Threadmilling speeds and feeds check (I don't do it enough to know)
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    1,069
    Post Thanks / Like
    Likes (Given)
    75
    Likes (Received)
    442

    Default Threadmilling speeds and feeds check (I don't do it enough to know)

    On occasion I break out the thread mill when doing some one-off threads. I've got a couple iscar tool bodies with the full form thread inserts. Whenever I use them, it seems it takes significantly longer than tapping. And I think that is to be expected.


    Although when I see people say "just threadmill it" on here, it seems to come with the undertone of, "it is plenty fast".



    So my question is, how fast do you guys run your threadmills? A couple examples:


    Lets say I have a 1/2-13 thread, 3/4" deep, in 1018 using one of these: 1/2-13 Variable Flute Carbide Thread Mill

    Lakeshore's recommendations seem to be 350-500sfm, .0025-.0035ipt. middle of the road numbers would be about 4600rpm at 55ipm.

    Harvey tool's recommendations are about 550sfm, .0016ipt. That is about 6000rpm at 38ipm. But harvey's guide also has an adjustment formula ((major - tool dia)/major), which ends up putting me at 11.4ipm


    Are you guys really running these at 500sfm? I have a long running job, running the lakeshore threadmill, and we settled in at 2000rpm at 3/4ipm a long time ago. Tool life is pretty good, is consistant. I remember we tried going faster but settled in on this after a short period of trial and error, settling on the current numbers just because "it worked"




    Another example (the real reason I'm asking):


    I am running a one off repair job, where I need to mill a 4"-12 thread about 5 inches deep in some sort of steel (seems to cut easy, might be 1018 although the finish I got while boring the hole was nicer than I expected. The part is welded so I don't think it is 12L or similar)

    The only tool I have for this is a boring bar from the lathe dept. 1.5" bar, approximately a 2" diameter. So it is basically a single point, single tooth threadmill. I am running 300sfm (573rpm) at about 8.5ipm (.015 per tooth!!!) now. I had started at like .003" but it really felt like it was creeping along way way way too slowly.

    Even at this speed it takes about 40 minutes to complete the part (in this case, not a big deal, i wander off while it is cutting) but to you people who do this all the time, how fast can I ramp this up to? Can I expect to gain anything on this part?


    Is there another place to look for even different threadmill information?

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,380
    Post Thanks / Like
    Likes (Given)
    2551
    Likes (Received)
    3158

    Default

    Well at that depth I would guess it has to be single point, but for shallower threads, say up to 1" deep (depending on diameter) you can get multi tooth mills so you only need to make 1 or 2 revolutions around the ID of the minor diameter.

    * I see you linked a multi tooth threadmill. You are only going 1 or 2 revs, yes?

  3. Likes BT Fabrication liked this post
  4. #3
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    82
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    27

    Default

    I don't do too much larger than 3/4-16, but I can tell you a lot of machines will have a hard time making a nice circular path at 55ipm at that diameter or smaller.

    Lets say you have a Haas VF?, one would want to turn the quality setting up to medium or finish to help with accuracy. The machine will slow itself down as needed when these settings are on.

    For me in steel, I start with 70sfm and .005" stepover and at least 1 spring pass. Super conservative, but I have yet to break a threadmill, even in inconel/monel. From there you can speed things up or increase stepover distance. To be the most effective, maybe try a bigger stepover with a slow feed/speed to start, and just increase that until you find your diminishing returns.

    I do have the benefit of running 1-offs for prototypes, so taking a little extra time here isn't a huge consequence for me as long as I don't make the thread(pitch diameter) too big on the first cut. If I were running 10+ parts, I would use the first part to try and speed things up as much as I can. But you will either have a larger stepover with slower feed/speed or vice versa. Pretty much always need a spring pass from what I've observed, especially if you are making class 3 threads.

    Just my 2 cents.

  5. #4
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    1,069
    Post Thanks / Like
    Likes (Given)
    75
    Likes (Received)
    442

    Default

    Quote Originally Posted by Mike1974 View Post
    Well at that depth I would guess it has to be single point, but for shallower threads, say up to 1" deep (depending on diameter) you can get multi tooth mills so you only need to make 1 or 2 revolutions around the ID of the minor diameter.

    * I see you linked a multi tooth threadmill. You are only going 1 or 2 revs, yes?
    yes, the 1/2-13 example, I do one depth pass on the rough (doing 2 radial passes, 65%/35%) and do a second circle around on the finish pass. I am climb cutting. I generally use the generated program from SCT (Thread Mill Code Generator – Scientific Cutting Tools, Inc.)

    And the iscar threadmills I use are inserted, 14 and 21mm insert lengths, so I can do many threads in 2 depth passes.

    I always have a skim pass too (so technically it's 3 passes, with the 3rd the same as the 2nd)

  6. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,267
    Post Thanks / Like
    Likes (Given)
    5862
    Likes (Received)
    4014

    Default

    Quote Originally Posted by dandrummerman21 View Post
    yes, the 1/2-13 example, I do one depth pass on the rough (doing 2 radial passes, 65%/35%) and do a second circle around on the finish pass. I am climb cutting. I generally use the generated program from SCT (Thread Mill Code Generator – Scientific Cutting Tools, Inc.)

    And the iscar threadmills I use are inserted, 14 and 21mm insert lengths, so I can do many threads in 2 depth passes.

