This instructable will get you going with Artcam, an easy to use CAM program that's geared towards decorative woodworking. If you want to dive deeper into the software, check out the free ArtCAM Class here on Instructables.
With ArtCAM, you'll get a fully functioning CAD/CAM program that is specifically tailored to decorative woodworking, and has some awesome features for 3D carving.
- Works with hi-res images
- Allows for direct editing of surfaces generated by 2D images
- Has a full suite of vector drawing tools
- Has easy, simplified toolpath creation
- Has excellent toolpath simulation so you can get a clear picture of what your carved piece will look like
For more info on ArtCAM, check out their Youtube channel.
The free version of ArtCAM will let you work with vectors and 3D shapes, which is a whole subject on its own that we won't get into in this class. The paid version ($40 / month, no recurring payments required) allows you to bring in bitmaps to create 3D surfaces and edit them, which we'll get into here.
What You'll Need
ArtCAM (Windows only- $40 / month non-recurring subscription)
What You'll Learn
- Create a New Model in ArtCAM.
- Create a 3D Surface (relief) from a 2D image.
- Smooth an uneven surface.
- Create and simulate a CAM toolpath.
If you'd prefer to stick with Fusion and don't want to pay for software, check out my other instructable: https://www.instructables.com/id/3D-CNC-Relief-Sculpture-Fusion-360/
Step 1: Create New Model
To start a project in ArtCAM, just click on + New Model on the Welcome screen.
The New Model dialog will open with options for the following settings:
- Dimensions: This is the width and height of the model. This should match the dimensions of the stock you intend to cut out. In the class example, the stock will be 3" X 3".
- Resolution: This is the level of detail that the model will use. Higher resolution will mean that the surface being created will have finer detail. The default is 1000px X 1000px which is fine for our purposes.
- Job Origin: This is the location of the model origin. It defaults to the bottom left corner, which is usually the best choice because it will match the origin of the CNC machine.
- Units: You can select mm or inches here.
For this lesson, all the tools and settings we'll be using can be found in the following regions of the user interface.
Step 2: Create Relief From Image
Go to Relief > Import > Import to select an image as the base for the 3D object. Any image will do, but black-and-white images make it easier to predict what the 3D surface will look like.
You can download the Zip file attached in this lesson if you want to follow along.
Relief Image Settings
When you import a relief, Tool Settings will automatically pop up. ArtCAM will translate a bitmap image into a 3D surface by translating the value (blackness or whiteness) of each pixel to the height a point in 3D space.
- Origin Position: When the bitmap image is imported, it will be placed against the origin that was set when you created your model. The origin position should correspond to the model origin so that when you scale the image, it will stay on the origin. In the example, that's the lower left corner.
- Width / Height: These are width and height of the surface created by the image that was imported. Se these to match (or at least fit) within the boundaries of the model you've started. In this case, the image should be at least 3" X 3". Since it's a little bit wider than it is tall, set the shortest dimension to 3". It's okay if it's a little bit wider, the extra will be cut off.
- Z Range: This is the delta (the difference between the highest and lowest values) of the points that will make up the mesh surface of our 3D object. If the range is set to 0.5", a white pixel will be set to an elevation of 0.5", and the height of a white pixel will be set to 0.0". It's important that this range be set to a value less than that of the thickness of the stock to be cut. Since the piece I'm going to cut will be .76" thick, 0.5" is a safe depth to cut.
When the image is properly set up, click the Paste button in the dialog. ArtCAM will create a machinable 3D surface from the image.
Smooth The Surface
With most images, you'll notice that the surface created isn't very smooth. This is a function of the variation that happens in most images- white pixels make high points, black pixels make low points, and unless an image was created specifically to create a uniform 3D surface (that's called a Depth Map, and there are tons of them online), there will be plenty of errant pixels.
To fix this, ArtCAM has a handy tool called Smooth. Click the Smooth icon in the Relief Editing toolbar and you'll get a tool settings dialog. This tool will decrease the difference between the high and low points on the surface without changing the relationship between them. The result is a smooth surface that still has the recognizable character of the image.
- Radius: This is the size of the brush you'll be using to smooth the surface. A larger radius will smooth a larger area with each stroke.
- Strength: This is the degree to which the tool will level out the points. A low strength will change the height of each point by a short distance, whereas a higher strength will move the points further.
- Smoothness: This setting changes the character of the edge of the brush. A high smoothness will make the smoothing effect fade to zero at the edges, and a low smoothness will make a sharp edge on the brush.
Play around with these settings and see what the effects are. If you use this tool over the whole surface using the image provided in the Zip file, you'll get a very smooth result.
Step 3: Create Toolpath
Now that your surface is nice and smooth, it's time to make a toolpath. In this process, you'll select the area to carve, select the end mill you're going to use, set the thickness of your stock, and pick the style of cutting.
Create Machine Toolpath
First, go to the Make toolbar (upper right corner) and click the Create Machine Relief Toolpath.
This will bring up the Machine Relief Toolpath pane where you'll enter all your toolpath settings as seen below.
Select Cutting Tool
Click Finishing Options and a tool database will open. This is where you'll select your cutting tool. It comes with a wide variety of common end mills, but you can also import tools or create your own. I'm going to use a 1/8" Ø (~3mm) ball nose end mill, so I click on that one and click Select.
When you select Click to Define Material... you'll get the Material Setup window. This is where you define the Material Z Zero and the Material Thickness. Z Zero tells the tool where its starting point is. The Othermill I'm going to use to cut this part has an automatic zeroing feature that works with the end mill touching a conductive build plate, so I select Bottom Offset here.
My material thickness is .76" (19mm), so the Bottom Offset value is automatically set by subtracting the maximum depth of my surface cut from the thickness.
Tool Clearance Strategy
Under Tool Clearance Strategy, select Spiral in Box. This will create a spiral pattern from the center that will stop at the edges of the material. The other options here may also yield good results, so it's worth it to test them in the next step, Simulation...
Step 4: Simulate and Create Toolpath File
Now that you've got your toolpath setup, it's time to simulate it to see how it'll look when it's cut out. ArtCAM has exceptionally high-quality simulations as compared to a lot of the other CAM software I've used- you really get a clear picture of how the material's going to look once it's cut.
To run a simulationl, right-click on the Machine Relief toolpath in the Project window and select Simulate Toolpath.
The Toolpath Simulation window will pop up and let you make adjustments if necessary. The defaults here should be fine to start with.
The simulated surface shows you in very fine detail how the surface will turn out. It shows the **scalloping effect created by the round profile of the end mill and helps you anticipate how your part will look once it's finished.
The simulation will help you make tweaks to your toolpath if necessary. You might, for example, choose a different Tool Clearance Strategy in the Toolpath settings, or you might decrease the **Stepover and **Stepdown distances in the Tool Settings.
When you're satisfied with the results of your toolpath simulation, click the Save Toolpath button in the Project window.
This will bring up a new dialog that will let you save the toolpath with a Machine File Format of your choice. The Machine File Format is the type of file that ArtCAM will export, and will be specific to your machine. If your machine doesn't show up in the list, g-code format is pretty much universal. Save the toolpath file, and it should be ready to load into your CNC control software.
Check out my How to Run a Desktop CNC Mill instructable- it'll show you how to take this tool path and run the mill to make a wooden sculpture.