Rigid taping rpm - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 49
  1. #21
    Join Date
    Apr 2009
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,555
    Post Thanks / Like
    Likes (Given)
    534
    Likes (Received)
    486

    Default

    Quote Originally Posted by Heinz R. Putz View Post
    Wow, what a variety of figuring the speed for tapping.
    This is because he was asking about how many decimals his machine can handle. The rest of your post (my opinion anyway) is making everyone else at PM sound as if they are all new apprentices. I'm sure the OP already knows about the basic rpm formula. Besides he wasn't even asking about speeds to begin with. I'm sure he also knows that the speed varies on different material, again not what hes asking. Not to sound like an ass, but your response was pretty much "useless" as it didn't touch any of the questions he asked except for that his machine will accept more than 2 decimal places.

  2. #22
    Join Date
    Sep 2002
    Location
    Lawrenceville GA USA
    Posts
    6,268
    Post Thanks / Like
    Likes (Given)
    846
    Likes (Received)
    1370

    Default

    My thanks to all of you who posted responses, the variety of ideas is just what I was hoping to see. There is no black art to what we do and there is no one only best way to do anything. We all learn by working with others and from our shared experiances. I value the opinion of everyone who posted and thank you all again.

    Charles

  3. Likes Mtndew liked this post
  4. #23
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Hi, I've been following this thread now, and dont have any experience with programming a tapping cycle, but today I was working on a job in stainless steel where we are tapping each end, one end 3/8-16 and the other 1/4-20. The 3/8-16 worked fine, but the 1/4-20 taps kept breaking left and right. The 3/8-16 was programmed for 75 RPM, and the 1/4-20, 50 RPM (G97). Reading this thread these sound really low. Could these RPMs contribute to breaking taps? For reference, I am tapping on old Hitachi Seikis, TS15.

    Edit: Actually on the trouble tap, it is in a floating holder, the other is in a rigid holder.

  5. #24
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,820
    Post Thanks / Like
    Likes (Given)
    4420
    Likes (Received)
    2915

    Default

    Quote Originally Posted by UncleDaddySwiss View Post
    Hi, I've been following this thread now, and dont have any experience with programming a tapping cycle, but today I was working on a job in stainless steel where we are tapping each end, one end 3/8-16 and the other 1/4-20. The 3/8-16 worked fine, but the 1/4-20 taps kept breaking left and right. The 3/8-16 was programmed for 75 RPM, and the 1/4-20, 50 RPM (G97). Reading this thread these sound really low. Could these RPMs contribute to breaking taps? For reference, I am tapping on old Hitachi Seikis, TS15.

    Edit: Actually on the trouble tap, it is in a floating holder, the other is in a rigid holder.
    What kind of stainless?What kind of tap? Uncoated? Plug? We need more info to give you a better answer.
    For instance, if you're using a Guhring spiral flute tap made for stainless, you would be going approximately 450rpm give or take.

  6. #25
    Join Date
    Mar 2011
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    90
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    23

    Default

    Quote Originally Posted by 706jim View Post
    It's hard to say just what the real limits would be for your machine. Let us know what model it is and someone may here may have the answer. We just received two new Haas machines and I got to see rigid tapping firsthand today.
    Backing out of the hole at 4X the rpm going in was one of the first surprises that I had.
    How do you back out faster on a haas? I have a 2013 VF4-SS and using Mastercam X8 if that is any importance...

  7. #26
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,270
    Post Thanks / Like
    Likes (Given)
    1865
    Likes (Received)
    812

    Default

    Newer Haas machines have a setting, where it can, if enabled, retract at 2, 3, or 4X the infeed RPM.
    I believe the setting # 130, but it should be a quick search of settings.

    Doug.

  8. #27
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,497
    Post Thanks / Like
    Likes (Given)
    3467
    Likes (Received)
    2057

    Default

    The Haas will let you set that retract at up to 9x tapping speed, but be careful you don't exceed the machine's max feedrate or max spindle rpm that way. I have our VF-6SS set to 4x.

  9. #28
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    California
    Posts
    844
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    207

    Default

    Quadman,

    I believe they (haas) come from the factory to reverse out at 3-4x the programmed speed...but a J# (J1-J9) can make the reverse speed from 1-9 times. It is the usual G84 cycle but you just add the J# if you want it different from factory (no J in the cycle defaults to the factory setting).

    Have you ever watched the speed when yours reverses? You can probably have Mastercam spit out the J# but like I said, the factory already does 3-4X and for me that rarely needs to be different.

