End Mill Advice

Any cutting fluid or wax? Standard taps? When tapping by hand I typically wouldn’t go more than one revolution (360 degrees) without reversing about 1/2 revolution (180 degrees) to clear the cutter! :star_struck:

This is what I’m using. Drill taps from harbor freight been good to me.

1 Like

If I have some cutting fluid, tapmatic, etcetera I will use those, but in a pinch WD40 works ok.
I save myself a lot of grief and only use HSS or better taps.

That’s the beauty of the slip clutch on decent drills. You can rely on it to engage long before the tap would break or damage. Feed in until it slips (either from lots of cutting engagement or caught on a chip), back off to break the chip or completely out to clear the flutes, rinse and repeat.

For utmost precision or small taps which require a delicate touch I wouldn’t advise a drill, but otherwise it can really be a huge help.

1 Like

I didn’t even know that combination drill bit/taps even existed! Do you that the whole task could be done with them, either with a power drill or a Shapeoko?

Believe they’re designed to be used with impact wrenches/drills. I’ve actually broken few, before I figured out how to properly use them. Method described by @PaulAlfaro is exactly how i do it these days.
If you bore a pilot hole (to the minor diameter of a desired threaded) with your shapeoko, then putting a thread with a drill tap is a breeze. They work best with a through holes though.

My projects often require thread milling blind holes and it’s easiest and quickest to do on a cnc with thread milling cutters.

You can use them to drill and tap holes simultaneously (as they were designed) but be very careful in thicker materials without pilot holes. Also, they snap easily without lubricant.

1 Like

The McMasterCarr link says “With a square shank, they’re compatible with tap holders for drill presses and milling machines.”

KISS for making tapped thru holes with Shapeokos?: Use slightly undersized Drilling endmills to drill holes for combination drill bit/taps. Most of the material is removed by the drilling endmills - reducing the torques required (to hopefully acceptable levels) for final precision drilling and thread cutting with the combination drill bit/tap.

1 Like

Very possible :wink: . I wouldn’t risk using them in a cnc router though. Gladly see someone else perform such experiment.

Those “compatible” auto reversing tap holders are kind of expensive and have limited speed capability. So a HF Spindle with a 1/2" collet and HDZ would probably be required. That likely makes your Fusion360 tapping approach much more attractive to most. But, using drilling endmills to drill (rather than endmills to mill) the holes required for the taps might still be worth considering.

2 Likes

Tap holder is way to pricey for me, regardless of how great it works.
I’m actually looking for a good set of metric drills (that I could use in a cnc) which would allow me to drill deeper holes. Remember @ScottLaird had some carbide drills worth recommending?

Wouldn’t you lose a lot of Z travel when using these? I cannot see the size but judging from the picture wih a tap, it looks fairly big. You would need an HDZ with a large spindle and fairly thin stock to use this device and clear the stock. I think that the tread milling cutters would be faster and more adapted to most.

Loss of Z travel depends on how high the spindle can be mounted on its Z plate. Regardless, it’s kind of a cool thing, don’t you think?
@BartK Wouldn’t cobalt (M42 HSS) suffice?

It is kind of cool but you still lose significant Z travel and would be impossible on the regular Z carriage. The fact that you can pull the spindle up in the mount only mitigates the issue and looking at pictures of large spindles, I think that there is not much room for moving it up.

@gmack Please post you step by step guide to programming thread milling ops. I’m a still new to F360 an do not want to risk screw up my stock. 1000 X 1000 X 12MM T6061 aluminum plate was not cheap.

@BartK is clearly your guy for F360 guidance. Personally, I’d be tempted to do some testing on something less expensive (like Baltic Birch and/or smaller pieces of Al) before going too far.

I’ll have to look into that. I’ve plenty designs where I really need longer end mills and they tend to chatter a lot.

@DCFYI This is the method I’m using and had no problems at all.

  • In DESIGN environment create a 5mm hole.
  • Use ‘thread’ function to create a 5mm thread. Your 5mm hole will automatically adjust to the thread’s minor diameter.
  • Switch to a MANUFACTURE environment and create a new setup. I’m assuming you have some experience with F360 CAD/CAM so I’ll only explain the thread milling essentials, simply because I don’t have the time for a whole F360 introduction.
  • First you need to drill a hole, so 1/8" end mill and BORING operation work best for me. You might want to change "RAMP FEEDRATE’ to something closer to 600mm/min. And set the ‘PITCH’ to 0.1mm or 0.2mm

Now that you have your hole you’ll need to cut the thread.
-Add a new tool to the library. And this is how I have it defined.


  • Choose a THREAD operation, from 2D operations drops-down menu and select your tool and hole that needs threading. These are all the tabs with settings that I’m using.
    -

    -This is probably the most important tab. You’ll have to specify ‘pitch diameter offset’ because it’s never given. 0.75 works for me with m5 holes, but you might need to tweek it a little, depending on the accuracy of your machine. I’m usually choosing multiple passes and 3 stopovers of 0.1mm. Used to do 2 stopovers of 0.2mm but 3 stopovers is a safer option.
  • Lastly, make sure to check ‘lead to center’ box and that’s pretty much everything you need to know about thread milling m5 holes.

This is the technique that worked very well for me, but before you try milling 150 threads in aluminium, you might want to try some hdpe. It machines super easy. Hope this helps.

6 Likes

This awesome! Thank you so much.

1 Like

@BartK do you have a link to the thread cutter you used?

Purchased them from beavercnc when it still existed. Maybe @Luke could chime in and provide a source for good thread mills.

1 Like

@BartK. Thanks again for the advice. I plan to air cut first. If all goes well I plan to cut a version MDF. BTW I’m taking the NYC CNC Fusion 360 online course right now, scheduled to take NYCNC’s hands on machining course March. Might even take the advanced fixturing and CAM course. In time I hope to become a resource for others who need help with F360.

3 Likes

Kennametal has a good selection of solid carbide drills and provides speeds and feeds based on workpiece material.

They also have a broad selection of taps.

2 Likes