Announcement

Collapse
No announcement yet.

Help with cross-drilling 316 SS

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Help with cross-drilling 316 SS

    Noobie time
    Okay, I have very little experience with 316 SS. I am making approx. 30 custom bolts that have a precision 5/16" cross-hole in the head. Stock began as 1/2" rod with a dual 316/316L spec. Parting off in the lathe went without a hitch. Same with facing and roughing threaded portion to size. My lathe tooling is all Tin-coated carbide inserts.

    I am having trouble with the cross-hole. I burned up both my HSS-Co drills and also my #2 and #3 center drill. I was using the latter as a spotting drill. So before I blow money on some carbide drills, I would like to know what I'm doing wrong with my HSS and HSS-Co. i.e. is it a speed/feed issue, order of operation, etc. I seem to remember that 316 SS work-hardens fairly easily. Is that the problem? Here is what I was doing:

    * Hold workpiece in a collet block perpendicular to milling spindle.
    * Centered in both axis for correct location on bolt head
    * Spot with #2 HSS center drill, 850rpm, downfeed by hand
    * Drill with 9/32" screw-length HSS-Co drill, 850rpm, see below for feeds
    * Finish with 5/16" HSS reamer, 250rpm, .01" feed

    A few notes... I first began with using oil cutting fluid when drilling. I then switched to a water-based misting coolant system. The drills were clearly getting too hot. I tried various different feeds---my mill has power downfeeds of .01, .007 and .0047". The middle feed seemed to work well for the main body, but would burn up on breaking through the back of the workpiece. I ended up doing by hand and using appropriate pressure to keep a solid-string chip to eject from the flutes. This is what I usually use on mild steel and seems to give the best performance. Perhaps stainless is different, however.

    The center drills seemed to need an unusually high amount of pressure to cut to proper depth. I imagine I should be using a spotting drill instead of a center drill, but that's what I did; and that's what I had on hand.

    I used to drill 1/64" undersize and then ream. I then found I got a better finish if 1/32" undersized was used. This case adds a different factor, I found. Because I am drilling into a small radius workpiece in comparison to the reamer, entry up to about 1/3rd depth produces a lot of chatter. This is because the reamer does not contact the full 360-degrees of the pilot hole at the same time. Until it reaches proper depth to do so, there is more vibration than I would expect to want.

    So basically, I just wanted to inquire of the more experienced hands on this board as to my technique and suggestions for drilling this job correctly... I'm usually happy to just move to carbide when I encounter this much trouble, but in this case it seems an unnecessary expense. Thanks in advance for your thoughts.
    Last edited by Arthur.Marks; 05-09-2010, 10:22 PM.

  • #2
    I'd try cutting the rpms in half and see where that gets you.

    Comment


    • #3
      316 Stainless

      You're running the drills way too fast. Cut the RPM down to around 200. Use only sharp tools. Use cutting oil. What we're doing here is keeping the heat out of the process. That keeps the SS from getting hard. Run the reamer at about 90 - 125 RPM. You will be surprised at how well the tools will cut at the slower speeds. You may want to counterbore the hole with a 5/16 end mill down to where it's a full diameter just before using the reamer. Done correctly, you can machine 316 all day with HSS tools. Higher spindle speed creates heat. Dull tools create heat. Heat makes stainless get hard to cut.

      Comment


      • #4
        Like Toolguy and X39 said, slow down.
        I had about 40 1/4" holes to do a while back in 3/8" 316 SS plate. I used one Viking Tool and Drill, 260 UB screw machine length drill for all 40 holes. A little coolant, 250-300 rpm, and keep it cutting, don't dwell in the hole or it will get hard. A good quality sharp drill bit and it's like drilling mild steel.
        Home, down in the valley behind the Red Angus
        Bad Decisions Make Good Stories​

        Comment


        • #5
          And I'll add. I like to use castrol molydee tapping fluid for drilling sometimes in SS for small holes. It really makes a huge diff. The bit cuts rather than work harden the SS.. Im a BIG fan of the molydee. And not just for SS. JR
          My old yahoo group. Bridgeport Mill Group

          https://groups.yahoo.com/neo/groups/...port_mill/info

          Comment


          • #6
            x5 on the lower rpm's.
            I would also use either oil or lots of coolant - mist doesn't seem to provide enough cooling because it doesn't get down into the hole.

            Comment


            • #7
              316 work-hardens very easily.
              Use low revs, lots of lube, and steady pressure to keep it cutting. Don't ever let the tool burnish the work, or it will instantly form a tough skin that you'll have hell's delight getting through.

