One of my favorite things to make on a CNC are signs. Typically these are your standard carvings with letters or simple vector images. They are great...but it's only scratching the surface of what you can do with most CNC's.
Enter Fusion 360 and its advanced CAM workflow. You can create 2.5 and 3D objects and import the toolpaths directly into your CNC's software. In this tutorial, we will go step by step through my full process of recreating the Haunted Mansion Plaque from Disney World.
Check out the full build video below, which is separate from this Fusion tutorial.
Before getting deep into Fusion let's talk about the general workflow for this process. We can break it down into 4 steps.
I loved going to the Haunted Mansion as a kid at Disney World. A few years back I ran across a few people 3D printing the plaque that is right outside the front gate of the ride. Turns out they used photogrammetry to take a bunch of pictures of the plaque and then produce a high-resolution 3D model from the result.
I downloaded the model from MyMiniFactory, which you can find at this link.
Before bringing the model into Fusion 360 we first needed to correct for any scaling issues. I've found Fusion can be a little glitchy if the units of the design are different than your model. For my set up, I made sure that I had my units set to inches in the Document Settings in the component tree.
You might need to change this depending on your situation.
Fusion 360 gives you the ability to directly import meshes into the program. These can come in as either an STL or OBJ file. When these are imported they are treated as a mesh and not a parametric body. If you are planning on making adjustments to the model then you would need to enter the mesh workspace and/or covert it into a body.
I didn't do this because Fusion has a hard time with high polygon count mesh models. I actually thought I was going to have to reduce the quality of the model so that I can import something that would be milled. But, it turns out that you can manufacture a mesh model directly in Fusion without doing any conversions!
After importing the model you will have the option to change the units, if you are having scaling issues this could be another area to help fix the issue.
To double-check that I had the size correct I used the Inspect tool in the top toolbar and measured the distance from the top and bottom of the model. This is roughly 10 in, and a great size for my small scale CNC
If you want to change the overall scale of your model then you could use the Scale tool in Fusion but you would need to convert the mesh to a body first. Since that wasn't really possible in Fusion another option would be to bring the model into a program like Meshmixer to scale it and then bring it back into Fusion to create all the toolpaths.
If you want to go into even more depth on CAM and CNC inside of Fusion 360. Check out my full course here!
With our model imported we move from the Design workspace into Manufacturing. Inside the Manufacturing workspace, we have options to do more than just traditional CNC work. Some tools allow for working with 3D Printer, laser, and plasma cutters.
Before creating our toolpaths we first need to define our setup. In the Manufacturing workspace you can multiple setups and toolpaths are nested inside of those setups.
A setup defines a bunch of different attributes that will be used to help generate all our toolpaths.
For our setup, we will select Milling as the Operation Type. I usually won't select a machine since those settings don't carry over to my small X-Carve. Depending on your actual CNC you might need to select this from the drop-down.
The most important part of the setup is the stock. This is on the second tab of the Setup tool options. Stock can either be defined with exact dimensions or relative to the model you are trying to cut out. I typically will use exact dimensions and then cut my stock to size.
Then I changed the model position on the Z-axis so that the stock was offset from the bottom with zero as the offset.
The final setting is to define your Work Coordinate System (WCS) and zero point. I set the origin to a stock box point that is on the top bottom left of the model.
If the model has been imported into another orientation you're able to change the axis around to get it in the correct orientation.
Since we set the stock with the model at the very bottom we are left with a good bit of material that needs to be removed from the top. The easiest and fastest way to do this is with a facing operation.
All of the toolpaths are split between 2D and 3D. Facing is the first 2D toolpath.
With the facing toolpath selected several things need to be defined. One of the most important is the feeds and speeds. I don't go in-depth into how to find those in this tutorial since they will be highly dependent on the material your cutting, the bit, and machine settings. Make sure and check with your CNC and bit combo for the values that work best.
Normally you will set these up with the Cutting Feedrate as well as Ramp and Plunge Feedrates.
The very first option in the Toolpath Menu is to select the tool that will be used. This opens the Import Tool selection box. Many bit manufacturers will allow you to download their entire tool library and import them directly into Fusion. I've actually done this for my Amana tools but for this tutorial, I stuck with the Tutorial-Inch bits in the Fusion 360 Library. You should already have this option.
For the facing operation I filtered the tools on the right side to give me just face mills and then selected the 2in version.
The second tab on the Toolpath menu gives an option to select stock contours. These are the contours that define the outside boundary of the operation. Since this is facing it has automatically selected the entire piece of stock and a yellow line appears along the edge. Nothing will need to be selected at this step.
Next is the Heights tab. Here various options are given for the different machine heights on the CNC. The only ones I typically change are the Bottom Height and Top Height which define the outer limits of the actual machining operation.
The Bottom Height was changed to .01 in above the model to give me a little bit of material to mill in later operations.
Next is the Passes tab. Here we will define our Stepover as well as Depth of Cut.
The Stepover is the distance the bit will move over between passes. The max value of this will be the width of the bit and Fusion will automatically set a value it thinks will work best. Normally this is around 95% of the bit's diameter. Which in this case is 1.9 in.
We do want to use multiple depths when cutting and this option is selected. A good rule of thumb for the maximum depth per cut is half the diameter of the bit. But since this is a facing operation and we have a pretty massive bit I went with a pretty conservative number of 0.25 in.
Once all the changes have been made Fusion with automatically calculate the toolpath. Then when it is selected it gives a preview. This can further be dialed with Simulation is selected from the top toolpath.
You can define how you want your stock to look as well as what appears during your simulation. I've got my tool holder turned on, the toolpath set to tail, and the stock set to Plastic Vinyl.
