6
$\begingroup$

I have a 10 mm depth x 5 cm length 99% Tungsten rod. How can I machine the described hole so that instead of having a bevel from the tip of the main drill-hole bit, it has a perfect 90 degree corner all around as if the tip of the drill bit were like a flat router bit?

If this is not feasible, I can think about a design that doesn't use this larger hole. For this design, the inside of the large hole will be filled with an AlO3 ceramic tube that snuggly surrounds 1mm D of round stainless steel wire that flows through the center.

Improve this question
$\endgroup$

2 Answers 2

Reset to default
7
$\begingroup$

You are likely referring to a counterbore hole, which may be drilled using a bit of the same name. Alternately, if you can't find a bit of the appropriate dimensions, it may be possible to remove the material using an end-mill tool in a CNC mill of smaller diameter than the hole (say 3 mm to the hole's 6 mm), and having the CNC machine mill a series of circles until the hole is the appropriate shape and the appropriate material is removed. From what I understand, using an end mill of the same diameter as the hole may cause it to get stuck and fracture in the titanium, which would result in a wasted component and a wasted tool.

@Ethan48 helpfully added that a CNC machine is not required, and a conventional milling machine may be used in conjunction with a rotary table. Align the axis of the hole with the axis of the table, and have the axis of the bit away from the table axis the appropriate amount. The table would then have the same effect as the CNC machine by rotating the part through the small circles.

Improve this answer
$\endgroup$
4
  • $\begingroup$ Would 15/64 inch counterbore bit = 5.953125 mm be close enough? $\endgroup$
    – Daniel Donnelly
    Oct 8, 2015 at 23:56
  • 1
    $\begingroup$ I would imagine you could find one with metric measurements somewhere if you really needed "exactly" 6 mm. Whether the inches measurement is close enough is a question you have to answer, i.e. consider your tolerances and the effect deviations will have on functionality. $\endgroup$
    – do-the-thing-please
    Oct 9, 2015 at 0:17
  • $\begingroup$ For reference there are hole standards, which might be worth looking up. To get a non-standard hole size may require the use of a CNC machine. M3 is 6.5 mm and M2.5 is 5.4 mm, so the closest standard I am aware of is the one you proposed. $\endgroup$
    – do-the-thing-please
    Oct 9, 2015 at 0:20
  • 2
    $\begingroup$ Just to clarity - it could be done by the smaller end mill technique on any milling machine - it doesn't have to be CNC. On a conventional mill, you would use a rotary table, with its axis slightly off of the spindle's axis. $\endgroup$
    – Ethan48
    Oct 9, 2015 at 14:25
0
$\begingroup$

Wow, tungsten, huh? Whenever I see exotic materials, usually a design mistake is being made. The other answer by starrise is wrong for various reasons. Counterbores are normally only used for making sockets, not boring blind holes.

If you actually want to do this, the right strategy would be to set up the work piece in a four-jaw chuck on a lathe and rough the bore with a carbide jobbing drill mounted in the footstock.

Your next step will be to dress a cylindrical form in Aluminum Oxide J 40-60 grit using a rotary dresser. Mount the form in the tailstock of the lathe and then finish the hole. Clean the lathe carefully, because now it will have grit all over it. If your bore needs to have a good finish (not apparent that it does, given what you have written so far), you can repeat the process with a 200 grit form.

Next you need to get an extension mount for your tailstock and mount a smaller diameter carbide drill to rough the small bore. Once again use a grinding form to finish the small bore. Depending on the tolerance of the small bore you will probably need to redress the form because it will wear down as it grinds out the bore.

Obviously everything needs to be concentric all the time, so you have to be checking runout carefully on every step.

All this work can be also be done in a drill press (or mill) if you make a suitable workholding fixture. Using a drill press or mill your maximum precision will be 0.005" and 0.002" respectively. A lathe will be 0.0002".

Improve this answer
$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.