Formula for calculating acceleration distance required when threading.
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default Formula for calculating acceleration distance required when threading.

    Hi,
    My first post, hope I can contribute something back to the forum in the future.
    I have a part on the machine that has an M36 x 4 thread on the end.
    I'm using the tailstock but I'm short of space to get the tool up to speed.
    I seem to remember that the manuals gave a formula for calculating how much distance in Z was required for the threading tool to get up to speed but I can't find it anywhere.
    I've only got about 6mm clearance so I'm running slow which is giving a rough thread.
    I realise that this formula is going to vary depending on how fast the machine can accelerate.
    The machine is a Mori SL25 with a fanuc 16T control (mid 90's).
    Just hoping to get a ballpark figure as I can't afford for the thread to be out of pitch.

  2. #2
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    8,893
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4311

    Default

    Quote Originally Posted by Truckerb View Post
    I have a part on the machine that has an M36 x 4 thread on the end.
    I'm using the tailstock but I'm short of space to get the tool up to speed.
    36 ? That's a decent size, you can't find one of those extended centers that's smaller in diameter and sticks out farther ? Should clear your threading tool niceley and give you more z ?

  3. Likes barbter liked this post
  4. #3
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,168
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Thread error length at start of Thread due to acceleration is calculated as follows:

    TE = 0.002 x RPM x L(Thread Lead)

    Regards,

    Bill

  5. Likes cameraman, Truckerb, barbter, LockNut, SumiSpy liked this post
  6. #4
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Thanks for that Angelw
    I guess the 0.002 value is specific to the machine. Do you know what machine that figure is for?

    I can't use an extended centre unfortunately as it's live, no bearings in the tailstock. (Short of buying a new one).

  7. #5
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,168
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by Truckerb View Post
    Thanks for that Angelw
    I guess the 0.002 value is specific to the machine. Do you know what machine that figure is for?

    I can't use an extended centre unfortunately as it's live, no bearings in the tailstock. (Short of buying a new one).
    There's a bit of math behind it, but its the simplification of the algorithm that can be used as a constant relating to acceleration and can be used with any machine.

    The result is the minimum Z stand off from the start of the Thread. Via hand-wheel, park the Threading Tool at the resulting Z coordinate and at the Minor Diameter of the thread and see what clearance you have with the tail stock. If still interference, it should be slight, particularly with a 36mm OD Thread and then do as HuFlungDung suggests and modify the tool holder.



    Regards,

    Bill

  8. Likes SumiSpy liked this post
  9. #6
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,398
    Post Thanks / Like
    Likes (Given)
    1420
    Likes (Received)
    3816

    Default

    Some threading tools are built in a sort of chunky style that won't allow you to get access near the tail center. Sometimes, these can be improved upon by grinding a clearance notch in the toolholder. It don't need to be beautiful, it needs to do the job.

  10. Likes Bobw, barbter liked this post
  11. #7
    Join Date
    May 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    1

    Default

    Ok, I used Angel's formula with a good safety factor and got it cutting at 165ft/min
    The thread is nice, shiny & clean now.
    Thanks everyone.

    The tool has already had the hell ground out of it

  12. Likes barbter liked this post
  13. #8
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,441
    Post Thanks / Like
    Likes (Given)
    879
    Likes (Received)
    638

    Default

    I’ve been dealing with this myself some lately. Mazak qt15 in my case. I wound up just doing by trial. I did the initial testing with the tail stock out of the way. At least on my machine the lead in required is very rpm dependent.

  14. Likes yardbird liked this post
  15. #9
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,432
    Post Thanks / Like
    Likes (Given)
    5041
    Likes (Received)
    1760

    Default

    Quote Originally Posted by Pete Deal View Post
    I’ve been dealing with this myself some lately. Mazak qt15 in my case. I wound up just doing by trial. I did the initial testing with the tail stock out of the way. At least on my machine the lead in required is very rpm dependent.
    Yeah me too. Formula or no formula im going to watch it run first.

    Brent

  16. Likes Pete Deal liked this post
  17. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,168
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by Pete Deal View Post
    I did the initial testing with the tail stock out of the way.
    How does watching the first run tell you if the tool is starting far enough away from the end of the work to avoid Lead Error? In the OP's case using 165ft/min cutting speed (445RPM), the distance of Lead Error would be 3.56mm, less than one Lead of the Thread. You won't see the error and would have to detect it via measurement.

