Why can't threading speeds be changed on CNC lathes?


Results 1 to 15 of 15

Thread: Why can't threading speeds be changed on CNC lathes?

  1. #1
    Registered
    Join Date
    Dec 2006
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default Why can't threading speeds be changed on CNC lathes?

    I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Jan 2007
    Location
    USA
    Posts
    355
    Downloads
    0
    Uploads
    0

    Default

    Interesting...

    was the programmed feedrate in inches per minute or inches per revolution? I can understand i.p.m. messing up the threads if the rpms change, but you'd think that i.p.r. would sync to the spindle speed.

    It should be possible to cut tapered threads in G96 (constant surface speed) mode if the feedrate is programmed in i.p.r.

    Also, (If I recall correctly), the Cincinnati lathe I ran years ago locked out any speed or feed overrides in threading mode.

    Even the vertical machining centers lock out speed & feed overrides while in tapping cycles.

    Weird.



  3. #3
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    My best guess would be that the acc/dec rate of the Z servo is constant. When you change spindle rpm, the feedrate increases proportionately for threading at the higher rpm, however, the servo still cannot accelerate any faster than it did before, and it has to accelerate for longer to get to a higher feedrate.

    A certain number of cpu cycles is required to detect the encoder index, and to initiate motion. Since the time delay between detection and motion is fixed, it seems reasonable to assume that a faster running spindle has managed to turn a little bit further than it did previously, before the servo gets up to higher speed at the faster rpm. This amounts to a change in timing.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #4
    Registered jackson's Avatar
    Join Date
    Oct 2006
    Location
    United States
    Posts
    586
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Hogger View Post
    I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.
    Well some machines you can use the the override on the control it kind of a pain cause you have to wait for it to come back to the z stat poin then ajust the override

    individual who perceives a solution and is willing to take command. Very often, that individual is crazy.


  5. #5
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    I am not sure if this is what you mean but this program runs okay on a Haas TL1. Starts at 1000 rpm and then drops down to 800 then 400 and the tool stays on track.

    %
    O00016 (THREADING)
    G20 G40 G80 G99 G61 G97
    G53 G00 X-2. Z-18.
    T202 S1000 M03
    G00 Z2.
    G00 X2. Z1. M23
    X1.77 Z0.2 M08
    G92 X1.74 Z-1. F0.125
    X1.7
    X1.66
    X1.62
    M03 S800
    X1.6
    X1.58
    M03 S400
    X1.56
    X1.54
    X1.52
    G00 X2.
    G00 Z6.
    M30
    %



  6. #6
    Registered jackson's Avatar
    Join Date
    Oct 2006
    Location
    United States
    Posts
    586
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Geof View Post
    I am not sure if this is what you mean but this program runs okay on a Haas TL1. Starts at 1000 rpm and then drops down to 800 then 400 and the tool stays on track.

    %
    O00016 (THREADING)
    G20 G40 G80 G99 G61 G97
    G53 G00 X-2. Z-18.
    T202 S1000 M03
    G00 Z2.
    G00 X2. Z1. M23
    X1.77 Z0.2 M08
    G92 X1.74 Z-1. F0.125
    X1.7
    X1.66
    X1.62
    M03 S800
    X1.6
    X1.58
    M03 S400
    X1.56
    X1.54
    X1.52
    G00 X2.
    G00 Z6.
    M30
    %
    looks like i may have to try this

    individual who perceives a solution and is willing to take command. Very often, that individual is crazy.


  7. #7
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Hogger View Post
    I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.
    Some lathes do allow spindle speed changes via the override knob on the control. But they need to have that option from the factory.
    We do it all the time on J & L 4 axis lathe to find the optimum speed, then edit the program to that.
    Most machine will cross thread if the speed is changed.



  8. #8
    Registered
    Join Date
    Dec 2006
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    Our machines won't let you change the speed with the override, just last Thur. I was making a 6" long 1 15/16-10 LH thread gage for a part we had to make, I was running a center in it and tried to thread it at 600 RPM, guess what... it chattered badly, so I slowed it down in the program to 300 RPM and tried it again, setting the wear offset high so I could see where the tool tip was cutting, I ended up having to use -.025 Z wear offset to get the tool back in the center of the tread.



  9. #9
    Member OldSchoolProgrammer's Avatar
    Join Date
    Nov 2021
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: Why can't threading speeds be changed on CNC lathes?

