Ø.020 drill .150 deep grade 5 titanium HELP

[Brad St.]

Ok, any suggestions on tooling,speeds and feeds please?

 

Thanks

Brad

[ReDEyZZ]

carbide drill or hss/colbalt?

[Brad St.]

Sorry, I should add a few more specs

Machine- Mori NV5000 12k spindle

we have on hand some MA ford carbide twisters as well as high speed.

 

The MA ford speed feed suggestions are calling for around 24k for rpms. . .I don't think I can make it there captain.

 

just thought to get some real world input for what we have on hand and available.

[ReDEyZZ]

For carbide I get around 22000 rpm, for hss around 10-12k.

 

prolly .0002-3 per rev

 

start at .0001 and work up, tricky stuff to do in titanium

 

hth

[Brad St.]

Thanks Jarret, that's what we were figuring also. Like I mentioned above, never tried drilling this stuff like this or this small. We've milled it but something about drilling I get real cautious.

 

We'll give it a try and see what comes of it.

 

Brad

[ReDEyZZ]

You will probably want a peck on it as well. every .005-.01" chip break or something.

[TK-32™]

I would do forHigh speed steel: s8500 f5.1 q.006(peck)

[Guest]

carbide circuit board drill. cant stress how important it is this tool have as close to zero run out as possable.

max rpm and .0005 chip load. .005-.01 peck. exiting the hole is no prob if you are flushing with coolant, but watch out too much coolant force will walk that size drill out.

this is going to take patients.

[Rick Henrickson 65]

if you have through spindle coolant and coolant collets it will be a big help

 

look at mitsu MZS drill with the spot drill

[Mike Mattera - TFM]

I had to do a job for the Bureau of Engraving and Printing where we needed to drill a 1mm home 17 mm deep. Tried all kinds of drill. The best results we with Guhring HSS drills. All other had inconsistent points. Get some small drills and put them under a microscope or comparator, you'll how bad the point is on most small drills. The Guhring drills were right on center.

 

Carbide is not the best choice because the drill needs to flex a little. Carbide doesn't flex. It breaks.

 

The other factor was the drilling cycle. I was using a Hermle with a Heidenhain Control. It had a special reduction peck cycle. It had large peck parameters and small peck parameters and reduction amounts.

 

Think of it like this...

I want to take 3 mm per peck.

Within that peck I want the first peck to be 1mm.

the next peck would be .25mm less. It keeps reducing until the peck - the reduction amount (.25mm). Each of these pecks does a .2mm retrect between pecks, until it gets the full 3mm depth (major peck) then it does a full retract pulling the chips out. Then if rapids back in (within a clearance amount) and does it all again. If you have a Fanuc control, someone must have a macro/cycle like that that you can buy. It would be worth every penny to get the job done.

 

I could never finished this job without that cycle. I was able to drill 40 holes per drill in H2 material. I had 1500 holes to machine total.

 

My 2 weeks in hell.

 

Mike Mattera

[88Matt]

quote:

---

carbide circuit board drill. cant stress how important it is this tool have as close to zero run out as possable.

 

this is going to take patients.

---

We use these all the time, down to Ø.004".

[Brad St.]

Thanks All, we had good luck with the carbide and were running 12k at .0005" fpt. Thanks for all the great input, thankfully this was a one of a kind for now and we got it done well enough. We have used circuit board drills and especially on our odd items like mp35n material. We run through a full range of materials here but support mainly R&D so we're never really on the same thing twice. So, we go from super soft to super tuff. Just great to come here and get the reponse needed to get through something that was due yesterday

[Josh T™]

Go with a EDM Hole Popper! Problems Solved