Need Help!- drill and tap 304 SS

[davereagan]

That makes no sense. You are pushing a .242" drill just fine right? The difference between .242 and .261 is 8%. Do you have a split point .242 and only a chisel point old style .261"?

[little bubba]

I see a lot of things wrong, and these are from my mistakes.

First, you're driving a #2 center drill .250 deep at .004" per rev, no pecks. Thats a .078 drill point going over 3X deep, no pecks at a HUGE feed for such a small drill. Then on the revision you are up to .005 per rev. Far too much, your original RMP and a 2ipm feed should work ok.

Second, you are using a center drill, and a little one at that, and driving it half way through the part. Center drills are for putting in centers to use on a lathe. What you are doing is spotting, use a spot drill, or the very tip of a bigger center drill. Since its a quicky job and you may not have the tools, take that little #2 and just stick her in about .030 or .040, not .250, you need a spot, not the grand canyon.

Third, as has already been said and corrected, pecking a lot DOES NOT make things better. The part is only .5 thick, one shot and done. On the same note, going from a .242 to a .261 drill isn't helping you at all. Drills get really pissy going down a hole that is close to their own size. They jump, chatter, chip, run oversize and do all kinds of nasty stuff. General rule, don't stuff a drill down a hole that is more than 1/3rd the size of the drill. I also think you are banging the feed a little hard, though I'm not an aggressive driller. .0025 to .003 for something in the .250 drill size, I would consider that the transition from ***** footing to aggressive. You have enough chip, but not too much.

A few more thoughts, if the part is only .5" thick, why are you drilling over an inch deep? Also, already been said, why do you think you can't drive a G drill? But can drive a C drill?

304 is a big jump from plastic(It's not harder to work with, just different), ease the feed(per rev) back a bit, skip the C drill, smaller spot or a better tool and you should be fine.

[Shop junkie]

Sweet thanks for the advice.

I made a mistake it's a #3 c-drill. But I'm pickin' up what your putting down. Next time I'll try a spot drill. I agree .250 might have been a bit much and I think it caused the early retirement of the .242 drill. So next time I'll use a spot drill and just pound the .261 in after, correct?

The part is .500 thick X 2.0'' wide X 2.750 long and I'm drilling and tapping with the part standing on end going into the 2.750, 1.100dp.

Sorry guys still fairly new with this machine not sure what the capabilities are, Ill take any help I can get. Everything you said so far has made sense and worked really well. I appreciate it.

[davereagan]

No spot drill. .261" Screw machine length drill can drill 1.1" and does not walk like a jobber drill. I'd go 400 rpm with cobalt split point drill, flood coolant with preferably soluble oil not synthetic, .004" fpt or 1.6 inches per minute and you'll be done without worn out tools. Need high vanadium tin or ticn coated spiral flute tap and tapmagic or other straight oil for long tap life. I would consider .266" drill to make tapping easier. Tap depths: .300", .500", .700" McMaster.com has nice selection of drills and taps.

[Shop junkie]

Awesome, I'll give it a try.

So peck or no peck on the drill?

[tnik]

for .5 deep, unless you have problems with the chips not breaking or not releasing from the drill, I wouldn't peck.

I tend to use a 35/40 SFM on stainless, and on small drills I go about 1 - 2% of the diameter for the chipload per tooth.

Worst thing with working in stainless is work hardening the material or the tool. Make sure to use plenty of coolant.

Also, why are you pecking the tap? I would just use some oil and drive it through. I usually run all taps at 100 rpm and oil by hand. unless its a huge production job then I purchase the more expensive coated taps and use coolant.

And I saw a couple other people say it, but you want to countersink the hole BEFORE tapping. Taps love a nice clean hole to enter, and having the countersink there before tapping will help the tap keep its life, not chip up, and give you a nice lead in thread.

[BigC]

I realize I'm commenting on an old post, but here is my 2 cents. You've had some good recommendations. Lots of coolant for sure. If you do get the 304 too hot from excessive speed you will work harden the material and NO slowing down will fix that part. You will not be able to go bigger or deeper or cut threads with HSS tooling.