Introduction: Drilling

Remember that it's impossible to machine sharp inner corners. When you're machining inside corners, you will end up with a fillet whose size is the radius of the tool you're using (see screenshot). You can solve this problem with a simple drilling toolpath.

Think about the purpose of the pushstick. You want to be able to firmly and safely push material through the tablesaw. If you have a radius on the inside corner of the "step" of the pushstick, the back edge of your material will not be flush against the pushstick. This would result in an unstable, and therefore less safe, system.

For this reason, you are going to drill a hole in that corner. This is called a dogbone--a style of machining that allows you to remove inner corners for a variety of applications.

Notice that there is not a hole in the solid model itself, so you will need to create a sketch that specifies where your hole will be drilled.

1) In the ribbon, change the Workspace to Model.

2) Orbit to the back side of the pushstick (no arrow), right click on the face, and choose Create Sketch.

3) In the ribbon, choose Sketch>Point.

4) Click the inner corner of the "step."

5) In the ribbon, click Stop Sketch.


6) In the ribbon, change the Workspace back to CAM.

7) Note the red exclamation point in the CAM Feature tree to the left of 2D Pocket1.

Because you changed something in the Model Workspace, you will need to regenerate the toolpaths you've already created.

8) To do this, right click Setup 1 and choose Generate Toolpath.

9) In the ribbon, click Drilling.

10) In the browser, click Select next to Tool.

11) From the Samples/Inch Aluminum library, choose a 1/2" Drill and click OK.

12) Change the Spindle Speed to 1000 rpm.

By default, drill rpm is not correct. Use the following schedule for Sample Library drills:

1/8" Drill: 4000 rpm

1/4" Drill: 3000 rpm

3/8" Drill: 2000 rpm

1/2" Drill: 1000 rpm

13) Click the Geometry tab.

14) Change Hole Mode to Selected Points.

15) Select the point you just created in the inner corner of the "step".

When you select a point for your hole geometry, you have more parameters to change in the CAM software than if the hole were already part of the solid model. Specifically, there is more to do in the Heights tabs.

16) Click the Heights tab.

17) Change Top Height to Selection.

This is because "hole top" does not exist--you just have a point.

Note that the Offset will have a red error, saying "invalid reference." This is just prompting you to make the reference, which you will do in the next step.

18) Click the top face of the pushstick.

19) Change Bottom Height to Model Bottom.

Note that the dark blue rectangle representing Bottom Height appears in the window.

20) Check Drill Tip Through Bottom.

A standard drill bit has a 118 degree angle at the end. By default, the drilling toolpath will end exactly at the tip of the drill. In this case, this means the drill would not go all the way through the model. By checking this box, the drill bit will continue past until it's created a complete hole through the model.

In general, you would use a spoiler board (scrap board) under your part on the bed of the CNC machine to prevent machining into the machine bed. However, it is OK to machine (lightly) into the Shopbot machine bed at Pier 9. Never machine into the bed more than 0.05".

21) Add a break-through depth of 0.02.

The break-through depth specifies how much further the tool drills past the bottom of the hole, after it has broken through.

22) Click the Cycle tab.

23) In the dropdown, hover your mouse over any cycle to read about the cycle types.

24) Change the Cycle type to Deep Drilling-Full Retract.

Though new fields will appear, leave those at the default settings. The default drilling cycle is Drilling-rapid out. This brings the tool into the hole once and then rapid retracts. Deep Drilling, which is more conservative, is the best cycle for the Shopbot, because it periodically retracts the tool out of the hole to allow chips to escape. This will help drill bits last longer.

25) Click OK to generate toolpath.


26) Click Setup 1.

27) In the ribbon, click Simulate.

28) Turn off the visibility of the model by clicking the light bulb next to "Shopbot push stick" on the left in the CAM Feature tree.

29) Make the stock transparent so you can watch the deep drilling.

30) Click Play.

31) Click Close to exit simulation.

More on Dogbone Joints

If you plan to use dogbone joints often, watch this videoshowing you another way to prepare your model.

Alternatively, download this pluginto automatically create dogbone joints in Fusion 360.