Fusion 360 CAM Tutorial for 3D Carving Beginners

I recently built a side table for my office with a modern and minimal style that has three splayed legs and a dish-shaped table top that was carved on my CNC. In this tutorial I will show you how to model this and then set up CAM in Fusion 360 so it can be carved on the CNC. Even though this is a top for a side table, the methods also work great for making serving trays, desk organizers, or larger table tops!

Be sure to check out the video!

These include affiliate links

■ 1/4" Dia. Downcut Bit

■ 1/8" Dia. Ball Nose Bit

Walnut Lumber

Fusion 360

The first thing we'll need is a 3D model of what we're going to carve. Follow these steps to model the table top:

1. In the Design workspace, pick Create Sketch
2. Pick the XY plane
3. Click on the Center Diameter Circle tool to begin drawing a circle with a diameter of 520mm (20.5 inches).
4. Type E on the keyboard to bring up the Extrude tool. And extrude the circle up 26mm (1").
5. Pick the top surface of the cylinder, and type O on the keyboard to bring up the Offset tool. Pick the outer edge of the top surface to offset it by 15mm inward.
6. Press E on the keyboard again and extrude the smaller circle into the cylinder by 12mm to complete the general shape of the top.
7. To create the shape around the lips, go under Modify and pick Chamfer.
8. Select the top inside edge of model, and push the edge outward until the inner vertical wall completely disappears.
9. Type F on the keyboard to bring up the Fillet tool. Pick the two sharp edges at the top, and type 3.5mm in the text box. This will round off the top edge.
10. Type F on the keyboard again to bring up the Fillet tool. Pick the final sharp edge at the bottom of the dish shape, and type 22mm to smooth out the inside bottom corner.

This completes the model!

Now it's time to set up the tool paths. To start, make sure we switch from the Design workspace over to the Manufacture workspace.

1. Under Setup drop down menu, select New Setup. This is where we get to define the type of operation we're generating a toolpath for; the model used to calculate that toolpath; and the size and shape of the raw materials we're starting out with.
2. Under the Setup tab, the Operation Type is set to Milling since we're using a CNC.
3. I like to set the Origin to Stock Box Point, and place the origin on the top surface of the lower left corner.
4. Under the Stock tab, I changed the Mode to Fixed Size Box, which allows me to input my own dimensions for the stock.
5. Click OK to finish the setup.

The first operation I like to start out with is a 3D Adaptive Clearing toolpath, which can be found under the 3D dropdown menu. This operation is used to remove the bulk of the material in the most efficient way possible, and prepare the workpiece for finishing passes.

1. The first thing is to select the tool we'll use for this operation. I picked the Amana 46202-K 1/4" downcut bit.
2. Next, go to the Geometry tab, I set the Machining Boundary to Selection.
3. Pick the outer top boundary on the model, which tells the machine to stay inside that boundary when it's carving. Otherwise the machine will try to remove all of the extra stock, which adds a lot of unnecessary time to our process.
4. Make sure Rest Machining is checked. This tells the machine to only remove the material left over from the previous operation. And since this is out first operation, I set the Source to From Setup Stock.
5. Under the Passes tab, I set the Maximum Roughing Stepdown to 6mm, which is roughly equal to the diameter of the bit.
6. Make sure that Stock to Leave is checked. This will leave a small amount of extra material for the finishing passes to chew through.
7. Click OK and let the toolpath generate.

After this operation, we'll end up with staircase shapes in areas where the part has contours in the Z axis. So now we need to define the finishing operation to smooth all that out.

The finishing operation we'll use is the 3D Parallel Pass found under the 3D drop-down menu.

1. Just like before, the first thing we'll do is select the tool we'll use for this operation. I picked the Amana 46294-K R1/8" ball nose bit.
2. Under the Geometry tab, we'll set the Machining Boundary to Selection.
3. Pick the outer top boundary on the model, just like in the previous operation.
4. Most importantly, make sure Rest Machining is checked. And this time the Source should be set to From Previous Operations. And make sure that Adjustment is set to As Computed, because the Ignore Cusps option will actually ignore the staircase shapes in the part.
5. Under the Passes tab, I set the Stepover to 0.5mm, which is roughly 8% of the diameter of the bit. I find that this is good balance between surface finish quality and machining time.
6. Click OK and let the toolpath generate.

The last operation we need to do is to cut the part out of the stock material. To do this, we'll use a 2D Contour Toolpath, found under the 2D drop-down menu.

1. I swapped back to the Amana 46202-K 1/4" downcut bit from the first operation for this one.
2. Under the Geometry tab, I picked the bottom outer edge of the part for the Contour Selection.
3. If you are using clamps to hold everything down, here you can also allow the machine to leave tabs between the part and the stock material. Once that's checked, you can go in to select the size and number of tabs. Since I usually use double sided tape to hold things down, I will normally leave this option off.
4. Under the Passes tab, I enabled Multiple Depths and set it to 6mm. Because if i don't, it will try to cut through the whole thing in one or two passes, which is too much for my machine to handle.
5. Click OK to generate.

Now that we have all three toolpaths created, it's time to post-process and create the G-code.

1. Under the Actions drop-down menu, select Post Process.
2. Under the Post drop-down menu, we can choose the post-processor. This is going to depend on the CNC you have, and which Machine Control Software you use. For this example, I will use Easel by Inventables, since I'm using the X-carve to carve this.
3. After choosing your post-processor, choose the folder where you'd like to save the G-code by selecting the Output folder.
4. So, if you're like me and are using Fusion 360 For Personal Use, we can't save operations that involve tool changes under a single file. Also, my CNC doesn't have automatic tool change capabilities anyway, so we need to do a few extra steps.
5. Go up to the Operations tab, and select only the first operation, which is the 3D Adaptive.
6. Go back to Settings tab and change the file name to something you can remember. I used "Adaptive".
7. Click on Post. This will save the G-code for the Adaptive Clearing toolpath to the folder we selected before.
8. Now repeat this same process for the next two toolpaths.

Finally, the last step is to load the G-code into your Machine Control Software. Here are the steps for Easel.

1. Click on New Project
2. Under Project, click on Import G-code. And then pick the first file we saved to load it into the Workpiece.
3. Once it's loaded, create a new Workpiece and repeat the same steps for the next two toolpaths.
4. When you are ready, just click on the Carve button and see your creation come to life!