So we’re going to study how do we create these two paths. So we cut out the proper thing with our CNC machine. Here I have the shape in plywood that we want to cut out. This demonstrates some typical cuts that you’re going to make with a CNC machine here in the middle we have a pocket cut that doesn’t go all the way through, but it has an organic shape. Then we also have a slot that goes all the way through, like a date or cut with a table saw. This is a very common cut in CNC.

And then of course we’ll need to make a contour cut that cuts all the way around the outside of the plywood. Once you have everything in your model and your design the way you want, we need to switch workspaces. So go up to the top left and select Manufacture Workspace. Here in the manufacturer workspace it looks the same, except now we have different options and we can create a stock or material that we’re going to cut our part from. In order to do that we’re going to click setup and then New Setup. Fusion is asking us some questions. It wants to know how the model is oriented. So we need to set the work coordinate system. And we also need to set the box point. This is the zero point that the CNC machine will use to start cutting. for these basic operations, when we definitely have a square object, we can select under orientation, select z axis plane and x axis. Now I can either select a plane or an edge for the z axis. And then I can select the x axis right here. If I want to flip the z axis I can. So now the z axis is pointing up. And then I just need to select the box point. So right now it says stock box point. So I need to select it. And for this first cut because we’re going to cut the pocket cuts.

First I want to select this box point at the top left over here. So now this is the z axis going up the y axis going this way. The x axis is going this way. And this is where the zero point will be on the CNC machine. in the setup we need to go to stock. For this we’re going to use a fixed size box. And for this box we’ll type in 12in. 12in in 0.75. Now we have stock that is larger than our object. And then we need to offset from the left and then offset from the Y. And we want to offset 1.25in. This gives us enough material that we can use hold downs and other equipment. And we don’t have to worry about the sharp part running into those parts. Often you will not have a symmetrical object, so you’ll have to use this offset to make sure your object fits with inside the stock. Once the stock is set up, then we can select post-process. And right now it just has 1001. But what we can do is type Z top. This will be the prefix for any program that we name. And that way we know that the Z is at the top for this program. Then we can select okay. Over here it says setup three. I’ll also rename this to Pocket Cuts. And now I need to make a new cut.

The first thing to do is to select 2d 2D pocket on this page. It’s going to ask for a tool. So I’ll select tool. I’m going to select the quarter inch flat end mill. If you want to know how to make this tool, you can watch the video linked in the description. Once I have my tool selected, it brings in all the feeds and speeds that I need, so I don’t need to do anything here. Then I go to the geometry tab by clicking the geometry and I need to select this face. So if I select this face it knows that this is going to be the pocket that I’m going to cut out. Then I’m going to go to heights with the pocket cut. We want to go the bottom height to be the selected contour then the passes. This is one of the most important things we need to make sure that our passes are correct. If we were trying to fit a part, we could have stock to leave be negative. But right now I’m just going to uncheck it. If you’re trying to get a specific fit in tolerance, this is the proper way to do it. You can have negative stock value or a positive stock value. We definitely need to check multiple depths, and we need to have our maximum roughing stock down of And then we want to select use even step downs. Then we can go to linking in for our ramp. Instead of helix we’ll select plunge. That should be everything we need. We can press okay.

Fusion 360 will now calculate the toolpath that you can see right here. You can see how it’s going to go around and be in that toolpath. if you want to watch the toolpath select it, then click simulate. You can click play to watch the simulation or you can click all the way to the end and see if it’s going to cut out the part that you expect will exit the simulation. And we’ll click on our setup. now we have a pocket cut that’s going to cut this one out. Just like we want to save time I can right click on this and I can duplicate it. Now this is duplicated and this is my second pocket. So if I right click and I edit it now I just need to change the geometry for this one I don’t need it. So I’m going to delete all the pocket selections. And this time now I need to select this pocket. Everything else will be the same. So I can just press okay. Now for the pocket cuts I can select the entire thing, select simulate, click play. I can change the speed of the simulation. And this is exactly what I expect. These are the two cuts that I’m going to cut first before the contour cut that goes all the way around the outside of the part. These will be zeroed from the top of the stock. That way their deaths are as accurate as possible. If we see from the bottom, then we will have variations in the thickness of the stock and the material that won’t give us the most accurate cuts. So now I’m going to exit the simulation.

