end mill life question


Results 1 to 5 of 5

Thread: end mill life question

  1. #1
    Member
    Join Date
    Jan 2007
    Location
    USA
    Posts
    92
    Downloads
    0
    Uploads
    0

    Default end mill life question

    I am cutting a lot of 1018 CRS steel plate (rated hardness 167 Brinell), usually either 1/4 thick or 3/4 inch thick. I am using a 2 HP step pulley Bridgeport converted to CNC with ballscrews for X and Y axis. The parts are held solid to the table, and backlash does not appear to be an issue.

    I am experiencing quite short tool life, and think perhaps I am cutting too aggressive, or have the wrong tools. I typically use uncoated solid carbide either 1/4 inch diameter or 1/2 inch diameter, varying from 2, 3 or 4 flute cutters. I am limited to a maximum 2720 RPM on the spindle. For the carbide tools, I typically use a SFM of 400 and a chip load of .0016 for the 1/4 dia cutter or .0032" for the 1/2 dia cutter. The chip load is based on a recommendation of a CNCZone member (I forgot his name) of .0064 * diameter per tooth. My cutting speed is calculated based on the SFM and chip load plus the number of flutes on the cutter. I am using a water based flood coolant. The member also suggested a maximum depth of cut (DOC) of 40% of the cutter diameter. I find that if I use anything over .060 DOC for the 1/4 dia cutter that I get some blue chips which means they got real hot even with flood coolant, so I usually limit my cuts to .060 DOC.

    Many of the cuts are what amount to slots of width equal to the cutter diameter, since I am cutting complex shapes out of a bar of steel. My cutters seem to get dull rather quickly, usually within less than an hour of use, and then often snap off. I have tried using the minimum extension from the collet to avoid flexing, but need about 1 inch extension to achieve the 3/4 inch final depth.

    Should I be using a coated cutter? Perhaps a larger diameter? Maybe a roughing cutter? Or a ball end metal removal mill (is that really a good idea)? Different SFM? Different chip load? Is a cutter with a length of cut of 3/4 inch OK for this application? Should I change to mist coolant so the air will blow chips out of the cut? I do try to remove as many chips as I can before the next pass to avoid problems.

    Based on the above SFM and DOC and chipload, if I use larger diameter cutters, I get a higher cutting speed, which is always desirable of course, but the cutters cost more and I end up with a little more scrap. I do not seem to have the power necessary to drive a 1/2 inch diameter end mill at 400 SFM and 0.0032 chipload per flute and a maximum DOC of 0.200 inch, so I usually compromise on a shallower DOC.

    Another possibility that I have available is to operate my Bridgeport at a frequency higher than 60 Hz from my VFD. Using 120 Hz would result in a spindle RPM maximum of 5440. I have been reluctant to push the motor and spindle bearings to that kind of speed, since I don't want to destroy a motor or spindle. Any thoughts on what is safe here?

    I have considered having the parts rough cut using a waterjet or similar and just taking finish cuts to conserve tool life, but don't know if this is economical. I also considered using 12L14 steel for easier machinability, but Speedy Metals only sells it in round shapes, not flat. Maybe another metal supplier?

    Similar Threads:


  2. #2
    lixingwen1987's Avatar
    Join Date
    Jun 2014
    Location
    116323
    Posts
    0
    Downloads
    0
    Uploads
    0

    Default

    KIND. ATTN. –PURCHASE DEPARTMENT AND PRESIDENT

    DEAR President and manager , GOOD DAY

    I AM GLAD TO TAKE THIS OPPORTUNITY TO INTRODUCE OURSELVES AS ONE OF THE LEADING SUPPLIERS OF Precision Bearings use for CNC and Machine tool ,AND Radial-Axial bearings WHICH ARE MAKE OF Wafangdian Tianjiu Bearings Technology Co.,Ltd.

    WE ARE IN THIS BUSINESS SINCE LAST FIFTEEN YEARS; IN THIS SPAN OF TIME WE HAVE SUPPLIED PRECISION IN ALMOST ALL THE CONTINENTS OF THE WORLD.

    BESIDES, WE DEVELOP HIGH-PRECISION YRT ROTATED BEARINGS, MACHINE TOOL MAINSHAFT BEARINGS AND MOTOR PRECISION BEARINGS. THE PRECISIONS OF OUR BEARINGS HAVE REACHED LEVELS OF P5, SP, P4 AND UP.

    FEATURED BY HIGH PRECISION, LOW NOISE, HIGH ROTARY SPEED, HIGH QUALITY AND LONG SERVICE LIFE, OUR PRODUCTS SAVE USERS’ COST AND SHORTEN PURCHASE TERM. WIDELY APPLIED TO COMMON MACHINE TOOLS, CNC MACHINE TOOLS, LARGE / MIDDLE MOTORS, PRECISION ROLLING MILLS, ETC., OUR PRODUCTS FILLED THE DOMESTIC BLANKS AND CAN SUBSTITUTE IMPORTED PRODUCTS.

    THIS IS TO INFORM YOU THAT WE HAVE PRECISION BEARINGS AND OTHER GOOD QUALITY BEARINGS AVAILABLE, CAN SUPPLY FOR YOU WITH BEST QUALITY.

    WE HOPE CAN CORPORATION WITH YOUR COMPANY.

