Steel Feeds and Speeds
Close
Login to Your Account
Likes Likes:  0
Results 1 to 16 of 16
  1. #1
    Join Date
    Aug 2004
    Location
    So Cal
    Posts
    157
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    38

    Post

    Hi guys,

    I've been doing pretty good so far with milling aluminum on my CNC mill, now I need to do some steel work. I basically have zero experience with milling steel on a CNC. I've done some stuff on manual machines but that doesn't quite count. I'm looking for some guidance on what variables to use. Ie; SFM, chip load, DOC, etc.

    My mill is a Hurco VM1. The parts I need to cut will be @ 1/8th to 1/2in thick.

    Is 1018 the “all around” type of steel that is generally used? I don’t need any super hard alloy, just need a good finish, easily machinable, and reasonable steel strength. The only thing I’ve tried so far is 12L14 from McMaster. It was for a small part lot and indicated good machining characteristics. It did machine very well, and left a extremely good finish. I used a 3/8ths cobalt end mill at @ 500 sfm and @ .003 chip load. There seems to be a much broader range of available stock dimensions in 1018.

    Can I use my current carbide endmills (used with alum) on the steel if I remain in the acceptable sfm and chipload parameters?

    Is there a general sfm, chip load spec that I can use a base? At what point does dry cutting come into play, with carbide insert cutting?

    I appreciate any guidance for a steel newbie.

    Mark

  2. #2
    Join Date
    Mar 2005
    Location
    Hermosa Beach California
    Posts
    3,665
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    77

    Post

    1018 is VERY soft...

    Getting a nice finish ( shiny and even )
    Requires LOTS of SFM...

    I preffer 8620 over 1018 anyday...

    I think 1018 sits somewhere around 2-3 Rc
    And 8620 is closer to 8-10 Rc...

    Both are very soft... But 8620 will give a nicer finish at a slightly lower SFM...

    Also 8620 is VERY good for heat treating...

    I dont know about strength... i only know 8620 is slightly harder...

    Does that equal strength ? i dont know...

    As far as price goes...

    We ussually pay around .75 per pound of 1018...
    and about .90 per pound of 8620...

    So not a huge difference in price unless you plan on getting 10,000 pounds worth...

    [img]smile.gif[/img]

    good luck

  3. #3
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,518
    Post Thanks / Like
    Likes (Given)
    49
    Likes (Received)
    98

  4. #4
    Join Date
    Aug 2004
    Location
    So Cal
    Posts
    157
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    38

    Post

    Thanks guys, much appreciated. Now I'm thinking I need to learn more about the different steel alloys.

  5. #5
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,865
    Post Thanks / Like
    Likes (Given)
    3563
    Likes (Received)
    3017

    Post

    Mark,
    I've found Hu's speed and feed recommendations he posted for download on the OneCNC board to be right on the money most all the time. If you downloaded that and substituted it into your tool table, it will make an expert of you right away. If you haven't gotten the file yet, you need to get it.

    In steel rectangular stock there's "available" and "readily available". 1018 is really the only widely available cold finished flat stock from a variety of sources and in a good selection of sizes. Re-sulfurized free machining stock like 1117 or the leaded stocks like you mentioned above are available in flats, but not widely so unless you're a major user. The popularity of 1018 is due to decent (not great but passable) machinability plus good weldability. None of the more free machining chemistries are weldable. When all is said and done, the variety of chemistries and alloys is just not there in steel flats like it is in rounds.

    There are times when its better to use hot rolled stock for milled parts instead of cold rolled. Hot rolled is in an essentially fully annealled state, so it doesn't have the tendency to warp from an imbalance of residual rolling stresses when face milled, etc like cold rolled stock will often do, particularly in thinner sections. However, its generally worthwhile to bead blast or pickle HR stock to remove the scale if any substantial amount of milling is to be done. Mill scale has about the same effect on cutters as ground up glass would have, and its not the most friendly thing for your machine ways either.

  6. #6
    Join Date
    Aug 2004
    Location
    So Cal
    Posts
    157
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    38

    Post

    Thanks Munchr, just the info I needed!

    I just downloaded HU's tool list, quite a bunch of info. So, would 1018 be equivilant to "steel up to 7% carbon" or what?

    To be brutally honest, I don't typically use the material and chip load auto-calc. At first I just really wanted to learn, and get the “feel”, for cutting aluminum so I manually calculated everything with my trusty sliding chip load chart. Then, I just got used to knowing what and how fast I could go. I found the material sfm and chip loads in that table to be extremely conservative. For aluminum, I typically go way faster than it recommends but still retain excellent tool life. I know steel is another ballgame altogether and you must go slower or suffer major tool life consequences.

    Mark

  7. #7
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,241
    Post Thanks / Like
    Likes (Given)
    1796
    Likes (Received)
    797

    Post

    Mark,

    I find Hu's feeds for aluminum and steel really close. (IMHO)
    But, when I tend to use insertable Iscar mills, I kick the feed WAY up.
    Using Hu's stuff will put you in the ballpark.

    1018 is the "base" steel around here. It is 1018 in cold finish, and called A36 when in hot finish. (I'm sure that they are a little different in composition, but for all intense and purposes, they are the same)

    4140 H.T. is my favorite steel to machine, with A516-70 about second.
    Both machine really well, and are predictable with tool life. (once again, IMHO)

    1018 (36KSI) is about the cheapest, with A516-70 (70KSI) second, followed by 4140 (130KSI).

    Have fun,

    Doug (Vision)

  8. #8
    Join Date
    Mar 2004
    Location
    Philomath, OR USA
    Posts
    104
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    Where does one get Hu's tool list. I was unable to locate it on the OneCnC web site, but I'm also not a member and it appeared to require that you owned their software.