Now we need to make a new setup so that we can zero from the bottom. The most accurate way to do this is to duplicate your previous setup. So I’m going to right click on the setup and click duplicate. If we look here it says Pocket cuts I want to go ahead and delete this one and delete this one. I want to rename this setup as contour. And then I want to right click and edit. The most important thing is to change the box point. So I’m going to click Box point. And then I want to click the bottom here. So if you look down at the bottom we are now zeroing the z axis from the bottom of the stock material. This is basically the bed of our CNC machine. Everything else is exactly the same. We don’t need to change it. If you change the stock size then all your cuts are not going to line up under post-process. Go ahead and click the name and type Z bottom or Z bottom and then select okay.

The last thing we need to do is make a contour cut so we can go to 2D. 2D contour. fusion 360 will have already selected the quarter inch flat end mill, but go ahead and double check to make sure you have the right tool selected. Then for geometry we’re going to go ahead and select this bottom edge. So we can just click the edge.

And now it’s going to go all the way around. something that is different than using pocket cuts is when you make a contour cut, it’s actually going to cut all the way through the material. So we need to have some way of holding down the pieces so they don’t rattle around the router. In order to do that we add tabs. Tabs are something that don’t get cut all the way through, so they leave a little tab in between the material so it’s still attached. These need to be cut out later when you are post-processing your CNC materials for three quarter inch plywood, we want to use rectangular tabs. Have them be a quarter inch wide and a quarter inch height. We want to make sure the tabs are robust enough that they hold the piece in place, yet they’re really easy to remove with a router later. There are two options of setting tabs. You can either set by distance. And here we have them every two inches which would be too many tabs. We can try four inches. And this gives us a nice set of tabs. But sometimes you get a tab right in the edge here and that can be not the best. If you position them by the segment here, it’s going to try to avoid putting tabs right on the corner. So if you notice that, try the different methods here. And if it still doesn’t work, you can always use manual tabs. And you can still add a manual tab like this. If I select and I click here, it’s going to add a tab. If I need one more. So that’s usually the best way to go about that. I’m going to delete that tab by holding shift.

Next I need to click on height Before we wanted our bottom height to be exactly the height of the selected contours. In a perfect world, that would be perfect. We would just cut all the way through our three quarter inch plywood, and it would magically cut all the material away. That’s not the way it works generally, because there’s always imperfections. So we want to go just a little bit further than the plywood. So we’re going to type -0.02. Then click on passes. And once again we need to make sure we have multiple depths. We don’t want .75, we want 0.125, which is half the diameter of our bit. We can use even step downs. If you needed to make this part fit into something else, we could use stock to leave in stock. The leave could be a negative number or a positive number, depending on how your fit and tolerances work. Everything under linking should be fine. And then we can click okay.

Notice that the toolpath will go up over the tab. So when we simulate that. So I’ll go ahead and select the contour. And I’ll click simulate. And we start pressing play. It goes around but it leaves these tabs that need to be cut out later. And you can see how the toolpath will go up and over for those specific operations. Once you are sure that everything works for your simulation, you can exit the simulation.

And now it’s time to post-process. We’ll go ahead and select this entire set up at the top so I can select this set up pocket cuts. Then I can click post-process up at the top. It’s the d1, G2 for your post. Make sure you click shop, but open SBP. If you’ve been doing something else like laser cutting, you may have a DXF post-process Esser selected here, but make sure you select shot. But name number. We want to label this and I’m going to call it Z top example cut.

Fusion will save all your programs inside the fusion folder you may want to have a different folder. So I’m going to do that. I’ll select this output folder. So I made a folder of posts on my desktop. So now I have right under my desktop post. Very easy to find. Make sure that you’re using inches for the shot bar and then click post. Next we need to make a post for the contour cut. Because remember in between these two operations we’re going to change the z axis of the machine. So select contour then post-process. And notice it already changes this to remind you that you’re going to zero from the bottom. It will remember where you’re saving and then click post. So here I have my two posts, my contours and my pockets. So now I can take this to the shop mat or the CNC machine and use those to cut out my material. Happy 3D modeling!