What's new
What's new

Drill/tap SSteel tool life?

M. Moore

Titanium
Joined
Jun 8, 2007
Location
Vancouver Island, B.C. Canada
Looking for info on how many holes I can drill and tap per tool in 304 SS as a rough number to help decide when to change to new tooling.
Size will be 4mm tap with a 3.3mm drill. The holes will be 12mm deep and the threads will be 8mm deep. I am using an auto reverse tapping head so I allowed for extra depth. The drills are stub cobalt TiN coated, the taps are spiral flute for steel/stainless, all ordered from McMCarr. I also curious as to the best peck depth for the small drill. I have read a few threads on here but there is no definite answer. One suggestion was to peck to the diameter of the drill.
I will have about 500 holes to do which I know is not a lot but stainless can be a bit of a pain if everything is not just right.
I have run some of these parts in steel and a few in aluminum and now my customer wants a large batch in stainless.
Thanks for the help.
 
I find that drills last quite a while in Stainless when run at the right speeds/feeds. I use 40-45 sfm on 304/316 with HSS/Cobalt. They last about 2 weeks of runtime at 32+ hours a week.

Peck if you have too, but try not too. If you have to do it, make sure they are evenly spaced out and make sure coolant/oil has time to clear the chips and cool the hole.

Dont dwell anywhere as it will workharden.

I run .116" holes, .375" deep in 316 in 1 pass. Then roll tap a 5-40 thread. I do about 5k in 2 weeks with the same drill and tap. About to set this one up this week for another 5k run.

Good Luck.
 
Thanks for the replies.
DanASM, those are some impressive numbers. Not sure what you mean by “peck if you have to”? I will try without a peck and see how it goes. I ordered a dozen drills so I will have some spares if I ruin one or two.
What sounds when drilling mean “time to change the bit”?
I have an older mill with manual tool change so I can inspect the drill after each run of 16 parts, 32 holes.
I have no experience in deciding when the tap should be changed.
I actually will have 500 parts to do, so 1000 holes.
The little parts will be laser cut from plate and I am assuming 304 but will confirm that with the laser cutting shop.
 
Hopefully the laser isn’t too close to the holes to be drilled.
304 ive had drills last hundreds of holes.
Biggest thing is to have the speed and feed bang on, and tons of coolant.
Pecking isn’t great on stainless until you get into deep drilling like 3x D or more
Buy quality drills and 304 isn’t a problem
 
The laser cut edge is where I need to drill and tap. The material is 1/4” thick 304. Parts are about 1” square and need two holes in one edge. I ran about 6 for a test and had to spot drill first as the drill wanted to skate.
In steel and AL I did not need to spot first as a stubby drill worked fine.
 
AFAIK 304 has no advantage over 316 other than price, so when a customer specs out 304, it's usually to save money (at the expense of the machine shop).

It's no coincidence that 304 machinability can be a crapshoot, as it's made to be cheap. We've seen it time and time again on this forum where someone will machine 304 with zero issues for years, then suddenly gets a new batch of material that machines like crap.

So to answer your question directly, it's virtually impossible to tell you how many holes the drills will last because 304 is notorious for having a very wide swing with regards to machinability, and things have only gotten worse in the last two years.
 
Orange, I hear you about the variability and was only hoping for some rough numbers. I will keep a close eye on the drill to check for wear each tool change. Hopefully with the right feeds and speeds I will get decent life out of the drills. They are cheap so I am not worried about it as it is a cost plus job. I have very little experience with SS so I did not know if I would get 50 holes or 500.
 
If I had to guess, you could probably get through the entire job with anywhere from 1-5 drills.

Tool breakage detection would make life easy on a job like this.
 
Bob,
I already ordered the drills and spiral flute taps. His numbers are very impressive. I will have to check if the auto reverse head will do well with form taps, it seems like it would be fine for such a small tap.
 
The laser cut edge is where I need to drill and tap. The material is 1/4” thick 304. Parts are about 1” square and need two holes in one edge. I ran about 6 for a test and had to spot drill first as the drill wanted to skate.
In steel and AL I did not need to spot first as a stubby drill worked fine.
laser cut edge? like sideways into the part or someone pre cut the holes? if its going in sideways clean the face up 0.030" with an endmill on a climb cut to remove the HAZ then spot and drill. ive had to grind the edges down with something to get it to drill nice and last long. The HAZ (heat effected zone) allows the stainless to harden because of carbide precipitation on the surface.
 
BT, I have to drill into the 1/4” edge of the part. There is no extra material to machine off so I will have to deal with the parts as they are. After your comments I think that a carbide spot drill might be the answer?
As I said I did a few test pieces with no problems but not enough parts to show any tool wear.
 
I haven't had a lot of luck with spiral flute taps in SS. I prefer spiral point where I can use them.

If you use roll form taps, and soluble coolant, make sure your concentration isn't too low, or you will break taps. At least that's been my experience.
 
Finally an update on this order. Parts came in on Friday so I ran some today and here are the results so far.
The drills are not lasting well but the tap is performing very well. I have only done about 170 parts or 340 holes and I have used about 4 drills plus one I crashed.

The big problem is that one of the holes breaks through on an angle which I am guessing is very tough on the drill. I was also not going quite deep enough with the spot drill (carbide) and the last 32 holes were much better with a deeper spot.

I am pecking the 3.3 mm drill at 0.070 which takes a long time but it seems to work well. I did try a run with a 0.250 peck which is halfway (.0.490 depth) and the drill lasted only about 15 holes and then broke after not sounding good on the very first hole.
Drill speed is 1100 and feed is 3ipm. So it is working but not great and there is much room for improvement given the numbers others have posted.

All the above advice has been very helpful.
 
Hopefully the laser isn’t too close to the holes to be drilled.
304 ive had drills last hundreds of holes.
Biggest thing is to have the speed and feed bang on, and tons of coolant.
Pecking isn’t great on stainless until you get into deep drilling like 3x D or more
Buy quality drills and 304 isn’t a problem
What would you recommend for sfm while drilling in 304 and when do you feel I pilot hole is necessary. Thanks
 
What would you recommend for sfm while drilling in 304 and when do you feel I pilot hole is necessary. Thanks
I'm usually right around 50-60 sfm, need it slow enough that it has time to cut and pull itself underneath it (lots of down pressure) but not so slow that it grabs too much and snaps the edge off. essentially about half of mild steel but all depends on the equipment you use.

pilot holes I might use when over 5/8" or3/4" or more as if in a manual drill press you don't have enough torque or leverage to push down hard enough. also the flat on the end gets large enough then that its harder to mash it out of the way once you get into the silver and deming size of bits.
 








 
Back
Top