  9. #9
    Join Date
    Mar 2006
    Location
    usa
    Posts
    188
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    I cut a lot of 1018 and hot rolled on my haas.

    one part in particular is a hog out 2. x 2.5 x 4. bar stock. I will use a 3/4 hanita cobalt 6 flute ticn coated .

    I will take a 1.5 depth of cut and a .08 side cut at 400 rpm feeding at 5.ipm .

    Ive tried different strategies with carbide ect.
    For my machine and my style of machining and the hanitas are only $38.00 a pop , i can get 18 parts a end mill. its the most bang for the buck AND I AM NOT BEATING THE HELL OUT OF THE MACHINE.

    I can walk away for the machine and do something else with out worrying about something bad happening.

  10. #10
    Join Date
    Jan 2003
    Location
    Phoenix, AZ
    Posts
    2,091
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    89

    Post

    Monafly

    You have to have Onecnc software to use the tool and material list.

    Hu's tool lists are just one of the many benefits of Onecnc

  11. #11
    Join Date
    Apr 2005
    Location
    Prineville, OR
    Posts
    112
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    When you really want to start machining steel in the 1018-1117 class, go get you some Hanita varimills. They are a 4 flute rougher with a varible helix and a .030"x 45deg. chamfer on the corners for retaining edge strength at the bottom of the endmill.

    I rough with these endmills at 800SFM taking .004-.005" per flute chip load and cutting depth equal to the diameter. I finish at about 1000SFM, but I'll use hanita's 5 or 6 flute for this operation.
    With these numbers on long-term continous production, I'm getting phenominal tool life.

    The tools are carbide, but I can't remember what their coating is off the top of my head. If you order the varimill, there's only one option on coating anyway.

    I've been running them now for nearly 3 years and will never go back to anything else for machining 400 series stainless or mild steel. They flat kick ass.

  12. #12
    Join Date
    Aug 2004
    Location
    So Cal
    Posts
    157
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    38

    Post

    How do those Varimills work in aluminum?

  13. #13
    Join Date
    Apr 2005
    Location
    Prineville, OR
    Posts
    112
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    I've only ran a couple of odd jobs....nothing on a production basis, but I think they would work okay.

    You really can't crossover with a premium steel milling cutter over to a premium aluminum cutter.

    Aluminum needs really good flute depth and a very high positive rake to shine, where is that same geometry would go to hell in a handbasket on steel, pushed to the same limits of course.

    I've used high-helix endmills intended for finishing steel in roughing applications and also used them for aluminum, but when you want to start moving aluminum at over 700IPM, you'd better start looking for something like dataflute endmills or some of the others that are out there.
    I haven't ran enough serious aluminum production to be much of an authority on the subject, but steel I push harder than most anyone you'll talk to.


    I scare my tool salesmens when they see what I do with their stuff. They've sent over about a half a dozen guys from other shops to show them what they can accomplish with hanita endmills because the average guy just can't buy into it without proof.
    The cool thing is, i've gotten lunch twice out of the deal.....can't beat that.

  14. #14
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,865
    Post Thanks / Like
    Likes (Given)
    3563
    Likes (Received)
    3017

    Post

    Mark,
    In the material list that shows up on the tool page there's an error regarding carbon content. It shows 4% max C and 7% max C. Should be .4% and .7% This refers to XR. Don't know about XR2. I've had it for 3 or 4 months but haven't had time to load it yet and spend some time to become familiar with the changes.

    The last 2 numbers in the designation of carbon steels is the carbon content. 1018 has nominally .18% C. 1045 would be .45% C. etc etc. The same holds true for common alloys like 4140 at .40% C, but the effect of alloying elements like chrome and nickel have more influence on the speeds you'd run than does carbon content alone. Most hot rolled flats are less than .4% C if they carry a structural designation like A-36.

    As Doug and Matt said, when you get into inserted cutters or high performance carbide endmills, you have to use the manufacturer's data as a starting point. But, once you determine workable speeds and feeds for them, its easy to add any tool like that to the OneCNC tool table so you can just plug it in when that's the tool you're planning to use, and let the program crunch out the rpm and ipm from the sfm and fpt data.

    In general, its not worthwhile to mess with hss endmills for general steel cutting. Even the generic carbide endmills last so much longer that their cost per part is a fraction of hss. The time savings due to higher overall production rates is another benefit on top of the long tool life. You'd probably be smart to stay away from the high performance carbide endmills while you're in the learning mode, because they sure ain't cheap. You can buy decent generic coated carbide endmills in 1/2" size for $20-$23, and you don't have to stop and have a memorial service for a major loss when a little whoops kills one of them. Once you're comfortable with steel milling, then its worthwhile to move up to the high performance cutters. What some of them will do, and how they'll survive, will leave you scratching your head in amazement

  15. #15
    Join Date
    Apr 2006
    Location
    Boston
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    Hey Natchamp

    I wrote a speed & feed calculator that's the balls. Email me at [email protected] if you want a copy of it.

  16. #16
    Join Date
    Feb 2006
    Location
    Ohio
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    Natchamp is being modest when he says I've been doing pretty good so far with milling aluminum on my CNC mill", his work is top shelf.

    With regards to feeds and speeds I have used a program for about two years now called ME Consultant, now called ME-Pro that has been invaluable to me so I brag it up at every opportunity, there is also a whole lot more to it then feeds and speeds.
    http://www.mrainey.freeservers.com/

    In addition to Hu's tool list he also put up a material list on the OneCNC user forum that is a great help also.


Bookmarks

Posting Permissions

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