    If you're referring to possibly hitting the Tail Stock; that has nothing to do with Thread Lead Error, only that where you're starting in Z may have the tool interfere with the Tail Stock. In cases where clearance is going to be tight, I attempt to manually to move the Threading tool to the Z Start and Thread Minor Diameter in X position using the Hand-wheel, with the Tail Stock in place to see if there is any clearance issues. If there's clearance, then there will be clearance when running the Thread Cutting Cycle.

    Quote Originally Posted by Pete Deal View Post
    At least on my machine the lead in required is very rpm dependent.
    Of course it does and that's the case with all machines; hence the RPM being used in the screw cutting operation being included in the algorithm.


    @Truckerb

    You say in your last Post that you're cutting at 165ft/min. Are you running the Threading Cycle with Constant surface Speed (G96)? With the diameter Thread you're cutting, that would equate to circa 445RPM and would only work without stuffing the thread if the upper RPM were clamped at 445RPM using G50, otherwise the start of the thread will be indexed to a new position with every change in RPM brought about by G96 Mode and cutting at an ever decreasing diameter.

    Depending on the material being used, 165ft/min is generally rather slow to use with carbide inserts and would most likely lead to Built Up Edge of the insert. If you're really limited in the distance you can start from the end of the work-piece, then by slowing the Spindle Revs will allow staring closer to the work-piece in Z without Lead Error at the start.

    165ft/min equates to 445RPM and a minimum start distance in Z from the work-piece of 3.56mm. 328ft/min (100M/min) equates to 884RPM and a minimum start distance in Z from the work-piece of 7.07mm.

    Regards,

    Bill

  18. #11
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,432
    Post Thanks / Like
    Likes (Given)
    5041
    Likes (Received)
    1760

    Default

    Quote Originally Posted by angelw View Post
    How does watching the first run tell you if the tool is starting far enough away from the end of the work to avoid Lead Error? In the OP's case using 165ft/min cutting speed (445RPM), the distance of Lead Error would be 3.56mm, less than one Lead of the Thread. You won't see the error and would have to detect it via measurement.

    If you're referring to possibly hitting the Tail Stock; that has nothing to do with Thread Lead Error, only that where you're starting in Z may have the tool interfere with the Tail Stock. In cases where clearance is going to be tight, I attempt to manually to move the Threading tool to the Z Start and Thread Minor Diameter in X position using the Hand-wheel, with the Tail Stock in place to see if there is any clearance issues. If there's clearance, then there will be clearance when running the Thread Cutting Cycle.


    Of course it does and that's the case with all machines; hence the RPM being used in the screw cutting operation being included in the algorithm.

    Regards,

    Bill
    Hi Bill,

    I always just assumed that after you've position the tool at the thread cycles starting point if the G76 thread cycles first initial Z move is towards the tailstock instead of the chuck it was spinning too fast and that move was to create room for it to start. I think I remember you could eliminate this opposite direction Z first move by slowing the spindle down.

    That's why threading left to right and starting up against a shoulder always had me nervous the first time so I'd watch it run first make sure all Z moves are in the correct direction.

    Brent

  19. #12
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,168
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by yardbird View Post
    Hi Bill,

    I always just assumed that after you've position the tool at the thread cycles starting point if the G76 thread cycles first initial Z move is towards the tailstock instead of the chuck it was spinning too fast and that move was to create room for it to start. I think I remember you could eliminate this opposite direction Z first move by slowing the spindle down.

    That's why threading left to right and starting up against a shoulder always had me nervous the first time so I'd watch it run first make sure all Z moves are in the correct direction.

    Brent
    Hello Brent,
    Absolutely not. If you have a value for the included angle of the Threading Insert other than Zero (no compound feed when Zero is specified), the tool actually moves towards the chuck (RH Thread - cutting towards the chuck) to the appropriate Z Start so that the tool is cutting on the leading Edge of the insert.

    The control has no idea where the actual part is, therefore it doesn't know to make any move to create room for it to start. What if the chuck end of the part is set as Z Zero; Okuma used to always show Z Zero set that way in program examples. If the Tail-stock end of the part is at Z150.0 with the Thread starting at, say, Z160.0, the control has no idea whether the Thread is at the end of the shaft, or halfway along it. Accordingly, it would be illogical for a control to force a move in the Z+, particularly when the MTB is cognizant that there can be a Tail-stock frequently involved.


