Welcome to Our Community

Some features disabled for guests. Register Today.

Feeds and speeds calculator - an online resource 2015-08-20

Free online feed and speed calculator

  1. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    Josh B submitted a new resource:

    Feeds and speeds calculator - an online resource - Free online feed and speed calculator

    Read more about this resource...
     
    dddman likes this.
  2. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    I'm not really sure how to use it... what is the purpose of the yellow boxes? Why doesn't the feed/speed change when I change the depth of cut?
     
  3. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    dddman, it's a little twitchy when you start changing the yellow boxes. I found that if I input the bit info and max spindle speed and then give it a moment, it'll catch up with itself. If you change too many things randomly it seems to get confused. I didn't have to enter depth of cut, once I hit calculate the DOC box was populated by the program. Also, I think the purpose of this calculator is to give you the ideal depth of cut and feed rate based on the bit and spindle max spindle RPM's. Just a starting point, I guess. I could be wrong though.
     
  4. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    5.5mm DOC @24k RPM @1263 mm/min... scary! But I have to try it now...
     
  5. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    that is relatively slow for aluminum... (-:
     
  6. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    Even for our OX?
     
  7. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    I'm limited to a max RPM of 12,000, that puts me at around 681 mm/min with a .125" carbide bit with a 45 degree helix and ZrN coated...sssllloooowwwww! Beats buying them from someone else though.
     
  8. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    At what DOC are you cutting?
     
  9. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    I haven't cut any aluminum yet, just got my bits ordered. I will probably use 0.076 as a starting point. I think you have to check the "slot/pocket" box to get a depth of cut.
     
  10. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    Definitly my OX can't handle those settings in aluminum... too much flexing in the Z axis
     
  11. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    dddman,
    I've been messing around with this calculator and, your right, the yellow boxes are goofy. Feel like I'm playing Wac-a-mole while trying to input information. But, I believe I have it figured out. The DOC it generates is based on a large, solid mill that a large manufacturer would use. I've found that if I populate all of my tool parameters and then in-fill my target DOC, it will adjust everything to match.
    Here is a link to one of my calculations: http://micro100.hsmadvisor.com/?page=FrontPage&shell_id=247&load_tool_id=4657 .
    Also, I've attached the manufacturers technical data sheet for the end-mill I'm going to use. You'll need this manufacturer data to get the recommended chip load, axial depth of cut and radial width of cut. Use these to populate the DOC and WOC boxes in the calculator, they will override the suggested values given by the program (give it time to calculate, it's rather slow). As you can see, I should only be cutting at a depth of 0.12 mm when pocketing, plunging, slotting or roughing, at a speed of 681.40 mm/min. I will probably tweak these numbers a bit outside the recommended suggestions but not too much as these bits are costly. I'll just have to be patient and let the mill...well mill!
    Hope I haven't added to the confusion.

    Josh
     

    Attached Files:

  12. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    I'll try those settings tonight :)
     
  13. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    fast, shallow cuts are much better than slow deep ones. Mark runs the C-beam at 0.5mm deep cuts in aluminum. it can probably do more, but at that depth it can cut fast and clear the chips properly and stay within it's limits, after all it is not half at on of cast iron! if you want to cut 20mm deep at a time, you have to spend for the cast iron!

    example
     
  14. dddman

    dddman Master
    Builder

    Joined:
    Mar 2, 2014
    Messages:
    466
    Likes Received:
    181
    What are the other cutting settings he uses? FR (bor X, Y and Z) , spindle speed, what kind of endmill?
     
  15. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    David,
    I regards to setting up the gcode for aluminum, do you guys use the same parameters (F & S, DOC and WOC ) for the entire string? Or are you joining codes each with different setting ( plunge, pocket, slot, profile....) All of these variables are a bit overwhelming and I don't want to start off my aluminum milling with breaking a bit.
    For reference, I'm cutting on a standard OX machine (450 mm x 750 mm) using a 400 W, 12k RPM spindle. I will be using the Aluma-Mill 3825 bits - .125" 2 flute 45 degree helix end mill. I know what my SFM, chiploads and depth of cut need to be but I'm uncertain where this WOC% needs to be. I guess my biggest piece of confusion is when do I need to account for the axial width of cut % which is found in the feeds and speeds calculators. Is this the amount of step over? Changing this % changes everything else drastically. Can I just calculate everything assuming 30% WOC, similar to the step over in SketchUcam? Any help is appreciated.

    Josh
     
  16. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    you will need to ask @kram2422 since I set up the basic cut file but he may have changed the feed speeds for that test.
    I set them high (2500mm/min) to make the simulator quicker (-:
     
  17. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    again, @kram2422 is the man to answer this definitively.

    however, any feed speed that will work for a 100% width of cut will be fine for anything less, though maybe a little slow for production runs. any slot cut is 100% width, pockets and large holes will use stepover%. if you have ramping turned on then the initial hole for a large hole ( > 2 x bitdiam), will be ramped in without any plunge at all, which will be a 100% stepover helix so any holes have to be using a feedrate suitable for 100% stepover.

