A decent speed and feed chart - Page 2
Close
Login to Your Account
Page 2 of 5 FirstFirst 1234 ... LastLast
Results 21 to 40 of 85
  1. #21
    Join Date
    Mar 2006
    Location
    Northern California
    Posts
    529
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    12

    Default

    I'm with CarbideBob.

    To get good feeds and speeds, you need two things: a good calculator and calibration.

    As some have said, the calculator will get you a starting point. It performs an even more important role though, which I'll come back to in a second. First, let's look at this idea of calibration.

    Calibration means bringing the real world experience and data into the equations that the calculator uses. A feeds and speeds calculator starts with its own internal tables of what the chiploads, surface speeds, tweaks for different materials, and all the rest should be. That's a database, and the best calculators will make it possible to "calibrate" that database with your experience, your tooling, and your shop's best practices.

    You can plug in your tooling manufacturer's recommendations right away to the database. There's a few other things to plug in as well if the calculator is able to take them, such as what the spindle power curve looks like.

    But then the experience and shop best practices have to kick in. Every time you make a cut, you have the opportunity to learn something. Make it a little faster than you did the last time. Fiddle the variables. And keep a record of it. Whether the cut works well or breaks the cutter, both are important as they're helping to map out the envelope for that cutter, that machine, and that tooling under your shop's best practices. All that information needs to go into a database that's linked to calculator for best results. Done right, it's easy to track and easy to take advantage of. That calculator + database should do most of the record keeping work.

    Once you have some of that data to go from, the real value of the calculator emerges. While a lot of variables have to be calibrated, there are also a lot that can be calculated and that are very predictable. Radial chip thinning is a real effect that works the same every time on every machine. The role of different tool engagement angles for HSM toolpaths are well understood. Tool deflection is predictable and can be calculated.

    This means your precious data collected from real jobs is reusable in new jobs that may have slightly different parameters. The stepover or depth of cut may need to change for a new job, and maybe you will only make one or a small number of the parts so no experimentation is possible. Take your calibrated database which is hopefully built into the calculator and let the calculator tell you what to do there. Since it's been calibrated by your real world experiences in your shop with your tooling, it's going to be pretty bang on right about it.

    Combining a database with a calculator that considers a lot of variables (about 50 at last count) is what G-Wizard does.

    Cheers,

    BW

  2. #22
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    940
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    220

    Default

    Makes me wonder how I've survived this long without a 'calculator', short of my trusty TI-89.

    It does seem redundant to me to use a starting point, develop tool paths, record that data in a database when most are using CAM systems with this technology on-board.

    The procedure I use...

    1. Record tool holder, gage length, tool ID, machine tool
    2. Pick starting chip-load & rpm
    3. Pick axial DOC for testing (this will not change for this portion of test)
    4. Test cut at set radial DOC; say 0.5mm
    5. Increase radial cut by set increment; say 0.5mm
    6. Record stable and unstable cutting modes (no chatter present)
    7. Rinse and repeat at +500 rpm

    What you will find are the stable cutting speeds, and from there, you can increase the axial DOC to find best MRR for that material with that combination of tool, holder, etc..

    It use to take me ~30 minutes to run through this procedure once the machine was ready to go. Harmonic software negates the step-increment to find stable lobes, which speeds things up considerably.

    Anyhow...

    All of this data goes into the CAM system... because all of the setup data should come out OF the CAM system for the operators; ie, the gage length, holder ID, tool ID, etc..

    All of the data is logged into the CAM system for the type of cut being performed as a "process" or whatever your system supports, such that a separate database is simply not necessary.

    Warning: stable lobes will tax machine HP, so pay attention to your load meter. A good cutting condition will remain stable right up to the machine's limits, especially with large cutters.

    There are plenty of variations on this technique and I'm all eyes to reading them, but my point in all of this is that most have the capabilities right there in their CAM system to log 'best' conditions for future reference.

    My 2.5 centavos

  3. #23
    Join Date
    Dec 2009
    Location
    Newtown, CT
    Posts
    104
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    5

    Default

    I've gotta say, the guys that always play it safe and go slow, they tend to stay at their skill level.

