Carbide drill, and carbide reamer speeds and feeds

I have some 4130 1.300" dia. tubing that has been heat treated to Rc41-44.
I have to drill/ream some .3125 +.001 -.000
holes thru the tubing.I purchased some 9/32 solid carbide drills, and some .3115 dia. solid carbise stubby reamers.

What rpm's and what feed rates do you all think I should run on the hardened tubing.

I have to drill 49 holes totally.
Each of the 7 tubes will have 7 holes.
I purchased 4 drills, and 3 reamers.
So I need to be conscience of tool life., and also hole dia. tolerance.

Thanks,
Doug.

bump! Come on guys. I have to do these tomorrow.
Please

Doug,

I'd start with a drill rpm of around 3,000. Reamer would be about 1,000. You don't say what kind of drill or what kind of machine, so I can't help you on feed rate.

The reamer you will want to feed fast!

JR

Thanks for the reply JrIowa.
This job will be done on a manual b-port clone with a geared head. The work will be in a super spacer, with a "floating" vise (meaning we grab the work in the vise, and then lock the vise to the table) on each end of the 28" long 1.3 dia. tubing to give it some support on each end.
The carbide drills are marked US-22. Just some generic micrograin carbide stubby that the tooling house sells. They look to be 118* point, but with a thinned web. Go figure.
The reamers are probably the same brand
3" overall length.

If you have any feed rec.s on the reamer I would love to hear them. I was thinking between .004-.006 fpr.
Sound good?
I am hoping that the reamers will ream a little big, as that is what I have always seen in the past. So I went for a .3115, figuing it will ream to .3125. My hope anyway. If not I will get a bigge reamer.
Oh yeah, I will be holding the drills, and the reamers in new R-8 collets.
Thanks for any info.

I'd say more like 1800 rpm on the drill (150 surface feet per minute), you can run the reamer at the same rpm, but you need about .002-.004 feed per tooth, per rev. So, if it's a 6 flute reamer .003 x 6= .018" per rev, .018" x 1800 rpm = 32.4 inches per minute. If the hole was solid and deep you'd have to worry about chip clearance on the reamer, but as it's tubing that shouldn't be an issue. Personally I'd run the reamer slower, they tend to chatter at the start, so I'd drop it to about 1200 rpm or slower.

Oh... and you should be able to do 49 holes with one drill and reamer with plenty of life left over.

Brian

Brian, are you sure about the .003 fpt, fpr?
That just seems REALLY fast to me. But what the hell do I know anyway. Just making sure.
Thanks,
Doug.

What does the Application Engineer from the tool supplier/manufacturer recommend? Your questions pay their salary, and you should hammer them for info at or before the purchase.

Yep, .002-.004" per tooth is a good chipload for just about anything from about 1/4" to 1/2" diameters. You would have to slow down the feed for smaller endmills, but could increase for say a 3/4" endmill that is stronger. YOu have to be aware of the side loading and not snap stuff off, but for drilling, reaming, etc., (Z axis feed) then the .002-.004" should work great.

Reamers are designed to be fed fairly fast, if not they will tend to cut oversize, good to know if your hole is a bit small, but really they are meant to kind of be crammed thru there. You didn't say, but I assume this is a conventional mill, not CNC, if so, you can feel the "right" speed with the feedback on the handle. You should be only removing say .010" or so in diameter with the reamer, so it's not a heavy load.

Brian

Just to follow up (if anybody is interested)
9/32 carbide drill from Garr Tool
120 sfm, .003 Ipr

.3115 solid carbide reamer,no-name
57 sfm, .006 Ipr

seems to give the desired hole dia. of .3125-.3128.
The drills are giving me 14-20 holes before dull. The reamer is still going strong.
Thanks to all who replied.
Doug.

Cool, sounds like I wasn't too far off, glad it's working well for you.

Brian