The play bar at the bottom lets your cycle through the tool path.
The green bar at the very bottom of the screen is a timeline view of the entire toolpath. You can mouse over this and see all the stats for that position in the toolpath. This also shows up as red if there are any errors when running the simulation.
With the excess material removed from the top of our stock, it's time to move into removing the majority of the material with a 3D Adaptive Clearing operation. I find that this is usually the best option when carving anything 3D. It will automatically optimize the toolpath and can be applied for the entire part.
A 1/4 end mill is selected for the tool in this operation.
Unlike our facing operation we don't want the entire stock to be milled away. Instead, the Machining Boundary is set to a silhouette. This will remove only the material that is within the shadow of the actual part.
Tool Containment is set to Outside with an offset of .25in. This will create some additional space on the outside edge of the part to give our next operation a little more room to get into the actual cutting position.
Rest Machining is left turned on. This removes all remaining stock from the previous operation. Now, since we just did a face milling operation we shouldn't have any remaining stock but this is a great option to leave select is you are slowly stepping down the size of your bit and you want to be sure that all the material is removed from the previous step if some were skipped because the bit couldn't fit into certain spaces.
Again all the feeds and speeds will need to be adjusted depending on your situation.
On the Heights tab the Bottom Height was changed to .25 in above the model bottom. Since the part is going to be removed from the stock in a later operation I didn't want this toolpath milling all the way to the bottom. Also, I went up 0.25 in so that I could still get the rounded over edges from the model.
If your part is completely flat on the sides then this could be set much higher. Inversely if your part has a 3D profile on all sides that you might need to use a two-sided milling operation to leave those profiles intact.
On the Passes tab the Maximum Roughing Stepdown is set to half the bit width (.25/2).
I love the ability to simulate each tool path. Your not only able to see what the part will look like but also see if there are any collisions and general errors before actually running the CNC.
Once multiple tool paths are created then make sure and simulate by right-clicking from the Setup instead of the toolpath itself. This will run all the toolpaths and color code for each operation (green and blue in this picture).
With the majority of material removed it's time to move to our finishing operation. There are a bunch of different strategies for finishing but I will normally use a Parallel tool path. This will run a bit back and forth across the entire model just like an inkjet printer.
Parallel toolpaths work best with ball nose end mill. You can still get a similar result with a straight edge end-mill but it will take A TON more time.
Just like on the 3D Adaptive toolpath the Bottom Height is adjusted to .25in on the Heights tab. This is again to leave stock at the bottom of the piece so it is only completely removed during the 2D Contour toolpath.
The quality of the finishing pass is defined by the Stepover of the operation. Varying this amount can greatly increase quality but it comes at a cost of time. For this example, I left it at 0.05in but you would want to increase that to get less of the scallop effect seen in the simulation.
Now we've got a part milled out in the stock, we just need to remove it. Typically this is done with a 2D Contour that will go around the edge of our model. Now if the model has been created inside of Fusion then you would be able to select the outside edge for the contour. In our case, it's a mesh and it won't be that easy.
The following process will create a silhouette image of the plaque and convert it into a DXF that can be imported back into Fusion. I'm using Adobe products but any photo/vector editing combination can get you there.
I first grabbed a screenshot of the plaque when it was loaded in Meshmixer. I did it in Meshmixer because it had a dark background (which I could have done in Fusion) that would help in the next step.
That image was brought into photoshop and I used the Select Subject tool.
This constantly surprises me how well Photoshop does it grabbing the main subject. From there I masked the background away and applied a black color overlay. Now I have a solid color image of just the plaque shape. I could then bring it in Adobe Illustrator.
In Illustrator I converted the image into a vector with the Image Trace tool which is set to Black and White Logo. I expanded the vector and deleted the background. Which left me with just the shape.
I exported it as an SVG file and imported it back into Fusion in the Design workspace. Again at this point, you can run into scaling issues depending on your units.
This is a pretty crude way of getting the outline and the shape wound up not fitting exactly once I scaled it done. I was ok with it, but if you want to get something exact you would need to convert the mesh into a parametric body at the beginning.
With our outline created as a new sketch we can go back into the Manufacturing environment and select our 1/4 end mill.
The option to select the outline is under the Geometry section of the tool tab. This then gives the ability to set up your tabs. I like to select the points myself instead of having them evenly spaced.
Once the tab locations have been selected you'll see a 3D transparent outline of their shape. If that is overlapping with your model then the toolpath is set up to go in the wrong direction around the model. Click the red arrow to fix the toolpath's direction.
The only other setting to change is the depth of cut with multiple passes under the Passes tab. Again use half the bit diameter as a good rule of thumb (.25/2)
An awesome feature of Fusion is the ability to export the simulated stock. If you run the entire simulation you'll wind up with something similar to the image below. By right-clicking on the stock, there is an option to save the stock. This save's the model as an STL that can be brought back into Fusion
It's useful to round trip the model like this to get an idea of what your part will actually look like once it's milled out. In this case, the scalloping from the parallel tool path is pretty visible.
With all the toolpaths created the last step inside of Fusion is to export them. Right-click on each tool path and select Post Process. You'll have a few options on how to save them and then will show up in your directory as a .nc file. I like to name them with the toolpath used as well a bit to make sure I have the right one loaded in the machine.
Lastly, the GCode is imported into your CNC software. I use an X-Carve so Easel lets me import GCode directly. To set up multiple toolpaths I just add a new workspace at the bottom.
It's pretty amazing to see something as complicated as this sign gets milled out in my garage shop. This process can scale to tons of different applications and machine setups. It's pretty crazy what all you can create with Fusion!