This tutorial will walk through basic CNC milling in 3 axes. We will hold a piece of stock in the flat vise, find its origin/WCS with the probe, and mill it. Then we will repeat this operation for a second setup. We will make a simple elbow fitting, a 1/4-20 to 1/4 NPT adapter:

Setup

Tools

• Tool 2: Thread mill
• Tool 4: Flat endmill

Make sure X-Y and Z offsets are set for both tools.

Stock:

First measure your stock on all three sides and record these numbers (they will be necessary for CAM programming). This piece is 25.5 x 33.5 x 33mm.

Workholding: 

Clamp the stock in a flat vise, roughly in the center of the dovetail bed. First, set the fixed vise (square top) in place and tighten one screw until it is firmly wedged in the main dovetail slot. Next, push the clamping side of the vise by its lower section until it is in contact with the stock, then tighten one of the two screws to wedge it firmly in the dovetail slot:

Lastly, tighten the screw that moves the sliding portion of the vise to firmly hold the stock (note: it may help to use sandpaper to increase grip on low-friction stock). Here, the short edge of the stock is along the X-axis.

Finding the stock (WCS Setup):

Next you will "find" the stock in space using the touch probe. Make sure you have a good understanding of WCS offsets and how this relates to actual machine position. Before beginning, make sure you are in G54.

First, move off the -X edge of the part, and bring the tool down past the top surface of the stock:

'

Then probe the stock:

And set the X WCS position (here we will use G56). Do not forget to account for the radius of the probe, which is 1mm as-shipped from Diabase).

Repeat this process for the -Y edge of the stock.

Now repeat for the top surface (no probe radius compensation is required in Z). As a quick sanity check, pull up one of the tools, activate the G56 WCS, and jog to the -X/-Y corner of the stock. At X=0, Y=0, the center of the tool should be over the corner of the stock. If it is not, go back and recheck your tool offsets and WCS position.

Toolpath Generation

Now that you have all the information you need about the size and location of your stock, you will put this information into the CAM setup. In the "Manufacturing" tab of Fusion360, create a new setup, and type in the dimensions that you recorded earlier. Also, in the "Setup" tab, make sure that the short edge is in the X-direction, in order to match how you held the stock in the vise. To reiterate: by probing the left (-X) and front (-Y) sides of the stock, and setting that point to 0, you are setting the origin to align with the coordinate system shown below. The probed origin must match the CAM coordinate system.

In "Post Process", set the WCS Offset to "3", which corresponds to G56:

We will perform 4 operations on this side: 3D Pocket, Face, 2D Pocket, and Thread. The 3D Pocket should be configured as follows:

Which yields this toolpath:

Similar settings can be used for each of the subsequent operations, which can be seen in complete detail by downloading the attached Fusion360 file.

Now post-process the toolpaths using the H-Series Post:

Then upload the file to the machine and run it from the web control. This is the resulting part:

Second Setup:

The second setup requires exactly the same procedure as the first. Rotate the part forward 90degrees so that the other end of the elbow is facing up and the bore is open to +Y: 

In theory, if the vise does not move, then the X position of G56 will remain the same, but it is best to confirm this before milling. Of course the Y position must be found again. The Y-position is most-accurately found from the +Y direction (See the note at the end of this tutorial.) But for simplicity, and because the relative Y-position of the bore is not critical in this part, we will use the -Y surface to locate the stock.

Again, match the probed origin and the CAM coordinate system:

Here, only the facing, boring, and threading are necessary. The elbow cutout has already been milled in the previous setup. See the attached Fusion360 file for all the toolpaths. The finished part will look like this:

A note about alignment between setups: the above was the simplest way to align two setups, and it relied on square, accurately measured stock. If alignment of setups is critical, then you should probe on a previously milled surface, and set the coordinate system in the CAM setup accordingly. This is something to consider in the first setup: mill surfaces that can be used for probing in subsequent setups. In the above example, it would be best to mill the perimeter to some depth to enable more-accurate probing of the X sidewall relative to the bore. (Of course we would not want to mill the perimeter too deep because it would affect how firmly the part can be clamped in the vise.) Similarly, measuring the Y-position using the milled (+Y) surface rather than from the -Y side will ensure the accurate location of the second bore. 

The more advanced tutorials, specifically 4- and 5-axis milling, go into more detail about better practices for setup-to-setup alignment.