Rigid taping rpm - Page 3
Close
Login to Your Account
Page 3 of 3 FirstFirst 123
Results 41 to 49 of 49
  1. #41
    Join Date
    Aug 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    2

    Default

    wow Bob you lost me

  2. Likes CarbideBob liked this post
  3. #42
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,766
    Post Thanks / Like
    Likes (Given)
    489
    Likes (Received)
    1963

    Default

    Quote Originally Posted by CNCbeginer View Post
    Thanks Jancollc,
    I should have mentioned that i am using a floating tap holder, My speed is at 250rpm

    If i change my speed will the program still be ok?
    I assumed you had a floating holder by your feedrates. Yes, you can change the RPM in the program.

    The tension/extension holders vary. Some release, some don't. Releasing holders are designed that way to control the depth- not a factor on your thru holes.

    It's not uncommon to program a slightly higher or lower feedrate going in, depending on how long your spindle takes to reverse. I have never seen someone program a lower feedrate both going in and coming back out- this would mean the holder is extending both directions, and you risk busting the tap or tearing out the threads.

    I start with my tap pitch going in and coming out, and I watch the holder to make sure I am not getting to the travel limit of the holder. If I am extending too much on the way in, I'll increase the feed a bit, etc. I like to see a little bit of compression on the way in, and extension at the spindle reverse and feed out.

    Watch your RPM increases, as this will affect the time it takes the chuck to stop and reverse. That in turn will affect how much travel you are using on the holder.

  4. Likes CNCbeginer liked this post
  5. #43
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    I typically feed in slightly under - with a hard start.
    If my holder doesn't have a hard start, it will by the time I walk away.
    Compression is a very big cause of junk parts!

    Feed in slightly under rate, and maybe feed back out at rate, or even slightly under - depending on reversal time.

    Main spindle on a lathe - prolly want to feed under.
    Sub-spindle or GT27 type machine - prolly feed at rate.

    If you are under feeding on the way in - you already have some cush, and then when you hit that Z+/G4 line, you will get some more yet.
    Over feed on the way out and you will be trying to pull the first thread on the way out.


    -------------------

    Think Snow Eh!
    Ox

  6. Likes CNCbeginer liked this post
  7. #44
    Join Date
    Aug 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    2

    Default

    Quote Originally Posted by jancollc View Post
    I assumed you had a floating holder by your feedrates. Yes, you can change the RPM in the program.

    The tension/extension holders vary. Some release, some don't. Releasing holders are designed that way to control the depth- not a factor on your thru holes.

    It's not uncommon to program a slightly higher or lower feedrate going in, depending on how long your spindle takes to reverse. I have never seen someone program a lower feedrate both going in and coming back out- this would mean the holder is extending both directions, and you risk busting the tap or tearing out the threads.

    I start with my tap pitch going in and coming out, and I watch the holder to make sure I am not getting to the travel limit of the holder. If I am extending too much on the way in, I'll increase the feed a bit, etc. I like to see a little bit of compression on the way in, and extension at the spindle reverse and feed out.

    Watch your RPM increases, as this will affect the time it takes the chuck to stop and reverse. That in turn will affect how much travel you are using on the holder.
    Thank You for the explanation, I have a better understanding of what i'm doing now
    Thank you for thatI'll adjust the feed a bit to get it close to .050

  8. #45
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    8,116
    Post Thanks / Like
    Likes (Given)
    415
    Likes (Received)
    6699

    Default

    Quote Originally Posted by CNCbeginer View Post
    Thanks Jancollc,
    I should have mentioned that i am using a floating tap holder, My speed is at 250rpm

    If i change my speed will the program still be ok?
    With a floating tap holder you push the advance per rev higher than than the thread on purpose.
    You want to "push" it but not run out of travel in the float or spring.
    It will not start like a rigid so it will lag
    You do not want to hit solid on the bottom but well in on compression is good.
    If you program at rigid tap feed likely it will not work well.
    In such you want to use some of the spring built in and it should for sure compress during the process.
    Bob

  9. #46
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,721
    Post Thanks / Like
    Likes (Given)
    855
    Likes (Received)
    2560

    Default

    Quote Originally Posted by CNCbeginer View Post
    ..I should have mentioned that i am using a floating tap holder, ....
    Since you are using a floating holder, why post in a thread about rigid tapping????

    Your code doesn't look like any rigid tap code I have seen either.

    Maybe start a new thread?

  10. #47
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,241
    Post Thanks / Like
    Likes (Given)
    4758
    Likes (Received)
    1635

    Default

    Quote Originally Posted by CarbideBob View Post
    I modify the spindle speed to an even feedrate or at most 1 decimal out and modify spindle speed.

    We work in base 10, computers work in base 2, some numbers on the right of the decimal point don't convert well between the two worlds. That is confusing.
    Internally it is likely your control is doing all the math in encoder counts so rounding and if you have inch or metric screws comes into play on that conversion.
    In most use you only are off by one or two counts and no servo is that accurate so it is never a seen problem. There are some numbers worse than others.
    0.1 + 0.2 does not equal 0.3 in a computer.
    https://0.30000000000000004.com/
    Fanuc used to do BCD math inside which is somewhat different, I do not know if the new ones still do.
    Encoder count rounding, servo lag and tracking kill most of this by miles.

    Anywho, the error is small and your spindle and axis can't track within it anyways so those extra decimals on your feed make you feel good but are not going to happen
    A 20 inch long or deep thread and then the errors may stack up to some oh-shit.
    A metric screw machine tool at one micron resolution has a problem with .0001 inch moves. There is a skip or jump and no way around it.

    How close is the spindle speed to real and how tight the loop to the feed axis. Rigid tap usually ties one to the other in a master/slave on the numbers you supplied.
    Resolution on the spindle may matter.

    I just like staying out of decimal points as I know any control can handle that so I just move the RPM this or that ways.
    Bob
    Bob I've never seen anyone explain it like this. If I understand it correctly then you've convinced me. Have you noticed any improvements doing it this way? Longer tap life, better threads? Weather you have or you haven't I can't see it hurting anything going this route. Time be the only thing. If you rounded down on the RPM that is.

    Brent

  11. #48
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,061
    Post Thanks / Like
    Likes (Given)
    1611
    Likes (Received)
    1889

    Default

    All I can say is I'm glad I haven't needed to use a floating tap holder in forever!


  12. #49
    Join Date
    Sep 2002
    Location
    Lawrenceville GA USA
    Posts
    6,268
    Post Thanks / Like
    Likes (Given)
    846
    Likes (Received)
    1370

    Default

    Kind of neat seeing a thread of mine that I started 10 years ago. First CNC mill that I worked on that supported rigid tapping. Still using some of the advice given here today.

    Charles


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
  •