              Comment


              • #8
                Low rpms for the win.
                Remember: SFM recommendations on webpages/books and such are for high production 'moderate' tool life conditions.

                Much lower SFM works fine with HSS tools.
                just think how slow a file or scraper works, Theres really no lower limit other then how long you want to wait for the job to finish.
                Play Brutal Nature, Black Moons free to play highly realistic voxel sandbox game.

                Comment


                • #9
                  Slowly

                  The worst drill you can use for this purpose is a centre drill as if has zero top rake and a very wide chisel edge - with no web-thinning. That drill is going to rub and not cut freely from the very start.

                  Use a drill with a very sharp edge and with the web thinned.

                  A centre drill will quite often drill "on centre" in a lathe but the wide chisel will cause it to "wander" on a mill or drill.

                  If it were me, I'd make a drilling jig/fixture for the "reaming" drill then follow up (outside the jig/fixture) with the reamer.

                  I would use slow speeds and high force slow-revving hand feeds for all drilling and reaming. The set-up and the job will tell you via "feel" how it is going. My reaming would be very slow revs and fed as high as my "feel" would let me.

                  Plenty of cutting/tapping oil.

                  If the job or process hesitates and/or the drill gets blunt and "rubs" it will work-harden the job. A carbide drill may follow-up and finish the drilling but I'd be surprised if the reamer stood up to much cutting in the localised area of any previous work-hardening.

                  I'd have at least four - preferably six - pre-sharpened drills so that as soon as it even hinted at the drill getting blunt it can be replaced immediately with a replacement. Its all too easy - "rushed" or not - to know the drill is losing its edge and to "take a chance" and "give it one more go" and then - bingo - "work-hardening".

                  Its not a matter of how fast you work but rather how quickly you finish the job that matters.

                  Hasten slowly.

                  Comment


                  • #10
                    I am left with only one question from such excellent responses:

                    Is the consensus that I should eliminate a spotting drill entirely?
                    I was going to switch to a 120-degree NC spotting drill.

                    Comment


                    • #11
                      These make great little spotting drills and will walk right through work hardened SS. http://drillcity.stores.yahoo.net/newtuncardri.html Great until you snap one and have to get the broken nub out, that is You need very low runout (ie mill and collet) and as high of RPMs as you can muster. Might or might not be the answer, but it's inexpensive and when they work, they work very well. If you have an HF nearby, they sell a grab bag set of the same thing, just look through the plastic and buy a set with several larger sizes in it. That way you can try them out for $5.

                      I drilled 60 very small holes (1 or 1.5 mm I think) in a watch bezel and only snapped one. I drilled it out with a larger, 1/8" I think, cheap HSS bit, turning the HSS bit into a core drill and pulling it up as a plug. Worked dandy it did. That hole became 12 O'clock and go a larger brass pin pressed in, so the part was saved.

                      Comment


                      • #12
                        I just wanted to follow up. I finished it up and didn't burn a single drill after the suggestions. I stuck with the HSS-Co 120-degree NC spotting drill and it worked just fine. After more than 20, I am sure I can do this job again with one twist drill. I swapped three as I was going to make sure I kept a sharp edge. The problem with the reamer turned out to be almost entirely based on too high a speed on the proceeding drill. It had work hardened the surface and made the reamer chatter until it got a decent cut into it. Not mentioned, but it also came to mind that a spiral flute reamer would help me with the radius on the workpiece. I swapped out my straight flute for a spiral flute midway through. It did produce a slightly nicer finish, but otherwise was negligible in comparison.

                        Thanks again to all that responded. It is truly appreciated.

                        Comment


                        • #13
                          Job well done

                          Arthur.

                          Thanks for the feed-back - appreciated.

                          I'm pleased that it worked for you.

                          I prefer to hand-feed just about everything as I "listen" and "take note" of the "feel" of my machine/tool/set-up combo as it sure will "tell" if you are going right or wrong and when you hit the "sweet spot".

                          It will also tell you if and when a tool is incorrect or "losing its edge" or when it is labouring and rubbing etc.

                          When I am power feeding, I get it right by hand, count the number of turns per second/minute and then use the same counting to set my power feeds.

                          I rarely set my feeds by the so-called "production" methods of "feed per tooth = RPM X Number of teeth". Others may if it suits them.

                          Its usually best to start off with a slow feed and speed and "work up" until you feel its right for you and your job/machine. Cutting oil is needed where lubrication is required and "suds" (aka "soluble oil") or even "spray mist" are required where cooling and perhaps swarf removal are required.

                          Sharp cutters are essential. I think this job of yours has made that point pretty well.

                          Comment

                          Working...
                          X