I spent some time figuring out how to get the HAAS VF-2 CNC Machine to make high quality holes into 304(L) Stainless Steel. Specifically, I wanted to make 2 0.625" deep holes with a 1/4-20 tap 0.5" deep and connected with a 1/8" groove to avoid virtual leaks.

For the pilot hole, the standard diameter for a 1/4-20 hole is 0.201". This seemed to break the tap, so I used a 0.209" diameter drill that Paul Stovall, the MCE machinist, recommended. This means the threads are a bit weaker, but they will be plenty strong for our purposes. Specifically, I used a #4 gauge carbide drill bit with 2 flutes and a TiAlN coating.

To drill into the material, I used a spindle speed of 2300 rpm and a plunge feed rate of 7 in/min. This is a bit slower than what the manufacturer recomended (11 in/min plunge rate) but in line with what FS Wizard calculated. 11 in/min broke the drill bit. Importantly, after each hole I spun the drill bit backwards at 2000 rpm. This removes the chips that can get stuck on the drill and break it. I also used coolant through the spindle to help with chips.

After drilling, I used a 3/8" diameter 90° chamfer tool to chamfer the holes to make threading easier and with fewer burrs. I used a spindle speed of 1000 rpm and a plunge feed rate of 2.3 in/min. To be safe with chips, I spun the chamfer tool backwards at 800 rpm. I used flood coolant.

I then used this 1/4-20 steel bottom tap with 3 flutes and a black oxide coating. A true bottom tap has a bit less of a chamfer; this tap is better for starting threads. This CNC machine can't use multiple taps. I used a spindle speed of 200 rpm. I did a chip breaking cycle ever 5 mm. I used coolant through the spindle.

Lastly, to add a groove, I used a 1/8" diameter carbide end mill with 4 flutes and a TiAlN coating. I used a spindle speed of 5136 rpm and a cutting feed rate of 4.76 in/min. I used flood coolant. To help with the longevity of the end mill, I plunged over the existing hole. This groove is only 0.015" deep to help with tool life.

I have added plenty of pauses after each drill to ensure the chips are gone. If the chips remain, I can stop the CNC machine.

Next, I will write some CAM software for the tapped flange and run it.