PDA

View Full Version : What speeds and feed are needed to weld a SML drill into 303SS?



cacrawfo
05-13-2007, 01:48 AM
OK, so I know what speeds and feeds are needed to weld a screw machine length drill into my part, because I just did it on my setup part today!

Here is what I am trying to do, can anybody sugest an appropriate speed and feed?

I have a slant-bed Ikegai 8" CNC lathe, and I am making some 5/8 OD hydraulic fittings from 303SS bar stock. I am holding the stock in a 5C collet. The hole in the center is .300, and it is about 1.3" deep in Z. I would preffer not to center drill the part, so I would like to use a SML drill to keep things ridgid.

I set RPM to 2500, and used a peck-drill cycle at .006 feed per rev. I pecked .300 deep per peck. It started going poorly about halfway through, and I knew it was in trouble so I had the good sense to hit the E-stop as my machine does not stop the spindle in feed hold.... I caught it just as the drill started to turn a bit in the collet. :(

I know now that 2500 is WAY too fast, and I should probably use a deep-drill type cycle that completly retracts the drill out of the hole to clear the chips. (not sure if my Fanuc 6T has this, or if I will just have to hand code it.) A better adjustment of my coolant nozzle would help as well.

So, the million dollar question is, what speed should I be running, what feed, and how far can I peck before retract?


Thanks to all that care to reply, it takes a while to get the "feel" for these things, and the charts seem to be all over the place with such a large range. I have never had any F-ups (crashes), just a few mistakes (break a drill here and there) so I consider myself lucky!

Carl Crawford

Geof
05-13-2007, 10:24 AM
Pecking in stainless is not always a good idea. Every time you retract you leave a work hardened surface that the drill has to break through to re-enter the cut. A depth of 1.3" on 0.3" diameter is pushing it but I would try doing it in one go at a much slower speed...like 800rpm and drown it in coolant.

Obviously your drill survived one peck so you could compromise and do a single peck of 0.7".

fizzissist
05-13-2007, 03:02 PM
Pecking in stainless is not always a good idea. Every time you retract you leave a work hardened surface that the drill has to break through to re-enter the cut. A depth of 1.3" on 0.3" diameter is pushing it but I would try doing it in one go at a much slower speed...like 800rpm and drown it in coolant.

Obviously your drill survived one peck so you could compromise and do a single peck of 0.7".

I do peck drilling all the time on 304SS, but for that kind of depth especially, not only do you have the work hardening problem, but the chips ...the chips...the chips....You're stuck with retracting way too often, and all the way out....
Might try a gun or spade drill? They can be a lifesaver.

davereagan
05-13-2007, 03:37 PM
Your grade of stainless is a dream compared to 304 or it's evil twin, 316. 303 is resulphurized and makes nice chips. It cuts about like 1018 cold rolled steel, but is more sensitive to speed. I would run a cobalt split point screw machine drill at 900 rpm with flood coolant, and .007" feed per tooth and two pecks with full retract to cool the drill. I've never seen 303 misbehave like the others. Not sure what material your drill was made of, but that speed would melt a HSS drill even in 1018. Whatever you find to be the best, never think you can run that speed with 304 or 316. That week, you could be working for minimum wage.

Dave

cacrawfo
05-14-2007, 12:43 AM
Thank you everyone for your advice, I think I will order a few new drills on Monday and give it a shot again on Tuesday. The other problem that I need to adress is that I am holding the drill in a ER32 collet chuck, and the nut is so large that I cannot get a clear shot to the entire length of the drill with the coolant nozzle. I might try to build a "ring nozzle" out of copper tubing to surround the drill bit and spray more perpendicular to the bit. I usually drill a lot of brass and aluminum, and they do not need as much attention!
Dave, when you say .007 feed per tooth, do you mean a feedrate of .014 when using a 2 flute drill bit? I am familiar with feed per tooth when looking up feeds for endmills, but have not heard of it with drill bits. I bought a cheap Hertel letter set of HSS SML drills, I probably should have never tried one in the 303.... I will do as you say and get a cobalt 135 degree drill and turn it way down!
Also, I own the shop, the machines, and do all the machining so I pretty muck work for minimum wage already! ;)

Thanks!
Carl Crawford

davereagan
05-14-2007, 03:02 AM
Carl,
I should have said feed per revolution, not tooth. I just put 1 tooth in the tool file for my drills. By the way, when I put a drill in a pocket where a 6 flute endmill used to be and don't change the number of teeth, that gets really interesting. So, I would drill at .007" per rev. You might approach .010" if it sounds and acts well. Using a split point drill is important in any challenging material. Do you use a true soluble oil compared to a semi or full synthetic? I have run all three and never got much performance from a synthetic on difficult materials. I would be more willing to push the feeds and speeds with a chlorinated soluble oil like Rustlick WS-5050 or SwissLube. If you study the feed and speed charts for various drill manufacturers, you'll find out who knows their drills. Titex has the most thorough guide I have ever seen. They (Germans) and the Japanese drill makers (Tungaloy, Mitsubishi, Sumitomo, OSG) all specify soluble oil strictly. Also, I have smoked enough carbide drills in stainless, even after cutting my speeds, that I use only cobalt and take my time. It's such a hmubling material because it doesn't even measure on the Rockwell C scale (303, 304 and 316) but 304 and 316 especially will make 4140 HT or O1 look like a picnic. Unless you are into hundreds of holes or more, the cobalt Precision Twist drills should be fine. they cost a fraction of even the premium cobalt drills made by Titex, OSG or Nachi. Good luck, but it's not luck.


www.titex.com (http://www.titex.com)









Thank you everyone for your advice, I think I will order a few new drills on Monday and give it a shot again on Tuesday. The other problem that I need to adress is that I am holding the drill in a ER32 collet chuck, and the nut is so large that I cannot get a clear shot to the entire length of the drill with the coolant nozzle. I might try to build a "ring nozzle" out of copper tubing to surround the drill bit and spray more perpendicular to the bit. I usually drill a lot of brass and aluminum, and they do not need as much attention!
Dave, when you say .007 feed per tooth, do you mean a feedrate of .014 when using a 2 flute drill bit? I am familiar with feed per tooth when looking up feeds for endmills, but have not heard of it with drill bits. I bought a cheap Hertel letter set of HSS SML drills, I probably should have never tried one in the 303.... I will do as you say and get a cobalt 135 degree drill and turn it way down!
Also, I own the shop, the machines, and do all the machining so I pretty muck work for minimum wage already! ;)

Thanks!
Carl Crawford

davereagan
05-14-2007, 03:42 AM
Carl,
Here is a link to a 19/64" drill in J & L Industrial's Ozone overstock discount area. It's a Precision Twist HSS split point, Tin coated with a QC point for $3.11 marked down from $10.55 For $30, you can have an OSG or Titex, but would it last 5-10 times longer? Maybe.



http://www.jlindustrial.com/catalog/product.jsp?id=PQC-62319A&origin=SEARCH:OZONE_CATEGORY&backtosearchpage=Y&spec=XO

cacrawfo
05-14-2007, 01:31 PM
Dave,
Thanks for the link, unfortunately they only sell that drill in 12 packs... I ordered a 135 cobalt Cleveland drill, and a backup just in case.....

Here is what I am making, a small hydraulic adaptor. The turned part is lightly pressed into a punched flange, and then the asembly is furnace brazed.

I'll let you all know how I fared in a few days!
Cheers, Carl Crawford