    WE CAN SUPPLY OUR BEST PRODUCTS FOR YOU.

    THANK YOU !

    REGARDS?

    --------------------------
    Lixingwen?????
    Wafangdian Tianjiu Bearings Technology Co.,Ltd.
    (Wafangdian Heavy Bearings Researching & Manufacturing Co.,Ltd.)
    Brand?WZFB
    Web: ??????????????? ????????????????
    Tel: 0411-85366785
    Fax: 0411-85366785
    Mobile:+86-15942617721
    E-mail:lixingwen@wzfb.com
    Q Q : 178702120
    Skype: lixingwen1987

    Do our best to give customer best service.



  3. #3
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    206
    Downloads
    0
    Uploads
    0

    Default Re: end mill life question

    I went online and found SFM calculator. at 2720 RPM you are at 178 SFM on 1/4" and 356 on 1/2" end mills. Coated carbide on my CNC is normally run about 500-900 SFM without coolant and the chips are almost black from being so hot. The object is to put all of the heat into the chip to keep the tool and work piece from over heating. I would not advise you to run the Bridgeport any faster or you could destroy the head. MSC .com and check out some coated cobalt or High speed steel coated end mills and run them according to mfg specs. about 100 to 250 SFM. If you have mist coolant, use KOOL TOOL oil in it, with enough air to blow the chips away from the cut. recutting chips destroys carbide almost instantly, running water based coolant on a carbide end mill will reduce its life to 20% or less . As the flute is in the cut it heats up, upon exit the coolant causes it to cool off rapidly. Carbide is so hard and brittle and the thermal shock that it encounters on each revolution starts to microscopically fracture the razor sharp cutting edge and dull. this is what is causing your mills to snap off. If you can get by with 1/2" cutters I would suggest you ruff it out with coated cobalt fine tooth ruffer and leave about .02" on the wall for finish pass and come back with different 4 flute coated carbide to finish. On the 3/4" thick make the ruffing pass in 3 passes and on the 1/4" 1 pass. If you have ball screws and solid mount anchor bearings then Climb Mill, NOT Conventional Mill as you would on a lead screw Bridgeport. Climb milling will allow the flute to engage a determined bite and work around thinning to Zero. on Conventional milling the flute engages at zero and the chip progressively gets thicker. this builds a very large amount of unnecessary heat and adds force into the cutter to start developing a chip. If you need any more info PM me your phone # and I will call you at night.

    Good Luck
    Farmers Machine



  4. #4
    Member
    Join Date
    Jan 2007
    Location
    USA
    Posts
    92
    Downloads
    0
    Uploads
    0

    Default Re: end mill life question

    Thank you very much for your detailed reply. That is very interesting and explains a lot. As I understand you recommend using mist cooling with Kool Tool (I found Cool Tool II oil, is this the same?) for carbide instead of flood coolant to avoid shock cooling. Is water based flood coolant OK with HSS or cobalt tools? I am about to add a good flood coolant system to my mill and may change my mind if it is not the best idea. I have seen some systems that just use air to blow the chips away and provide some cooling without lubrication. Is that a good idea for carbide?

    Bob



  5. #5
    Member neilw20's Avatar
    Join Date
    Jun 2007
    Location
    Australia
    Posts
    3757
    Downloads
    0
    Uploads
    0

    Default Re: end mill life question

    Lots of air and no coolant for carbide. Micro-chipping of cutter with the coolant causing thermal shock as stated by Farmers Machine.
    As much energy removed by the chips as possible. Blue-black chips are fine, and they always hurt!!
    3 flute cutters, I have found work well in slots, because the 'back side' can't react against the front. 3 flute cutters are a bit stiffer, too.
    Always climb mill.
    Working in slots is always a problem because climb milling is next to impossible when contact is more than 30-40% of the diameter.
    Multiple passes in a slot with a smaller cutter might be a solution, but your depth of cut will be reduced and number of passes takes much longer.

    Reduced feed as cutter starts into a cut, from an edge, can help.

    Doing a lot of work on SS316L (low carbon) my initial cutter life went from 20 minutes, moving towards 4 hours with experience.
    I discovered that once a tooth had dulled, making it work harder, to even up the wear on the other teeth, made the cutter come back to life!!
    I found as soon as it was starting to turn pear shaped, I upped the feed by 20% until it settled again, then became less aggressive.

    I discovered this at the end of a BIG production run while stretching the life of the last few cutters. <<'cutters' link (if you got the link) to advert NOT BY ME. What dumb sh1t is this??.!! What is VigLink?? Grr!!!

    This did eventually, after some delay, fix it!! Opt Out of VigLink



    Last edited by neilw20; 01-10-2015 at 12:46 PM. Reason: last paragraphs added.
    Super X3. 3600rpm. Sheridan 6"x24" Lathe + more. THREE ways to fix things: The RIGHT way, the OTHER way, and maybe YOUR way, which is possibly a FASTER WRONG WAY!


  6. #6
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    206
    Downloads
    0
    Uploads
    0

    Default Re: end mill life question

    "Cutting Tool Engineering " is a very informative magazine on metal working tools. go to their web site and subscribe for free. Just answer a few questions. Their current issue has a lot of ads for end mill manufactures.

    Good Luck
    Farmers Machine



Tags for this Thread

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 for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

end mill life question

end mill life question