Drill 3.5mm hole in 304L

[jeffrey001]

Hi, I have a lot of 3.5mm holes to drill in long 304L stainless steel bar, I have maybe 800 to one thousand holes to drill about .75 inch deep.

I have to tread 8-32, about half in deep.

What drill would you use for this, carbide or HSS coated.

Fot the last year or so, I have used HSS tin coated drill with some success, but now, the company I was buying drill from, DORMER have change their design, old number was A577 and now it have been replaced by part number A901 that is suppose to be twice as good.

Lip design of the drill is not the same and I'm having trouble drilling as the drill bit tend to break.

Would you use coated carbide drill with 304L SS.

If so, could you recommend part number.

Thanks, Jeff

[Metalmanti]

Jeff,
I have had really good luck with The Kennemetal B210HP solid carbide drills. I am not sure if you are using a CNC but if you are this is the way to go. Even if you are using a manual machine you may want to try these. Just make sure the drill has less than .0005" runout.

3.5mm drill
Kennemetal order # 2575493
Catalog # B210A03500HP
Run it at 246 SFM and .002 IPR
feed into the part at half the feed rate until you get to the full diameter of the drill and then let it rip. These drills need to run all out or they will not work right and could break.

We used a similar Kennametal drill just a different grade for Inconel 625. We were previously using cobalt drills and peck drilling. The job would take 8 hours. When we switched to the carbide drills we were able to do the same job in 15 minutes. We got very good life out of the drills before resharpening. It doesn't hurt to have a few on hand in case one breaks. I do not believe we have broken one yet.
We have done a lot of 316L and 17-4 drilling with the drills as well with the same success.
Hope this helps.


Scott

[neilw20]

I have had good success with Goliath Blue Point 2 flute intermediate gun tap as advised by Goliath using 'Tap Magic'

Problem with gun tap is chip goes ahead of the cutter, but if there is enough space in the hole that is no problem.

Tapped over 100 M4 holes with no problem.

The 2 flute tap is much stronger.

Using a drill cycle to position job, and a pause (M1 cycle) and 150 RPM
I used the manual quill hitting the reverse button on SX3 quill CNC but a reversing tapping attachment would work great.

As a torque limit I didn't tighten the chuck too tight and it skids in the chuck if you reverse a bit late. A bit touchey feely huh? Still haven't broken a tap yet.

Tried a Tn coated tap and it chipped before it even formed 1 turn of the thread. The blue point taps look they are nitrided, but that's just my guess.

You get a bit cockey with the RPM's after the first fifty holes but keep checking if it starts to load up it is going blunt. Just a touch on the CBN wheel by hand and another 50-60 holes go flashing by.

[ctate2000]

OSG Exgold series drills will perform better than carbide. 3.5 mm should only cost $15 or so. For 800 holes you will only need two or three drills.