    Regards,

    Bill

  20. Likes barbter liked this post
  21. #13
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,124
    Post Thanks / Like
    Likes (Given)
    935
    Likes (Received)
    536

    Default

    As an aside...I've always used the value of 5mm.
    Also for rigid tapping on the mill - R value (5) for spindle synch.
    Never any issues and cutting a range of thread sizes from M3 to M30.
    I appreciate the formula is the correct way, but I got the 5mm (0.2") value from here many years ago from a long thread (no pun!).
    The conclusion was that using this value, would always be "safe"...

  22. #14
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,168
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by barbter View Post
    As an aside...I've always used the value of 5mm.
    Also for rigid tapping on the mill - R value (5) for spindle synch.
    Never any issues and cutting a range of thread sizes from M3 to M30.
    I appreciate the formula is the correct way, but I got the 5mm (0.2") value from here many years ago from a long thread (no pun!).
    The conclusion was that using this value, would always be "safe"...
    Hello barbter,
    Its not correct that it "would always be safe". It all comes down to the spindle revs and the Lead of the Thread.

    In an earlier Post I gave the example of the OP's M36 x 4 being cut with a more acceptable cutting speed for carbide inserts. Even the 100M/min I suggested in the example is quite conservative, but better than the 50M/min the OP was using. As the OP has a clearance issue with the Tail-stock, it becomes a compromise between the RPM that will allow the tool to start at a distance that will avoid Thread Lead Error and a cutting speed that won't damage the insert via built up edge.

    At 100M/Min, the RPM of the spindle would be specified at 884RPM and that results in a minimum start distance in Z from the work-piece of 7.07mm for the 4mm Lead Thread. Accordingly, you can see in this example, your 5mm wouldn't be safe.

    The fact is, many don't even realize that the first part of a thread they're cutting has a Lead Error; its not all that obvious by eye. The Thread is cut progressively deeper until the Nut or whatever screw on gauge they may be using fits and they call it done.

    Regards,

    Bill

  23. Likes barbter liked this post
  24. #15
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,957
    Post Thanks / Like

    Default

    Quote Originally Posted by Truckerb View Post
    Thanks for that Angelw
    I guess the 0.002 value is specific to the machine. Do you know what machine that figure is for?

    I can't use an extended centre unfortunately as it's live, no bearings in the tailstock. (Short of buying a new one).

    https://www.riten.com/wp-content/upl...nters-2021.pdf We have the "long point" centers on all the machines.

    FWIW, I almost always set start point two thread leads off part..

  25. #16
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,124
    Post Thanks / Like
    Likes (Given)
    935
    Likes (Received)
    536

    Default

    Quote Originally Posted by angelw View Post
    Hello barbter,
    Its not correct that it "would always be safe". It all comes down to the spindle revs and the Lead of the Thread.

    In an earlier Post I gave the example of the OP's M36 x 4 being cut with a more acceptable cutting speed for carbide inserts. Even the 100M/min I suggested in the example is quite conservative, but better than the 50M/min the OP was using. As the OP has a clearance issue with the Tail-stock, it becomes a compromise between the RPM that will allow the tool to start at a distance that will avoid Thread Lead Error and a cutting speed that won't damage the insert via built up edge.

    At 100M/Min, the RPM of the spindle would be specified at 884RPM and that results in a minimum start distance in Z from the work-piece of 7.07mm for the 4mm Lead Thread. Accordingly, you can see in this example, your 5mm wouldn't be safe.

    The fact is, many don't even realize that the first part of a thread they're cutting has a Lead Error; its not all that obvious by eye. The Thread is cut progressively deeper until the Nut or whatever screw on gauge they may be using fits and they call it done.

    Regards,

    Bill
    Thanks for your detailed reply Bill.
    Yes fully understand the whole pitch and RPM issue - that's why i said "safe"...
    I guess a better word would have been "standardised"....as in all threads we produced were in a range where that worked.
    And progs were then all standardised where operators always saw the same R/approach values which was great as a double check.
    All said i do remember an issue we had once on the lathes - coarse (bastodial) thread prototype which was coarse pitch and ally.
    I had siemens shopturn controls and this did alarm with a SPOS (by memory) error which was spindle positioning (in this case synch).
    Solution was reduce RPM.
    Cheers

  26. #17
    Join Date
    Feb 2011
    Location
    ct. usa
    Posts
    36
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    9

    Default

    the way i would get around the tail stock interference would be to long hand the threading cycle with G32 programming
    start further from the face in the Z axis and high in the X axis (movement is down the tail stock ) this gets the Z axis moving at the required speed from further away from the face of the part before you start threading

    M3Sxxxx
    G0X40Z10
    G32X36Z5F4.
    Z-xxxxx
    X40

    G0Z10(REPEAT until threading is done)


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
  •