Advice needed: drilling .030 and .050 holes in 304 stainless

Hello all,
Ive decided I despise 304. Im slightly spoiled and run mostly 303 so im on a bit of a learning curve and figure the wise ones on this board might be able to save me some broken drills and frustration.

Here what's up. Both jobs described below are in 304 stainless steel.

I need to drill a .052 hole .300 deep. I was thinking 6k rpm, .010 peck and .0004 or 5 feed. Hows that sound? I only need to make 150 pieces for that job.


The one im really dreading is a 500 piece job with a .036 hole .430 deep. Hows 7k or 8k rpm, .007"? peck at .0003 ipr?
How many tools should I order for this one? Also do you think its worth buying expensive 12xD or 15xD carbide drills? or just a crap load of HSS?

I havent made holes this small for a while and wasnt programming when I ran jobs like this.

Any help or general 304 advice is appreciated. In general what do you guys use for turning SFM, feeds, and how much corner rad on your turn tool?

Thanks!

Call Guhring, they have great products with solid technical support. I recently upgraded my drilling process on 304 material and I'm drilling a lot faster with greater tool life based on their suggestions.

Also, keep your oil fresh, if it's been awhile since you changed it, then I would suggest to change it before you start your larger production run. Many shops underestimate the value of clean oil and sacrifice tool life because they think their oil is "good enough".

One of the unique hurdles in swiss-type machining is there are more opportunities for your cutting oil to be diluted by bar feed oil & way lube. I've seen many applications return better results by just putting in new oil.

The only problems I have ever found running any type of stainless is that I usually needed about 1/8D peck increment with full retract. Was not a problem of clearing chips, was a problem of not keeping the drill cool. Remember, the flutes of the drill pull the chips AND THE COOLANT out of the hole.

Quote:

---

Originally Posted by txcncman

The only problems I have ever found running any type of stainless is that I usually needed about 1/8D peck increment with full retract. Was not a problem of clearing chips, was a problem of not keeping the drill cool. Remember, the flutes of the drill pull the chips AND THE COOLANT out of the hole.

---

I used to have the same issue however, over the past few years, I've learned to follow the speeds/feeds suggested on some applications.

For so many years, I came across applications where the speeds/feeds didn't apply to swiss-type machining. So, my learned or natural response was to do it how I thought it was supposed to be done. This led me down a path of always "going slower" or peck cycles or whatever.

Then I started to try some of the tool manufacturer suggestions and things started to get better and easier. Now, I understand and I'm sure many people in the forum for CNC Swiss understand that every application has its caveats.

So, with that said, sometimes the tool manufacturer is correct but, that doesn't mean that we can't use good judgment and experience to make good parts and have good tool life.

Guess I should have added, this technique was used mainly with much older machines with very poor coolant delivery systems.

We run mainly 304ss in our shop in in Swiss machines. We carefully monitor tool life. All of our machines have high pressure cooling systems, it is almost a must for running production 304 parts with small holes. Mitsubishi makes coolant through drills down to .029", and they are fantastic. It is the only coolant through drills we buy under 3mm. If you follow their recomendations for speeds and feeds, you will never go wrong.

I'll second DCogswell, I run very small holes on swiss machines, and you can nevr go wrong with Guhring drill bits. The best. Pricey but it will save you headaches. Make sure you get a coated drill if you decide not to go with Guhring. 304 work hardens, so make sure your drill peck is minimum the drill tip length, or you will be burning up your drill. on the .052 hole shouldt be too bad.
but the smaller dia hole, i like to spot/dimple a diameter 1/4 of drill diameter, drill the hole, then go back in and chamfer/break edge. try to have the spade drill/spot point the same or slight BIGGER angle. make sure the flat /web on your
spot is smaller than the drill diameter. good luck.