CNC Router Tutorial: Part 1¶

The CNC router is a fast, 3-dimensional automated machining tool. While CNC routers are geared primarily for machining softer materials like wood or plastics, they are still capable of machining aluminum or steel with the right settings.

This tutorial is split into two parts:

1. Part 1: (this page) Process a CAM file to prepare it for the router.
2. Part 2: Machine a part on the router using our generated .sbp files.

Objective¶

The goal of this two-part tutorial is to:

1. Provide a high-level overview of the CAM process.
2. Teach safe router setup practices.
3. Show the full and complete process to translate 3d models of plate designs into physical parts, to avoid confusion and to function as a reference manual.
4. Make a part out of aluminum!

Steps¶

Preparing a part for routing requires the following steps:

1. Import the file into Fusion
2. Create a part setup
3. Add machining operations to carve out material
4. Simulate the operations and toolpath
5. Export the toolpath as a file for our machine

1. Import File¶

Make sure you have Fusion installed and an account setup within our workspace.

Download a 3D model of the part you want to make. We typically use STEP/STP or IGES files, as they are an open, non-proprietary formats that work across most modeling programs.

You can use whatever file you'd like for this tutorial. However, you should find a file that is:

• A specific thickness throughout that matches material on hand. That would be 1/16in. (0.0625in), 1/8in. (0.125in), or 1/4in (0.25in).
• Not too big or small - a few inches on each side is perfect
• Contains holes in the middle that are no smaller than the router bit we typically use (4mm diameter).

Here is an example part. To download from OnShape, right-click or two-finger-click on the part and select Export, then under Format select STEP and give it a name. The file should download automatically in a few seconds.

Once you have a file on hand, the first step is to import it into Fusion. Open with File/Open or with Ctrl+O (Windows) or Cmd+O (Mac), then select Open on My Computer and select your file.

The file needs to be saved in a Fusion project before continuing. We store files within project folders in the shared Fusion space. Hit Ctrl+S (Windows) or Cmd+S (Mac) and select a project folder to save in.

2. Setup¶

We are now ready to create a setup!

A setup defines the orientation of the part along with the stock, or the initial material to cut from.

First, switch from Design to Manufacture, then select the Setup button in the ribbon to create a new setup.

A transparent yellow box surrounds the part, representing our stock material. We'll first reorient the part, then set the stock.

Most machines orient parts such that the X and Y axes form the horizontal plane, like graph paper, while the Z axis extends up in the positive direction from that plane.

The X-axis on our ShopBot is actually along the short axis, as shown:

As long as you know where the part is zeroed, you can select any point as the "origin". However, our router has an automated Z zeroing feature to the top of the stock material.

1. Select X & Y Axes under Orientation, then pick an edge that is aligned with the X-axis and another oriented at a 90 deg. angle for the Y-axis.
   • You may need to flip them so that the Z-axis is pointing upward.
   • You can reorient the part with the gimbal in the top-right corner.
2. Next, select the box point placing the coordinate system on top of the part so the bulk of the part extends out along the positive X and Y axis.
3. Finally, switch to the Stock tab and adjust the offsets to 0 in for Top, 0 in for Side, and something small for Bottom like 0.030 in.
   • This will ensure the tool cuts through the stock material and into the wooden spoilboard beneath it.
4. Hit OK on the setup dialog to wrap up.

3. Machining Operations¶

Now that Fusion knows our part orientation and stock, we can start adding in the machining operations. When routing parts, we will remove material and separate the part from the bulk sheet. We generally do this in two steps:

1. Machine inner geometry: holes, slots, pockets
2. Machine the outer boundary or perimeter of the part

We have to pause between the operations to fasten the part to the spoilboard, since it could go flying or break the tool if it becomes loose once separated.

The actual operations we can perform are listed under the 2D and Drilling sections in the top ribbon. Hover over the operations in Fusion to show an example and description. Here are some of the important ones:

• 2D Pocket: Removes a lot of material from an arbitrary shape, either completely through or at a specific Z (vertical) distance
• 2D Adaptive Pocket: This is a special type of pocket that tries to reduce the force on the cutting tool. This is typically not necessary.
• Slot: cuts back and forth along a line to create a slot
• 2D Contour: Cuts along a closed shape, like the perimeter of a part
• Bore: boring is the action of forming a hole, so the Bore operation is a special type of 2D Contour that just moves in a circular (or helical) path
• Drilling: Mimic a drill press by driving straight down into the material, with the expectation that a drill bit is installed in the machine.

