501,916 active members
5,739 visitors online
Register for free
Login
Results 1 to 6 of 6
  1. #1
    Registered
    Join Date
    Apr 2015
    Posts
    22

    Need tapping help

    I'm putting 1/4-28 threads into some 303 stainless fasteners I'm making. Blind hole in parts 1" long, so drilling .950 deep and minimum thread depth is called out at .750 (Why they need a 1/4" fine thread that deep, I don't know - but suspect it wouldn't be necessary if the engineer knew what he was doing...). I made a fixture to hold 10 of these at once for doing some milling on the ends, then drill/chamfer/tap each one.

    Presently, I have an M1 just before the end where the tapping starts. When it gets to this point, I blow the soluble oil/chips out the holes and fill each one to the top with Mobilmet 766 Thread Cutting Oil. Using 2-flute, spiral point, plug chamfer, coated taps (I first tried spiral flute since it's a blind hole, but those began seizing almost immediately at very shallow depth and even when brand new/sharp.). Back to the spiral point 2-flute: Works okay, but I can only program .550 deep (That's including the chamfered end) before seizing might begin. I think the cutting edges just need oil on them again to keep going deeper - which doesn't happen when it just continues to be driven down.

    So, after I've run them to this point, have to fill with oil, hold part in the lathe collet, pickup the thread with the tap (in the tailstock chuck), and power tap down to chips where the tap slips. Retract, blow out chips, and repeat down to the bottom of the hole. This gets me about 1/16" beyond the minimum depth specification (2 revolutions of the 28 pitch thread.) (I have the point of the tap ground off.). Having to finish them this way (640 pieces, manually) is too much trouble/time consuming.

    Two thoughts:
    1) If I have an M1 after tapping each part in the fixture to the .550 depth - to blow out and fill with oil again, can I program to go back in a second time (Two separate times actually, like I presently am manually.) and expect the machine to stay synchronized with the thread it put in previously? And then carry on through each of the ten positions in my fixture that way? By the way - using a 1993 Fadal VMC3016.

    2) I've never done thread milling, but thinking that might be the best solution. Can someone share a sample program for that? Don't know if it would need to be Fadal-specific in any way...

    Thanks!

  2. #2

    Re: Need tapping help

    Try using a #1 (0.228) tap drill and give the spiral flute another try. I use those almost exclusively in 304. Normally I tap 1/4-20, 5/16-18, and 1/2-20, never tapped a 1/4-28 in SS, so don't know how that would go. I ran about 11 hours worth of tapped parts in 304 yesterday with a spiral flute.
    Jim Dawson
    Sandy, Oregon, USA

  3. #3
    Registered
    Join Date
    Feb 2011
    Posts
    244

    Re: Need tapping help

    I would not use the #1 drill (.228) as the minor dia. of the 1/4-28 thread is .211-.220 dia.
    using a 7/32 drill would put it at the top of the minor dia.
    the spiral point plug tap pushes the chip down into the hole so you would have to peck tap it removing the chips at each peck
    you need to have the chip come up out of the hole in order to tap this part with a cutting tap
    you don't say if the tap you used was a high spiral if it was at some point in the tapping cycle it stopped clearing chip and seized- you might try a lower spiral tap
    you don't say if you have rigid tapping if you do you should be able to re tap the thread-- it might put the pitch dia. oversize at the beginning of the thread by re entering the hole a few times ?
    you could try a roll form bottoming tap ( 2-3 imperfect thread lead ) one shot down no chips
    try a 15/64 drill and a good tap cobalt or p.m. (the substrate is important here ) with a good coating like ticn