    Quote Originally Posted by Hogger View Post
    I've always wondered this, I've ran several different CNC lathes in my life and all of them will cross thread if you make a thread and then decide you need to change the speed in the middle of the thread to reduce chatter, or if your running a roughing tool and a finish tool the speed has to be the same for both, you can't run say 500 RPM on the rougher and 800 RPM on the finisher. It seems to me the machine should know where it is at all times and speed wouldn't matter.
    It takes longer for the slides of a machine to accelerate to the programmed IPR feed rate as spindle speed is increased, thus producing a position lag relative to a thread if you make a pass at one speed and increase spindle speed for the next pass. (The inverse is true for a lower spindle speed following a higher spindle speed.) There are ways to program around the problem, but without knowing the exact acceleration rates of the slides for different velocity commands, tedious experiments are necessary for every combination of different spindle speeds.
    As for trying to thread in G96 mode, only some controls are able to keep sufficiently accurate track of spindle speed and respond with a continuously changing feed rate sufficient to maintain correct lead, but even those controls may not be able to track adequately for a very steep taper or a scroll thread.



  10. #10
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3549
    Downloads
    0
    Uploads
    0

    Default Re: Why can't threading speeds be changed on CNC lathes?

    hy oldschool okuma takes into account spindle phase

    - parameter's value doesn't matter, what matters is consistency
    - you can reduce cycle time not by reducing it, but by reducing it's uncertainty


  11. #11
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    2864
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by deadlykitten View Post
    hy oldschool okuma takes into account spindle phase
    OLD thread .... 14 years ago

    And Kitty.... not everyone has Okuma, also Okuma don't like RPM change during cycles



  12. #12
    Member RetiredProg's Avatar
    Join Date
    Nov 2021
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default

    Similar prog worked for me doing acme threads
    on inconel and ferrillium materials on a
    Hass lathe when I was over prog. dept.
    awhile back. Never tried it on a Mori, but
    seems it would do it also.




    Quote Originally Posted by jackson View Post
    looks like i may have to try this




  13. #13
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3549
    Downloads
    0
    Uploads
    0

    Default Re: Why can't threading speeds be changed on CNC lathes?

    Okuma don't like RPM change during cycles
    hy superman

    okuma has variable spindle speed threading spec (vsst), but, like you said, i guess it doesn't like it so it uses a navy function ( T-g ) , to auto-tune its self; it listens for 1 or 2 pases, then targets different rpm for each pass after; it can detect chatter sound, like from long l/d ratio threads, or short ones with big inserts ( like width 4-5 mm, etc ), then take into account what threading pass is being executed, because rpm changing is periodicall, it repeats after a certain number of passes, depending on infeed pattern

    i have seen it in action, but i have never used it / kindly

    Last edited by deadlykitten; 11-28-2021 at 03:18 AM.
    - parameter's value doesn't matter, what matters is consistency
    - you can reduce cycle time not by reducing it, but by reducing it's uncertainty


  14. #14
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3549
    Downloads
    0
    Uploads
    0

    Default Re: Why can't threading speeds be changed on CNC lathes?

    hello again an idea just hit me a few hours ago : i think that is possible to syncronize threading passes at variable rpm on lathes that don't have such an option

    for example use a single pass thread g-code ( fix cycle), not a compound cycle, that targets a small doc, like 0.1, then repeat by increasing rpm, until the 2nd cut overlaps the 1st pass; normal eye should see 0.1mm details, or for higher accuracy, one may use a dial with a sharp palpator, etc

    i have done a similar thing a while ago, not trying to thread at different rpms, but trying to control a custom infeed patern by shifting spindle phase instead of z starting point; i had to do it, because there wasn't enough start-end clearance available

    ratio may be proportional to sqrt(2), thus for example 400 565 800 and 1131rot/min may be fine ? once base ratio is discovered, whatever inbetween scenario can be calculated / kindly

    - parameter's value doesn't matter, what matters is consistency
    - you can reduce cycle time not by reducing it, but by reducing it's uncertainty


  15. #15
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    2864
    Downloads
    0
    Uploads
    0

    Default Re: Why can't threading speeds be changed on CNC lathes?

    Kitty...
    As I stated earlier, this post is 14 years old.
    The OP may not care for any more info, machine may be scrap, who knows. They may not have an Okuma with a P300 control. Or any whiz-bang you-beaut control that may be space age capable.
    Let these old posts die a peaceful death, they served their purpose when created.



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Why can't threading speeds be changed on CNC lathes?

Why can't threading speeds be changed on CNC lathes?

Why can't threading speeds be changed on CNC lathes?