    Push the machine to its working limits, but don't do crazy stuff. Often times I will see someone slow a machine down because "the cutter burned up last time because it was going too fast." I watch the program and see that their real problem was chip evacuation and they were double and tripple cutting a mound of chips and little shavings. So basicaly slowing it down increases how many hours the cutter will last during the day, but you still get the same amount of parts out of it.

    I like to do things with inexpensive cutters if I can. I always start at the top of speed and feed and dial back from there. A carbide 1/2" 3 flute cutter costs under $40, we can easily make up for that cost by reducing our WIP time.

    We do not do large volumes of parts so our conditions will be much different than others. If we are making a bunch of parts and the program runs faster than the operator can debur the part, I will slow the program down slightly to save some tool life.

    Like I tell my trainees- If you break a tool in half because you are pushing it too hard I will not be upset. If you BURNISH a tool into oblivion, you are not a machinist.

  4. #24
    Join Date
    Mar 2006
    Location
    Northern California
    Posts
    529
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    12

    Default

    There's several things to consider with the scenario you bring up, Chuck.

    First is, does your CAM do the database work? You say most of them do, but they don't. Esprit does (which I seem to recall you use or used) and a few others, but there are a ton of them that don't in the mid to lower-end CAM systems that a lot of shops are using.

    Second is, does the CAM have enough feeds and speeds calculation that you can use the data you derived from the test runs in a variety of situations, or do you pretty much have to rerun the tests for most combinations? You're largely concerned about discovering the stable (chatter free) envelope which involves fixing a few variables, but there's more going on. Stable chatter zones can be figured out pretty quickly and that data re-used on a big variety of cuts if you have a calculator that will extrapolate. There's a fair bit about that here:

    CNC Milling Chatter and Stable Milling Speeds

    I haven't seen any CAM programs that have that much feed and speed calculation built in. It's fine if all the work you do involves making enough parts that it's no big thing to do all the test runs, but for many, that isn't the case. You reference new test runs at multiple axial depths. Shouldn't be needed once you understand the chatter envelope if you have a calculator that can deal with that. Axial depth and radial depth are variables you'd like to change over a pretty wide range without having to rerun the tests. That's a lot of test time that could've been saved.

    Last one is, what's the starting point if you don't have the test data available and don't want to run the tests? Lots of guys want starting points for say HSM toolpaths at a particular tool engagement. Or maybe for a micro-cutter that's going to have deflection problems. The things and a lot more aren't covered by the basic calculators. The closer you get to a decent answer the less trial and error testing is needed to get out to the edge of the envelope.

    TylerP, couldn't agree more about the problems with recutting chips a lot of folks seem to have.

    Cheers,

    BW

  5. #25
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    940
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    220

    Thumbs up

    Quote Originally Posted by BobWarfield View Post
    There's several things to consider with the scenario you bring up, Chuck.

    First is, does your CAM do the database work? You say most of them do, but they don't. Esprit does (which I seem to recall you use or used) and a few others, but there are a ton of them that don't in the mid to lower-end CAM systems that a lot of shops are using.
    We'd have to define "most" and a "ton" some time but I will go ahead and refine my statement to, "most of the better CAM packages" allow process saves and the like. hyperMill, Esprit, UG/NX, Catia, and probably many more that I don't know much about.

    Anyone care to chime in on the packages you're using?

    Second is, does the CAM have enough feeds and speeds calculation that you can use the data you derived from the test runs in a variety of situations, or do you pretty much have to rerun the tests for most combinations? You're largely concerned about discovering the stable (chatter free) envelope which involves fixing a few variables, but there's more going on.
    Sure there is. This was hardly an attempt at any kind of dissertation on the subject.

    Stable chatter zones can be figured out pretty quickly and that data re-used on a big variety of cuts if you have a calculator that will extrapolate.
    How does your calculator do this, because this is the part I'm really interested in!

    Run us through an example of how G-wizard does this if you don't mind.

    I'll cover the rest of your questions tomorrow.