    There is no way to seperate the feed rates for the initial helical hole and the rest of the boring process, unless you want to manually edit the Gcode. so, just go with the 100% WOC settings and it is all going to work (-:

    Remember that 50% stepover is the worst possible setting in terms of tool life since the cutting edges SLAP the surface at 90 degrees every time it starts to cut. Sandvik Coromant recommend 30% or less, or 70% or more.

    One big thing to keep in mind is chip clearance. You never want the the tool to re-cut a chip, ie get a chip between the tool and the thing being cut. This results in accelerated tool wear and a rough surface finish. Think about putting a bit of wood on your dining table and then cutting it with an axe. The wood will make a dent before being cut!
     
  18. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    Just to be clear: Say I have a single plate to mill which will require plunging, pocketing, slotting and profiling. If I use SketchUcam to produce 4 different gcode files, one for each process, and each with different feed rates, depth of cut and width of cut. When joined using gcode joiner, does each individual cut profile retain there parameters once joined? Or are they all mashed together using a single feed rate, doc and width of cut? Hope I'm making sense with my question.
    Example;
    Slotting and Plunge - DOC = 0.0304 mm , WOC= 100% , Feed =681.47 mm/min @ 12,000 RPM
    Pocketing - DOC= 0.08 mm , WOC= 40% , Feed= 693.78 mm/min @ 12,000 RPM
    Finishing- DOC= 0.1 mm , WOC= 30% , Feed= 725.08 mm/min @ 12,000 RPM

    When joined, will the joined cut file keep these parameters separate?

    Josh
     
  19. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    for each file, all the code from and including the G90 command up to but not including, except the last file, the
    G0 X0 Y0 line, is included in the output.
    since the feed rate is applied after the G90 line, yes, that will be retained (-:
     
    Josh B likes this.
  20. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    FYI, keep in mind that the "length" input field refers to tool stick out! I was inputting the actual tool length :duh:. Duh, no wonder I was only getting .03 mm DOC's...112 passes in 1/8" material would take a long time.
     
    #20 Josh B, Aug 31, 2015
    Last edited: Sep 1, 2015
  21. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    784
    Likes Received:
    362
    as a rough guide, here are some settings from a cut Mark did in aluminum. I do not know what bit he used, only that it is 1/8".
    you can save this to a .tpi file in your profiles folder and load it as a tool profile. read the help about 'sharing tool profiles'.
    this was used on a C-beam plate maker which is stiffer than an OX.
    Code:
    [profile]
    prof_spindlespeed=15000
    prof_feedrate=800.0.mm
    prof_plungerate=250.0.mm
    prof_savematthick=0
    prof_matthick=3.175.mm
    prof_cutfactor=109
    prof_bitdiameter=3.175.mm
    prof_tabwidth=8.0.mm
    prof_tabdepth=50
    prof_safetravel=6.0.mm
    prof_usemultipass=1
    prof_multipassdepth=0.5.mm
    prof_gen3d=0
    prof_stepover=30
    prof_mustramp=1
    prof_rampangle=4.0
    
     
  22. Josh B

    Josh B Veteran
    Builder

    Joined:
    Nov 4, 2014
    Messages:
    96
    Likes Received:
    25
    Thanks David, I appreciate your help.
     
  23. motopreserve

    motopreserve Veteran
    Builder

    Joined:
    Jul 3, 2015
    Messages:
    127
    Likes Received:
    51
    Great resource. Thanks for posting and all the follow up info.

    Quick question: do you guys do anything different if you are using diamond cut or chip breaker bits. I never see these listed as "type" and wondered if there is something that should be changed to account for the differences in the standard/provided boxes?

    Appreciate the help.
     
  24. Mark Carew

    Mark Carew OpenBuilds Team
    Staff Member Moderator Resident Builder Project Maker Builder

    Joined:
    Jun 28, 2013
    Messages:
    1,949
    Likes Received:
    1,125
    Here is where I got the test bit in the video
    http://www.precisebits.com/products/carbidebits/precisebit-stub.asp?tsPT=!!!2Flute_StubMill_FishTail!!!
    To be honest I do not remember the exact one ordered
    But I believe it was the last one on the page MN208-1250-019FC
    To be honest I am still looking for a good aluminum cutter out there.
    I have seen great cuts being made with the cutter from Brandon Satterfield @997.1 of SWM3D
    http://www.smw3d.com/single-flute-end-mill-1-8/
    So you may want to give it a go.
     

Share This Page

  • About Us

    The OpenBuilds Team is dedicated helping you to Dream it - Build it - Share it! Collaborate on our forums and be sure to visit the Part Store for all your Maker needs.


    [email protected]

  • Like us on Facebook

  • Support Open Source FairShare Program!

    OpenBuilds FairShare Give Back Program provides resources to Open Source projects, developers and schools around the world. Invest in your future by helping others develop their future.

    Donate to Open Source