Results 1 to 9 of 9

Thread: milling advice

  1. #1
    Registered
    Join Date
    Oct 2009
    Location
    Canada
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default milling advice

    Im just wondering exactly what some milling general rules are.

    At work I just finished a job on 304SS, where I had to mill some slots in a turned piece. I had to take a full tool cut with my endmills, and after about 150 pieces, 3 slots on each at a depth of about .080", I had eaten 2 uncoated endmills. No one in the shop was angry or anything, infact it was pretty acceptable, I just want to know if/what I could have done better.

    I took my cuts at 50sfm and .002 feed per tooth.

    What I guess im trying to say is that, taking the endmill right into a full cut worked, but it was putting a lot of stress on the machine, although I dont quite see how it is avoidable, and I think that is basically what ate the end mills. I know 304SS is a b***h to machine and it does eat tools however.

    What are some general rules, as far as taking full diameter cuts, plunging into a part - ive heard you should ramp down your plunge at a 15 degree angle - etc?

    Is it just the material? like I said I dont see how you could avoid taking full diamater cuts, I could have taken a bit at a time, say half the tool diameter but it would have taken a lot longer to machine (initally I had my finishing cuts at .001 fpt, and bumping to .002 saved over 40 seconds on the program), and I still would have had to feed in the whole tool to the point where it was halfway into the material before I started moving the length of the slot.

    Any advice would be appreciated

    Thanks

    Similar Threads:


  2. #2
    Registered christinandavid's Avatar
    Join Date
    Aug 2009
    Location
    New Zealand
    Posts
    661
    Downloads
    0
    Uploads
    0

    Default Slotting with Endmills

    Hi,

    End Mills don't like cutting full diameter at shallow depth. It is preferable to plunge at least 1xdiameter so that cutter is well supported. Downsides of going deeper are swarf build-up and cutter pushing-off.

    My strategy would be to rough slots using undersize slot drill/ripper cutter then finish with end mill.

    If you only have size end mill available, you could ramp to depth over the length of the slot then back-track to the starting position at depth.

    Push your feed until cutter breaks then back off a bit. The extra pressure on the cutter will help support it and the fewer cuts per slot the better.

    DP



  3. #3
    Registered
    Join Date
    Oct 2009
    Location
    Canada
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    well I had pushed the feed up to .004 per tooth, but left an undesireable surface finish. .002 was where it was good. Id rather not break an endmill either! haha.

    Thanks for the tips.



  4. #4
    Registered
    Join Date
    Jan 2010
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Have you ever tried using Hanita Varmill Solid Carbide End Mills with TIALN coating? These end mills have an A-Symmetric Helix. I did not see where you stated the diameter or corner radius of the end mills or the type end mills used except they were uncoated.

    I use the Hanita end mills mentioned for cutting 15-5 Stainless that I mill with. I have taken full depth cuts with no coolant and it will do it but it is hard on the tools.

    Using a 1.0" crescut Hanita end mill with a .05 fillet radius, I normally take no more than
    .350 depth of cut and no less than .050 depth of cut at 1500 rpm @ 15 ipm. I use Hangstefers Hard Cut oil for coolant and a finish end mill that is not crescut to make my finish side & facecuts with a .030 radius. A .0025 chip load per tooth works well.



  5. #5
    Registered
    Join Date
    Oct 2009
    Location
    Canada
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Hanites are our endmill of choice actually. However this job required zero corner radius and I was just using whatever I could find in the shop. Was plain uncoated hss.

    I realized I was actually conventionally cutting, which could have made an impact, although I was full diameter cutting so that was probably what was eating them mostly.

    Can anyone give me any advice on plunging?

    I had to make a jig out of 1018 the other day and I was originally going to pocket everything by using a 15-20 degree ramp to depth, but was advised not to as id likely break the end mill.. was told no more than a 3 degree ramp.. which seems pretty insane as 3 degrees is pretty much nothing and the ramp would be so long to get to any real depth necessary.

    I know for softer materials like aluminum and brass that plunging isnt really any sort of a problem. I really dont see why it would be any problem as long as the end mills are designed for it, which they are. 4 flutes, 2 go right across the diamater and 2 dont, so they are made for plunging..

    I just dont see how in say some steel job requiring pocketing how youre going to get away with not plunging, sure you can drill a hole.. but it wouldnt be to the depth and youd have to plunge the endmill at somepoint anyway, and a 3 degree ramp just doesnt seem practical to me, because if the pocket isnt huge, what are you going to do?

    Thanks!



  6. #6
    Registered
    Join Date
    Jan 2010
    Location
    USA
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    Drill the hole as you said. This will prevent your end mill from trying to center cut when you plunge back into the drilled hole. Then just mill out as needed. Even dished end mills can plunge some, as long as you mill out where the center of the tool began or try not to plunge too deep with a dished end tool that will gaul up the center up the tool. I am plunge milling into a shallow pocket with no starter hole, at 5 ipm and then I kick it up to 16 ipm. RPM is 1690. Cutter is a .750 Hanita Vara-Mill Solid Carbide TIALN Coated, material is 15-5 Stainless, about 32-36 RC. I then take a .010 finish depth cut and finish out the sides and bottom of the pocket.



  7. #7
    Registered BobWarfield's Avatar
    Join Date
    May 2005
    Location
    USA
    Posts
    2501
    Downloads
    0
    Uploads
    0

    Default

    The rule of thumb I use for plunge in my G-Wizard calculator is the normal feed rate for the cut (plunge is equivalent to a full width) divided by the number of flutes. The more flutes, the more iffy a plunge can be due to chip clearance problems.

    A ramp or helix is always gentler on the cutter. If you can plunge at a particular speed, you can certainly ramp at the speed. 3 degrees sounds tame, I tend to use 6 degrees more often. In terms of 13 degrees breaking the cutter, there will be a feedrate that is faster than the plunge and slower than a normal slot cutting feedrate that should be fine even with that steep a ramp.

    I may try to see if I can find any recommendations on ramping feedrate. Of the top of my head I would think you could use trig to create a blended feedrate based on the ramping angle.

    Cheers,

    BW

    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html


  8. #8

    Default

    My understanding is that SS work hardens so you need take reasonably agressive cuts. each pass to break through the work hardended area on the next pass.

    David



  9. #9
    Registered
    Join Date
    Jan 2010
    Location
    usa
    Posts
    34
    Downloads
    0
    Uploads
    0

    Default

    i would helix in and then peel mill ss at 180. ipm with a 3/8 titan 5 flute coated carbide em ( chatter free terminator) with 4650 rpm



Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed