Please kick-start my first attempt at rigid tapping.
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    383
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    53

    Default Please kick-start my first attempt at rigid tapping.

    So, I have a new mill with rigid tapping, (Fanuc OiMF control) and a job to do. The job is to drill and tap the end of a number of 0.375 aluminum rods with a 6-32 thread to a depth of 0.375 inch to accept a screw to secure a knob. The flats for the knob are cut in another process because they must be aligned to other features.

    I would appreciate advice to make a fast start on the project and reduce my learning time. I am happy with the coding side of things but I need practical advice.

    I have built a jig so that two rods at a time can be mounted in a vise. The first process will be to mill the rods to consistent heights which will provide my Z surface. Obviously the next jobs will be to drill and tap which is where my learning curve steepens,

    Questions.
    The working thread in the rod needs to be 0.375 deep. How deep should I drill to allow bottom clearance for the tap yet still providing a true 0.375 depth of thread? (This will, I imagine depend on the tap).
    Which specific type of tap should I use for this job bearing in mind I am tapping into a blind hole? I do not see that I could do the usual hand "taper followed by plug" so how will this effect the tapping depth and hole depth? I suppose I could machine taper tap followed by hand plug tap if I had to.
    Should I chip break or peck with a 6-32 tap?

    Thanks for any info. you can provide. I am really looking forward to using this new capability.

    Brian

  2. #2
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,064
    Post Thanks / Like
    Likes (Given)
    638
    Likes (Received)
    1026

    Default

    Given that your hole specs don’t seem that tight, drill as deep as you need to, tap as deep as you need without bottoming out. I’d use a roll tap.

  3. Likes aj liked this post
  4. #3
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,185
    Post Thanks / Like
    Likes (Given)
    721
    Likes (Received)
    1766

    Default

    I'd be using a bright finish spiral flute bottoming tap. Drill, chamfer, tap, repeat.

  5. #4
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,242
    Post Thanks / Like
    Likes (Given)
    1820
    Likes (Received)
    800

    Default

    6/32 is about the absolute WORST to cut tap. In any material.
    The taps (no matter what mfgr) are weak, and will snap....

    I STRONGLY recommend a thread forming tap, rather than a cutting tap.
    Any plug style will get you the simple 3/8" thread depth, just drill a little deeper than required to tap.
    IIRC a Ø.125" hole is the perfect size for thread forming a 6/32.

    I would use a 90° spot drill to chamfer to Ø.15",a parabolic flute 1/8" drill to depth, followed up by the forming tap.
    Standard, to slightly high ratios are okay, when using soluble oil coolant and thread forming.

    Just my $.02

    Doug.

  6. Likes thesidetalker, aj, yardbird, eaglemike liked this post
  7. #5
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    553
    Post Thanks / Like
    Likes (Given)
    39
    Likes (Received)
    190

    Default

    personally I wouldnt use a vise to locate 3/8 round stock unless they were very short pcs.

    I would use a collet, or a 2 3 or 4 multi collet block. due to rigidity and repeatability not to mention speed
    for lots of parts I have a few 3 5c collet blocks, and my cycle time from doing 1 part to 9 parts isnt much different maybe 2 mins tops. because your tool change is what eats up your cycle time.

    Locate as close to the top of part as possible.
    face 1/2" endmill
    center drill ( I only use keo style center drills I dont use spot drills cause they suck but hey thats me)
    drill
    tap
    chamfer ( in my case I do this extra operation last but no need to if you dont want too).

    spiral bottoming taps work best for cut tapping, roll taps are great also.
    you may need to check with your customer on the type of thread Ie cut or rolled some customers have a preference or requirement.not to mention how deep you can go on the drill depth and chamfer size along with what angle for the chamfer.

    if the chamfer is not specified I like a 120º gives a cleaner thread on the front end, doesnt give you a burr either.

    .375 tap drill depth is not called out .600 works great., if you have specs then pay attention to them,including the minor size which will grow in cut taping.

    no need to peck tap either one shot deal.

    6-32 cut taps work perfectly fine all day long very rarely have any taps break. and we do thousands of 0-80 2-56 and 4-40 threads.

    we do cut to length drill and tap often in both round a square, rectangle parts

  8. #6
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    383
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    53

    Smile

    Quote Originally Posted by Delw View Post
    personally I wouldnt use a vise to locate 3/8 round stock unless they were very short pcs.

    I would use a collet, or a 2 3 or 4 multi collet block. due to rigidity and repeatability not to mention speed
    for lots of parts I have a few 3 5c collet blocks, and my cycle time from doing 1 part to 9 parts isnt much different maybe 2 mins tops. because your tool change is what eats up your cycle time.

    Locate as close to the top of part as possible.
    face 1/2" endmill
    center drill ( I only use keo style center drills I dont use spot drills cause they suck but hey thats me)
    drill
    tap
    chamfer ( in my case I do this extra operation last but no need to if you dont want too).

    spiral bottoming taps work best for cut tapping, roll taps are great also.
    you may need to check with your customer on the type of thread Ie cut or rolled some customers have a preference or requirement.not to mention how deep you can go on the drill depth and chamfer size along with what angle for the chamfer.

    if the chamfer is not specified I like a 120º gives a cleaner thread on the front end, doesnt give you a burr either.

    .375 tap drill depth is not called out .600 works great., if you have specs then pay attention to them,including the minor size which will grow in cut taping.

    no need to peck tap either one shot deal.

    6-32 cut taps work perfectly fine all day long very rarely have any taps break. and we do thousands of 0-80 2-56 and 4-40 threads.

    we do cut to length drill and tap often in both round a square, rectangle parts




    Thanks for the suggestions guys. All valuable and I will work through them to find the best fit for my mill. DELW, I was not clear on my use of the vise. I actually made a pair of floating jaws that locate and clamp into my vise. These jaws are drilled and reamed to take the rod vertically and hold it firmly.

    There is a groove around the rod but I still have plenty of room to drill to the suggested 0.6 depth. I need to order some of the taps suggested - you can't have too many taps.

    This is not a commercial project, I use the machines to support my real business so thankfully I am under no pressure to produce in a hurry which gives me a chance to do things right.

    Brian

  9. #7
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    657
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    711

    Default

    I didn't read everything so sorry if repetitive.

    Drill .625 deep using a 3.2mm Guhring 2 Flute stub drill. 6000 RPM and 18 IPM, one shot no pecks.

    Tap with a 6-32 Roll Tap .450 Inches deep at 1000 RPM, 31.25 IPM.

    Feeds and speeds are conservative to accommodate most machines. I double them on my quicker machines. I'm guessing I run these specs ~10k per year, haven't found a need to change.

  10. #8
    Join Date
    Nov 2011
    Location
    Maryland, USA
    Posts
    234
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    21

    Default

    I'd also recommend a forming tap. Guhring makes great ones!!!

    Sent from my Pixel 2 using Tapatalk

  11. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,442
    Post Thanks / Like
    Likes (Given)
    1483
    Likes (Received)
    1626

    Default

    Quote Originally Posted by G00 Proto View Post
    I didn't read everything so sorry if repetitive.

    Drill .625 deep using a 3.2mm Guhring 2 Flute stub drill. 6000 RPM and 18 IPM, one shot no pecks.

    Tap with a 6-32 Roll Tap .450 Inches deep at 1000 RPM, 31.25 IPM.

    Feeds and speeds are conservative to accommodate most machines. I double them on my quicker machines. I'm guessing I run these specs ~10k per year, haven't found a need to change.
    Nothing wrong with drilling a little extra deep, but it is not needed for a form tap.

    We tap 4-40 and 2-56 all day every day in 6061 alum. The 4-40 tap drill (.0995") I drill .03" deeper than the tap, and the 2-56 tap drill (.0781") I drill .025" deeper than the tap. Your point, for 118deg is roughly .3xdia so for a 6-32 tap drill (.125") you would need to drill about .49" deep to tap to .45" deep.

    This all assuming form/roll taps and rigid tapping in a solid (not compression/ext) holder like a collet.

    edit: wanted to add this is for our own product so we don't have to meet any thread specs, if you are doing aerospace or gubmint, sometimes you can't use a form tap and need to cut tap to meet specs

  12. #10
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    657
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    711

    Default

    Quote Originally Posted by Mike1974 View Post
    Nothing wrong with drilling a little extra deep, but it is not needed for a form tap.

    We tap 4-40 and 2-56 all day every day in 6061 alum. The 4-40 tap drill (.0995") I drill .03" deeper than the tap, and the 2-56 tap drill (.0781") I drill .025" deeper than the tap. Your point, for 118deg is roughly .3xdia so for a 6-32 tap drill (.125") you would need to drill about .49" deep to tap to .45" deep.

    This all assuming form/roll taps and rigid tapping in a solid (not compression/ext) holder like a collet.

    edit: wanted to add this is for our own product so we don't have to meet any thread specs, if you are doing aerospace or gubmint, sometimes you can't use a form tap and need to cut tap to meet specs
    You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

    Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.

  13. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,442
    Post Thanks / Like
    Likes (Given)
    1483
    Likes (Received)
    1626

    Default

    Quote Originally Posted by G00 Proto View Post
    You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

    Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.
    LoL not brave, just a necessity for us. If you inspect a form tap (modified bottoming) the first 2-3 threads or so are tapered, almost like wood screw but not to a sharp point. This gives you a tad extra clearance at the bottom of the hole.

  14. Likes G00 Proto liked this post
  15. #12
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,442
    Post Thanks / Like
    Likes (Given)
    1483
    Likes (Received)
    1626

    Default

    Quote Originally Posted by G00 Proto View Post
    You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

    Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.
    Yes good point. We actually do some parts with holes near edge (not at work so not sure how close) that actually bulge the mat'l out a few tenths. We have to run the endmill back around them after they are tapped to hit our tolerance.


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
  •