  6. #26
    Join Date
    Dec 2007
    Location
    grants pass, Oregon USA
    Posts
    229
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    83

    Default

    With drills, my rule of thumb is this- If it breaks, its goin too slow. If it burns up, its goin too fast. If you are using insert cutters, the manufacturer's recommendations are usually kinda optimistic. I start at the lower end and work up cautiously. I never get on the guy's cases if they are working on up reasonably and push it too far. But if I hear SQUEEEEEAAAAALLLLL- Tink- silence...... on the first try, I know they were not even in the ballpark. That's when I yell "I HEARD that!!!!!!!!" and they know an ass-chewin is on the way. I hafta confess tho, I don't even remember the calculations I started with early in my career. I just kinda have an experienced idea where to start and go from there. In the slavery production shop I worked in for a while (huge quantity parts ONLY) the rule of thumb from above was "push it till it breaks then back off 10%". Now I actually use the recommended s&f fom the tool makers.


    Cheers!
    Tom

  7. #27
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    11,736
    Post Thanks / Like
    Likes (Given)
    51
    Likes (Received)
    8988

    Default

    We really need more information about what the shop environment is like.

    I have used a few CAM packages. I am using EdgeCAM now. I would consider this a pretty decent CAM system. It really has no cut information database. You basically get to assign a feed and speed for "rough" and "finish" for a given material. You can set up as many materials as you like for each cutter.

    If I was in a mold shop and all I ever had to machine was P20 and H13 with the same dozen or so cutters, I could make one hell of a good database. The tools are sometimes long or very small in diameter, but the setups are usually rock solid.

    Now the flip side is the job shop. Material could be D2 tool steel or 356 cast aluminum. The part could be a 400lb billet or a .25 in think hollow casting. You might have to be able to run the same job on a 50 taper or a 40 taper depending on machine availability. There is no database in world that can possibly include all of those variables.

    What the job shop needs is a good starting point. That could come from a chart or a calculator of from good old experience.

    Example:

    Today I had to machine 10 aluminum castings with a 37mm bore 5 inches deep. Called about an insert drill when I first saw the drawing. 6 week lead time.

    I scrounged around and found a 1" solid carbide end mill 6" long. I had about .8" to hold onto with a hydraulic holder. What kind of calculator is going to tell me what speed and feed to run that at?

    I decided on 1000 SFM, 60 IPM and .050 in/rev helical interpolation. Cut like butter. Upped the speed to 75 and called it good enough.

    No chart needed.

  8. #28
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    11,736
    Post Thanks / Like
    Likes (Given)
    51
    Likes (Received)
    8988

    Default

    Quote Originally Posted by moaprecision View Post
    With drills, my rule of thumb is this- If it breaks, its goin too slow. If it burns up, its goin too fast. If you are using insert cutters, the manufacturer's recommendations are usually kinda optimistic. I start at the lower end and work up cautiously. I never get on the guy's cases if they are working on up reasonably and push it too far. But if I hear SQUEEEEEAAAAALLLLL- Tink- silence...... on the first try, I know they were not even in the ballpark. That's when I yell "I HEARD that!!!!!!!!" and they know an ass-chewin is on the way. I hafta confess tho, I don't even remember the calculations I started with early in my career. I just kinda have an experienced idea where to start and go from there.
    Wow. Feeds and speeds for drills are the easiest of all tools to calculate. Insert drills are a little tricky, but usually well documented. You might want to blow the dust off of your solar calculator and save some money on drills.

  9. #29
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    940
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    220

    Default

    Quote Originally Posted by ewlsey View Post
    We really need more information about what the shop environment is like.

    I have used a few CAM packages. I am using EdgeCAM now. I would consider this a pretty decent CAM system. It really has no cut information database. You basically get to assign a feed and speed for "rough" and "finish" for a given material. You can set up as many materials as you like for each cutter.

    If I was in a mold shop and all I ever had to machine was P20 and H13 with the same dozen or so cutters, I could make one hell of a good database. The tools are sometimes long or very small in diameter, but the setups are usually rock solid.
    Can't say what every shop uses, but these are materials used regularly in our mold shop:

    Stavax variants
    Polmax
    PX5
    P20
    S2
    Aluminum alloys: RSA varieties, 6061T6, cast
    Copper Nickel
    CPM 10V and other variants
    H11 & H13
    1045
    Nak 55 and 80
    Vanadis
    Moldmax
    Electroless Nickel
    ...and quite a few I'm forgetting before my morning coffee

    More or less than you might have thought, I dunno.
    We've developed & databased (hyperMill) cutting parameters for all of these, and for the various breeds of machine in our shop, from the HSK32 spindles that don't do well with anything over 8mm to the HSK63's. There are plenty of shallow and deep cavity tool-holders in the mix as well, and that's probably par for course in most diverse mold making environments.

