Announcement

Collapse
No announcement yet.

Need Tough Face Mill - Advice?

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

  • Need Tough Face Mill - Advice?

    My next door neighbor has me milling S-7 steel blocks for him, to prep them to become molds for plastic parts. I have to shave more than 1/8" off them, and prep the sides to leave a lip for the host machine to grip. I currently have a Kennametal KSSR-3-TP3 face mill that uses TPG-322 inserts. S-7 is tough stuff. The inserts don't last that long.

    I need to look for another face mill that uses an insert better suited for tough steels. APKT? SPG? Octagonal? What would work best? Ebay has a LOT of face mills. Shars has some interesting stuff. Cabin Fever is coming up, and they always have good stuff. So... What do I look for?

  • #2
    What hardness is the steel you are milling?
    No one can make recommendations without knowing this.

    -D
    DZER

    Comment


    • #3
      How much horsepower/rigidity do you have availible?

      I have two Kennemetal 4" facemills at wrork that use CNMG-422 inserts wich are negative rake inserts nomally used for turning.Those facemills running some Kennemetal KC850 inserts will mill some tough materials.I use them to rough down rail steel on a semi-regular basis.

      They do take some power to run,the vertical head on our old universal mill is 5hp and these will use every bit of it.I don't think Kennemetal is making them anymore,but Dorian was.



      One bonus is they use four edges of the insert that aren't commonly used in turning so you can use the other four in a turning holder and get double life out of the inserts.
      I just need one more tool,just one!

      Comment


      • #4
        As far as tool steel goes, S7 is actually pretty easy cutting. However, it will tax the limits of a Bridgeport-type machine and I found that positive rake inserts worked best. Also, anything larger than a 1" cutter is going to get the mill shaking and require a smaller DOC and slower feed. Your mill may be in better shape than those I've used, but I always have better luck with a 1" positive rake cutter.
        George
        Traverse City, MI

        Comment


        • #5
          Originally posted by Doozer View Post
          What hardness is the steel you are milling?
          No one can make recommendations without knowing this.

          -D
          I agree. You need to know the hardness. If it's too hard no carbide insert will hold out long enough to finish the job.
          It may need to be ground, and I know it's a lot of grinding. An aggressive CBN wheel with coolant may do the job.

          JL................

          Comment


          • #6
            Originally posted by George Bulliss View Post
            As far as tool steel goes, S7 is actually pretty easy cutting. However, it will tax the limits of a Bridgeport-type machine and I found that positive rake inserts worked best. Also, anything larger than a 1" cutter is going to get the mill shaking and require a smaller DOC and slower feed. Your mill may be in better shape than those I've used, but I always have better luck with a 1" positive rake cutter.
            Hi,

            Don't think I've ever seen a pre-hard S7, and I've bought and milled a couple tons of the stuff over the years. George is correct that S7 is sweet to machine, HSS or carbide.

            If you are using a Bridgeport style machine, anything much over a 1 1/2" will quickly over power the mill. Particularly if you trying to move a lost of steel per pass. And the chatter will quickly destroy any insert edge.

            To maximize what you can get from your Bridgeport, I would try a TPG321 insert, and maybe uncoated. Sometimes uncoated is better for longer tool life. Hold your cuts to less than .050" deep, and feed faster. Lighter depth of cut will allow you increase your rpms and then feed rate. This formula worked quite well for the 15+ years I spent making punches and dies from S5 and S7.
            If you think you understand what is going on, you haven't been paying attention.

            Comment


            • #7
              Well then if it's annealed a 2" 45* integral shank face mill would do the trick.The one in the vid is from Shars with Iscar inserts.

              Shars R-8 shank 3 insert 45* facemill running Iscar SEKT 43AFR-HM inserts @ 1100 rpm/.006" per revolution and .200" DOC in Hotrolled 1018 plate.


              This is hot rolled 1018 on a 2hp Bridgeport VS head .200" doc and .006" per rev.

              This one here in fact-

              Last edited by wierdscience; 01-02-2019, 03:22 PM.
              I just need one more tool,just one!

              Comment


              • #8
                SEHT or SEKT insert on whatever size face mill your mill is happy to spin. Not toughest geometry but easier cutting than say TPG on a lightweight bridgeport mill category.

                Then if you have horses to spare and 6000+lbs mill octagon-shaped ODMT insert would offer you eight cutting edges.
                Location: Helsinki, Finland, Europe

                Comment


                • #9
                  Thanx.

                  Yes, S-7 is easy to cut. Easier than O-1, harder than 1018. My 1.5HP Bridgeport shakes, but does it just fine. Curly chips fly all over the city! After the second run, I'm indexing.

                  I'll look for a 2-1/2" SEHT or SEKT mill. What about APKT?

                  Comment


                  • #10
                    Hi,

                    If your Bridgeport is shaking, I'm surprised you aren't blowing edges faster. And it won't matter what style insert you use the life span will be short and brutal.

                    Back off the depth of cut until all shaking and chatter goes away. Then be amazed at how longer your inserts last. Or put up with the short life and buy more inserts. Choose one or the other - you don't get both. And now you understand why Bridgeports aren't much better for heavy machining than heavier benchtop machines.
                    If you think you understand what is going on, you haven't been paying attention.

                    Comment


                    • #11
                      Sounds like a good idea. Will take longer, but be cheaper.

                      Comment


                      • #12
                        John, if switching to a 1.5" lets you run your passes faster with a higher chip load and run the full depth it may not be any slower than having to "baby" the bigger cutter you have (3"?) to stop it from chattering and shaking as much as you're getting. Sure you have to make more passes. But if those passes are faster it all comes out in the end.

                        And if running the cuts more smoothly also means extending the life of your inserts by 4 to 8 times over shocking them into chipping then that's a further major bonus.
                        Chilliwack BC, Canada

                        Comment


                        • #13
                          Originally posted by BCRider View Post
                          John, if switching to a 1.5" lets you run your passes faster with a higher chip load and run the full depth it may not be any slower than having to "baby" the bigger cutter you have (3"?) to stop it from chattering and shaking as much as you're getting.
                          My first reply was done in a rush, but that's what I would have said if I'd taken the time. At my last shop I had at least a dozen high quality face mills to choose from but the smallest of them, the 1" Sandvik, turned out to be the quickest at material removal. Anything larger required backing off on the feed and DOC. The 1" could be run as fast as you could crank the handles and at more than twice the DOC of a 2".

                          I'm sure the insert played a part as well, as the Sandvik inserts had a very positive rake. The CNCs didn't care what cutter we tossed in, but the Bridgeports had some preferences.
                          George
                          Traverse City, MI

                          Comment


                          • #14
                            Oooh! Good stuff! Saved me from a stupid purchase.

                            I have a couple of 1" end mills. I'll try them, first.

                            I have my eye on a couple of used 1-1/2". So, SEKT or APMT are good? I'll have to look to see what the used shell mills take.

                            Comment


                            • #15
                              Originally posted by John Buffum View Post
                              Oooh! Good stuff! Saved me from a stupid purchase.

                              I have a couple of 1" end mills. I'll try them, first.

                              I have my eye on a couple of used 1-1/2". So, SEKT or APMT are good? I'll have to look to see what the used shell mills take.
                              If you need a 90* corner use APMT,if you want higher feed rates with less radial load on your spindle bearings and can tolerate 45* shoulders use SEKT.One extra benefit of SEKT inserts is you get four cutting edges per insert instead of two with the APMT.
                              I just need one more tool,just one!

                              Comment

                              Working...
                              X