    I always have a skim pass too (so technically it's 3 passes, with the 3rd the same as the 2nd)
    He's not talking about depth passes, he's talking about how many revolutions you make around the hole.
    For those multi flute thread mills, spiral up twice and done.
    For example if it's a 1/2-13 thread you'd have only 2 lines of code after it feeds down into the hole.
    G03 X-Y-Z IJK
    G03 X-Y-Z IJK
    G00 Z retract.
    M30

  7. #6
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,256
    Post Thanks / Like
    Likes (Given)
    3126
    Likes (Received)
    1648

    Default

    Threadmilling is great for one-offs, short runs, hard materials, when the stock (or previous operation) is very expensive, when a very high quality thread is paramount, or when you don't have enough torque for tapping. For most production in normal materials, I prefer form tapping. It can take some fiddling to get form tapping right (may need to ream the drilled hole), but once it's running it's very fast and reliable.

  8. #7
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    1,069
    Post Thanks / Like
    Likes (Given)
    75
    Likes (Received)
    442

    Default

    Quote Originally Posted by Mtndew View Post
    He's not talking about depth passes, he's talking about how many revolutions you make around the hole.
    For those multi flute thread mills, spiral up twice and done.
    For example if it's a 1/2-13 thread you'd have only 2 lines of code after it feeds down into the hole.
    G03 X-Y-Z IJK
    G03 X-Y-Z IJK
    G00 Z retract.
    M30
    Yes, I knew what he meant. That's why i said I do the thread at one depth at 65% (one G3 revolution), and I do 2 revolutions at 100% (2 G3 revolutions).

    Same as your code basically.

  9. Likes Mtndew liked this post
  10. #8
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,704
    Post Thanks / Like
    Likes (Given)
    1558
    Likes (Received)
    844

    Default

    +1 to being feed rate dependant.
    Successful (fast) threads depend upon your machines controlling accuracy.
    F500 (mm/min) would be max I'd be programmed at for this size (internal) thread.

  11. #9
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,503
    Post Thanks / Like
    Likes (Given)
    402
    Likes (Received)
    965

    Default

    It also depends on stepover. I tend to treat these like a lathe tool and run a few stepovers. I just did an oddball 15/16"x16 thread in a part using Carmex inserted tooling and with a 0.790" cutting diameter 14mm tall insert, I did 650SFM (3140rpm) and 0.0035" per tooth, so 11ipm. I used three 0.015" stepovers. Material was 1018 cold rolled. I also recently did a 304 job with an M6x1.0 thread and a Harvey single point. That one went 150sfm and only 0.0002" per tooth with a four tooth cutter, so 2.55ipm.

    I generally like going faster with lighter cuts and get better tool life and have never had a failure (chipped tooth, etc.). I always just follow the speeds and feeds from the tool manufacturer's website.

  12. #10
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,267
    Post Thanks / Like
    Likes (Given)
    5862
    Likes (Received)
    4014

    Default

    Quote Originally Posted by dandrummerman21 View Post
    Yes, I knew what he meant. That's why i said I do the thread at one depth at 65% (one G3 revolution), and I do 2 revolutions at 100% (2 G3 revolutions).

    Same as your code basically.
    Sorry about that, I must have interpreted it differently.
    No worries.

  13. #11
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    595
    Post Thanks / Like
    Likes (Given)
    252
    Likes (Received)
    460

    Default

    Fi= (Fl x (R-r))/R

    Where:
    Fi= the feedrate for an inside arc
    Fl= the linear feedrate (in/min or mm/min)
    R= the inside radius of the hole to be threadmilled
    r= the cutter radius

    Fl= r/min x Ft x n
    Where:
    Fl= the linear feedrate (in/min or mm/min)
    r/min= the spindle speed
    Ft= the feedrate per tooth of the cutter
    n= the number of cutter teeth

    Is this the formula you are searching for? This came directly from Harvey Tool

  14. #12
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    1,069
    Post Thanks / Like
    Likes (Given)
    75
    Likes (Received)
    442

    Default

    Quote Originally Posted by Houndogforever View Post
    Fi= (Fl x (R-r))/R

    Where:
    Fi= the feedrate for an inside arc
    Fl= the linear feedrate (in/min or mm/min)
    R= the inside radius of the hole to be threadmilled
    r= the cutter radius

    Fl= r/min x Ft x n
    Where:
    Fl= the linear feedrate (in/min or mm/min)
    r/min= the spindle speed
    Ft= the feedrate per tooth of the cutter
    n= the number of cutter teeth

    Is this the formula you are searching for? This came directly from Harvey Tool
    Yeah. I didn't have the formula until I started writing this thread.

    Maybe the question is more related to three things:


    1: why is the answer often "I threadmill everything" when we're talking about a relatively standard size and depth in a relatively standard material that someone might be having trouble with. When it takes 10 seconds to tap a 1/4-20 or 30-40 seconds, the choice is clear. Plus the tap is often an order of magnitude cheaper.

    2: does it seem reasonable for me to spin away at a 4"-12 hole 5" deep for 80 minutes?

    3: why does there seem to be a large discrepancy between feedrates and speeds(the example in my OP had lakeshore's tool doing about .003 per flute while the harvey tool was half that. But the harvey SFM was about 40% higher?)


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
  •