    What are the other mold guys working with out there?

  10. #30
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    11,736
    Post Thanks / Like
    Likes (Given)
    51
    Likes (Received)
    8988

    Default

    I haven't done any mold programming, but are P20, S2, H11, H13, 1045 really that different to machine?

  11. #31
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,234
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2656

    Default speeds and feeds

    Quote Originally Posted by stephon0913 View Post
    hello all i want to ask a question to some ppl that will be able to answer this question once and for all. does anyone know of a good reference guide or chart for speed and feed rates based on tooling and material??? also i wanted to know what everyone uses for this. most the time i start out with an experienced guess and go from there. theoretically i would like a chart or grid that i look at that would tell me the max speed and feed i can use for the tool and material combonation, or better yet when i choose the tool in mastercam it already loads it for me. any help on this is greatly appreciated!
    .
    i use an Open Office Calc spreadsheet calculator. it is free. it needs data inputted on cutting conditions and does dozens of complex calculations in a millisecond. you would need a very big chart to take into account all cutting conditions. a few like

    1) chart is a starting point. take 304 stainless. annealed is much different to machine than cold worked sheet metal. the hardness can double or triple. this means machining rates can vary 300%

    2) what are you doing? turning, milling, drilling. sfpm can vary 300% depending onhow you are machining.

    3) coolant what and how applied? i got a $90 metal cutting carbide tooth portable circular saw at HF that cuts 3/8" steel plate at about 6500 sfpm. try that with an end mill and it won't last long. air cooling does work if done right.

    4) heat buildup. cutting a deep slot with an end mill needs slowing down compared to a low DOC with a face mill. often sfpm can vary 300%

    5) feed. sometimes a higher feed with the heat being carried away by the hot chips works. i seen feed vary 300% depending on conditions

    6) depth of cut, width of cut with end mill can vary machining rates 300% or more. For example some cut hardened steel with carbide end mills but at a very low depth of cut and a fairly high feed. Or side milling that is a high DOC but low stepover or width of cut is faster. teeth are in cut maybe 10% per revolution compared to 50% when slotting. this can easily increase metal removal rate 50% easily

    7) coated carbide can influence friction and can lower or eliminate the need for coolant. sometimes coolant is not so much for cutting as keeping part at a consistent temperature so tolerances are easier to hold

    8) horsepower and cutting forces. charts rarely tell you a sfpm at feed with diameter and DOC with end mill with so many flutes will need so much horsepower and will push part with so much force. Cutting force i always calculate ahead of time.
    .......many a machine works fine til you get to a certain horsepower limit and it will chatter and vibrate and or part will chatter or bend from cutting forces. i have seen part move in vise and break end mill with pieces flying at high speeds far more than i care to admit.

    9) cutter shank material and length. carbide is stiffer and stronger than steel. cutting conditions can increase metal removal rate easily 10x higher by using a short carbide end mill compared to a long length HSS end mill. i have seen putting an end mill a 1/4" more into collet and the shorter stickout allowed increasing metal removal rate 200%. Going from a long length end mill to a stub length can easily increase metal removal rates 1000% or more. i have never seen this on any machinist charts.

  12. #32
    Join Date
    Jan 2011
    Location
    PA
    Posts
    420
    Post Thanks / Like
    Likes (Given)
    136
    Likes (Received)
    121

    Default

    Its unfortunate but the best answer to your question is: their is no answer. Really the best you can do is push it until it breaks or you get scared of it breaking. If you do it this way and take good notes maybe you can make your own chart some day, but since all shops and machines are different your charts would most likely not be a lot of help for someone else in another shop.

    That being said I have been getting good results using G-Wizard with some slight tweaks here and there to suit my machines.

  13. #33
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    940
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    220

    Default

    Quote Originally Posted by ewlsey View Post
    I haven't done any mold programming, but are P20, S2, H11, H13, 1045 really that different to machine?
    Take P20 and PX5; similar materials, PX5 was designed to be used in the same applications as a replacement for P20. It finishes better and while it can be machined at the exact same speeds as P20, you'd be losing 20% of the cycle time in doing so.