3.1 Template Library¶

Let's begin by adding some default operations. From Manage, select Template Library. In the dialog, navigate to My Templates / Cloud / Router and select the template for your material, such as Plate - Aluminum. Then press the top-left button above to add them to your file. Close the dialog when finished.

Some default operations should now be listed on the left under Setup 1. We will go through these one-by-one in the next sections.

Our final operation will be a 2D Contour, so we will start with the rest as our inner operations.

3.2 Inner Operations¶

Double-click on Bore in the browser tree on the left. Our template operations have the correct tool selected (4mm single-flute end mill), but we need to update the geometry, since the template does not know where these operations should apply on our specific part.

Unlike 2D Pocket, a Bore operation only follows a single path. That means the holes we select cannot be more than twice the diameter of our tool. With a 4mm tool, we can't cut less than 4mm (0.157in) or greater than 8mm (0.315in).

Select Circular Face Selection, then click on all of the smaller holes that fit the bill. We'll leave the larger holes for 2D Pocket.

Repeat this process for 2D Pocket and Slot, deleting the missing geometry and selecting the appropriate new geometry for each. For blind pockets or features that only extend partway into the material, you will need to select the bottom contour so the operation knows how far down to machine.

You can delete 2D Adaptive Pocket, since we won't be using it here.

3.3 Outer Operation¶

The last operation to add is the 2D Contour to cut the part out. Repeat the process above, first removing the existing outline geometry, then selecting the new outline. You can select the top or bottom edge - this operation just needs the shape, and will use the stock thickness information to determine the cutting depth.

We are now ready to simulate and export!

4. Simulation¶

It is always a good idea to simulate your toolpath before running it on the machine, since small mistakes can be costly with subtractive processes like routing.

Make sure Setup is selected in the browser so all operations are simulated, then hit Simulate under the Actions section. The simulation steps through the toolpath, removing a virtual stock just as the real router would. You can adjust the simulation speed, pause, and even rewind or jump ahead using the trackbar at the bottom.

- `Toolpath` is checked
- `Stock` is checked, and transparent is unchecked
- `Model` opacity is around 50%

In this example, we can see the triangular pocket was cut through the whole part! Whoops. Let's fix that by moving the triangle to its own 2D Pocket operation. Close the simulation dialog, then right-click or two-finger-click on the 2D Pocket op and select Duplicate. Edit the first 2D Pocket to remove the triangle. Then, edit the second 2D Pocket to remove the holes, and under the Heights tab, adjust the Bottom selection to be the selected contour rather than the stock bottom.

Run the simulation again to confirm the fix.

Our toolpath is ready for prime-time! The final step is to export our files for the router. Be sure to save your changes (Ctrl+S (Windows) / Cmd+S (Mac)).

5. Export (Postprocess)¶

We've created a toolpath defining the position, speed (feedrate), and spindle velocity (rpm) to machine our part, but we need to translate that generalized toolpath into a language our router understands. Most CNC machines use G-code, but even the specifics will differ between vendors and machines based on supported features. The tool we use to generate that G-code is a post-processor.

Our Autodesk cloud space includes not just tools, templates, and projects, but machines and their post-processors. All we have to do is define which operations to export for each of our two files (inner and outer).

Choose NC Program, right next to the Setup icon. In the dialog, select the dropdown under Machine and Post and navigate to the Shopbot Tools post-processor, then choose an output directory and give a name to the first file. Switch to the Operations tab and select every operation except the 2D Contour. Select Post at the bottom to generate the first file.

Repeat this process, giving our second file a different name (perhaps ending with outer) and selecting only the 2D Contour operation under the Operations tab. Make sure to hit Post at the bottom to generate the second file.

Takeaway¶

Congratulations! The two generated files ending in .sbp from the post-process step above can be used to machine our part.

In this tutorial, we used Fusion and our template operations to generate a toolpath for machining a custom part on our ShopBot router. The process used here is widely applicable for other types of machines, like the CNC mill, and is used by professional shops worldwide.

In the second half linked below, we will actually machine the part.

Part 2: Cutting the Part

Further Reading¶

• Official Fusion CAM tutorial (90 mins)