  10. #29
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Well, I'll be honest here, i work in a production shop where there are layouts, and we are just supposed to follow them, so I'm not real good with materials quite yet. Our company assigns their own numbers to the materials, but out of my own curiosity this morning i did read the material description, and "1018" was in it. We used a flat bottom spiral tap, but don't know the specifics. I'm in the process of teaching myself some of these things, the attitude of our shop is "just read the layout, " but that really hasn't worked too great for us. I just wondered if RPMs that low on harder material would cause taps to break. Thanks.

  11. #30
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    A) 1018 is not SS
    B) 1018 is not hard - it is actually very soft - making it gummy/stringy.

    It sounds like the tap that you have should work fine at about any speed in that material.

    Looks like we would need more specifics of your program/set-up.

    What drill are you using?

    What Z depth for both the drill and the tap?

    No clue why you slowed the RPM down for the smaller tap? If 75 works for 3/8, it would seem like you would jump to 100 for the 1/4" eh?

    Personally I would be in the 400 RPM range - depending on chuck size.
    A big chuck will take more Decel time, thus making bottom out a bigger issue - independent of your programmed Z depth.


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

    Think Snow Eh!
    Ox

  12. #31
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Ok, I did say that I don't know much about material at this point. And, I didn't slow anything down. We have a department programmer, and this is how he programmed it. I am actually doubting the way he did it and am thinking I should speed it up. I am trying to verify that here. I dont remember what the drill was off the top of my head, but it was drilled to .810, and tapped to .630. The machine doesn't have a chuck per se, it is a spindle that only takes #3 collet pads.

  13. #32
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I always calculate the sfm of the tap based on the material I'm tapping.
    When the tap is meant for the metal:
    Stainless- 30 sfm
    Alloy steels- 50 sfm
    Mild steel- 80 sfm
    Aluminum- 120 sfm

    When I'm getting by with, say, tin coated taps in aluminum or bright finish taps in steel, I adjust the sfm downward accordingly. Coarse threads also need to be slowed down a little because more material gets pushed around and thus more heat.
    Hope this helps.

  14. #33
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Thank you, yes it does.

  15. #34
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    Quote Originally Posted by UncleDaddySwiss View Post
    Ok, I did say that I don't know much about material at this point. And, I didn't slow anything down. We have a department programmer, and this is how he programmed it. I am actually doubting the way he did it and am thinking I should speed it up. I am trying to verify that here. I dont remember what the drill was off the top of my head, but it was drilled to .810, and tapped to .630. The machine doesn't have a chuck per se, it is a spindle that only takes #3 collet pads.

    Wait - WHAT?


    .810?
    .630?

    I thought that we were talking 1/4 & 3/8?


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

    Think Snow Eh!
    Ox

  16. #35
    Join Date
    Sep 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    625
    Post Thanks / Like
    Likes (Given)
    453
    Likes (Received)
    211

    Default

    I think those were the deeps (drill & tap) that you asked for above OX.

  17. #36
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,547
    Post Thanks / Like
    Likes (Given)
    5788
    Likes (Received)
    8173

    Default

    LOL!

    OK - got it!


    This 1/4" tap was a spiral flute tap right? Not a spiral point?

    At your RPM there shouldn't be any bottoming from slow decel I wouldn't think - depending on the program anyhow...

    I like the OSG and similar "Modified Bottom Spiral Flute Taps". I think the basic "spiral flute taps" are OK for alum maybe, but I don't like them for 1018.

    I don't use form taps near as much as I did 15 yrs ago, but 1/4" -20 in 1018 is a real good app.
    Gotta change to a #1 (?) drill tho. (or is it "A"?)



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

    Think Snow Eh!
    Ox

  18. #37
    Join Date
    Aug 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    2

    Default

    Hello All,
    I need Help

    I am using a GT75 controller and second opt threading 1/4-20 some slugs of 3/4" bar stock 1/2" deep
    I am through tapping them with a spiral point tap.
    I need some help with my program
    Thanks in advance

    G00G90G94F300S250
    T1 (1/4-20 Tap)
    G00X0Z3
    G00Z.020
    G95F.040Z-.975
    M04
    G04F.5
    G95F.046Z.050 (.044)
    M09
    G00Z3
    G00X-6.5
    M13
    M30

  19. #38
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,766
    Post Thanks / Like
    Likes (Given)
    489
    Likes (Received)
    1963

    Default

    Well, you might start by putting F.050 in your G95 lines so your feedrate matches the tap's pitch.

    General practice to start the tapping cycle farther then .020" from the part, so your spindle has time to come up to RPM. You are already at 300RPM, so this might not make any difference- but on rigid tapping cycles the spindle usually is stopped at the beginning of the cycle...

  20. #39
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    8,116
    Post Thanks / Like
    Likes (Given)
    415
    Likes (Received)
    6699

    Default

    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

  21. #40
    Join Date
    Aug 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    2

    Default

    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?


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
  •