    The material is more expensive and many moldmakers have drawn the conclusion that, "It's just not worth it to use PX5 in our shop over tried and true P20".

    So be it, they can make their molds 20% slower for all I care... it's good for business.

    Quote Originally Posted by DMF_TomB View Post

    .......many a machine works fine til you get to a certain horsepower limit and it will chatter and vibrate and or part will chatter or bend from cutting forces.....
    Chatter has absolutely nothing to do with reaching any theoretical horsepower limit. From where are you drawing this conclusion? Please site the sources.

    Thanks

  14. #34
    Join Date
    Aug 2011
    Location
    Portland, OR
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    1

    Default

    Wow ive been taught to start slow and work up...???

  15. #35
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    940
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    220

    Default

    Experience will give you some idea where to 'start', but ultimately, there is no right answer that automatically pops out of a spreadsheet. Anyone who'd like you to believe as much simply doesn't understand the dynamics at work.

    If you notice, most are examining cutting conditions from the tool-to-part. Why? Because it's a lot easier than accounting for the system dynamics, because... you can't really do that without testing and/or using the right software, period.

    This subject always falls off the deep end, because everyone has what works for them, and very few truly care about dedicating the time necessary to getting the most out of their tooling. Simple fact, they already have it figured out. Me... I don't... I test, preferably with the right software for the job. Those who can't make the investment, can still test in whatever way they like, or just settle for what works for them.

    GL

  16. #36
    Join Date
    Feb 2004
    Location
    Staten Island NewYork USA
    Posts
    3,786
    Post Thanks / Like
    Likes (Given)
    1110
    Likes (Received)
    1820

    Default

    Want some good general Speeds and feeds. Check out the Charts in the Machinist Handbook.

    It's all there and are good ballpark figures to start with.

    I took the materials I use most, pulled the SFM in both Carbide and HSS then arranged them in columns along with Feed rates. Made a separate area for Drilling. Also tossed in the equations to get RPM.

    Real basic, real simple and until I got a feel for it I used pretty often, copied a chart to put by each machine.

    Tweaking or just trying to get a job to run better...then look at your tooling manufactures charts, call their tech support and often you'll find you can increase time and tool life substantially.

  17. #37
    Join Date
    Oct 2011
    Location
    new mexico, usa
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default speeds and feeds

    With the internet, check what the manufacturer of your toolbits or inserts that you are using. If you are using carbide tooling a base rule of thumb I learned and teach here at our community college is 3x the cutting speed for HSS tooling. Catalogs can be helpful as well(ENCO, Travers are 2 of my favorites).

  18. #38
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,365
    Post Thanks / Like
    Likes (Given)
    711
    Likes (Received)
    1824

    Default

    Actually, the big catalogs for J&L used to have a nice feed and speed guide line in the very back of their catalogs. They are now MSC, but they use that big blue book now, and I'm not sure if the charts are in that book. But if you can find someone with an old J&L book, go to the back, it gives a nice reference, or at least some starting points.

  19. #39
    Join Date
    Jun 2011
    Location
    New York
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    I use this app.

    Machinist Calculator SFM
    ApplicationSoft
    Category: Utilities

  20. #40
    Join Date
    Dec 2009
    Location
    Kansas City, MO
    Posts
    29
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    4

    Default The answer is...

    "it depends". The reason it depends is cutting metal is still more art than science. We have not done a good job as a profession in defining hard and fast rules for cutting metal. The problem is three fold:
    1. The number of variables is huge (machine tool, cutting tool, part material, fixturing device, final part design, machine method employed, etc...)
    2. New technology in cutting tools, machining methods, and machine tools keep making old parameters obsolete.
    3. We're too busy trying to make money!

    One particular variable that is more controllable today is the stepover from one pass to the next. On a ZIG tool path, the stepover is always the same, but for most parts, this cut pattern is unacceptable. So we use cut patterns that are offset from the area to be machined. Most of these offset patterns have large variations in the amount of stepover the tool encounters (increasing the amount of tool pressure and reducing tool life or breaking the tool).

    There are some tool path engines now that do a great job of controlling the stepover and increasing efficiency (like Volumill). Even with a superior cut pattern, it is still necessary to perform experiments to develop the most efficient combination of feeds and speeds, because of all the other variables listed above.


Tags for this Thread

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
  •