  4. #4

    Re: Need tapping help

    Quote Originally Posted by rcs60 View Post
    I would not use the #1 drill (.228) as the minor dia. of the 1/4-28 thread is .211-.220 dia.
    using a 7/32 drill would put it at the top of the minor dia.
    the spiral point plug tap pushes the chip down into the hole so you would have to peck tap it removing the chips at each peck
    you need to have the chip come up out of the hole in order to tap this part with a cutting tap
    you don't say if the tap you used was a high spiral if it was at some point in the tapping cycle it stopped clearing chip and seized- you might try a lower spiral tap
    you don't say if you have rigid tapping if you do you should be able to re tap the thread-- it might put the pitch dia. oversize at the beginning of the thread by re entering the hole a few times ?
    you could try a roll form bottoming tap ( 2-3 imperfect thread lead ) one shot down no chips
    try a 15/64 drill and a good tap cobalt or p.m. (the substrate is important here ) with a good coating like ticn
    A #1 drill will give a 50% thread depth, typical in SS for non-critical applications. If there is no call-out for thread geometry and fit, then 50% thread depth is normally OK, especially when going 3xD depth of threads
    Jim Dawson
    Sandy, Oregon, USA

  5. #5
    Registered
    Join Date
    Feb 2011
    Posts
    244

    Re: Need tapping help

    the original poster would have to say whether the thread has a call out for the thread or not
    as he mentions an engineer i would say that even he can not say whether this would be a non critical application as he is not making it for him self
    the machinist hand book recommends .218-.222 for thread length engagements of 1.5-3. x dia.

  6. #6
    Registered
    Join Date
    Apr 2015
    Posts
    22

    Re: Need tapping help

    Thanks for your input, Jim and rcs.

    Yes, I forgot to mention - rigid tapping. As far as oversize holes: yeah, naturally, you can't go as far with a fine thread as with a coarse thread. I'm going to try a #2 at .221. Maybe I'll try the sprial flute again with the larger hole (Was using #3 at .213). It wasn't even a matter of clearing chips - when I'd put the parts in the lathe afterward to tap to the bottom, I couldn't even get a new sprial 3-flute to get down by hand to where the CNC had stopped - SO tight. Once I went to the 2-flute sprial point, I didn't have seizing problems within the first 1/2" like I did with the spiral flute (And a lot less breaking).

    I hadn't heard of "peck tapping" - thanks (I had suggested using an M1 to be able to clear chips and add oil, then down again deeper.). So the machine WILL stay synchronized - good. Looked up peck tapping and I see the code varies a bit with the control - some can use "Q" like drilling, others you have to repeat the X or Y position and then write the next deeper Z increment. And for the Fadal I'm using, yet another couple of formats I don't remember now, off hand.

    The drawing I was given is a crude sketch with the fit noted as class 2. A couple of examples: The 1/4-28 is hand written as ".250-28 UNC-2B" .... well these's a mistake right there, in that it should be "UNF". For another similar part with what I later found out was supposed to be 6-32, the print has written, "138-32 UNC-2B" ??? You can see why I'm questioning the designer's knowledge. My reference to this in my initial post is regarding the fact that more than 1.5 X the diameter doesn't really offer any more holding power.

    I've roll tapped aluminum, but didn't know I could do Stainless. My only concern is the clamping strength of the fixture I made for the CNC milling: Two steel blocks with ten precisely bored holes 1/2 and 1/2 between them to hold these round parts (Some are 7/16" dia., others 3/8": dia.). An 8-32 screw between each position and at the ends to clamp the halves together. It's pretty strong with all eleven screws all tightened down, but still afraid the parts might spin. Don't know- maybe it would be okay.

    I think I'll ask on the Fadal forum here if I can add an M1 to peck tapping to give me more time to add oil to the hole, besides just blowing chips off of a spiral flute or out of the hole for the spiral point tap.

    Thanks again.

Similar Threads

  1. Tapping with Torus Pro and Reversable Tapping Head
    By MRM RCModels in forum Novakon
    Replies: 26
    Last Post: 02-01-2014, 01:47 PM
  2. Replies: 13
    Last Post: 07-04-2009, 12:43 AM
  3. Tapping head or rigid tapping
    By Gregory_C in forum Syil Products
    Replies: 2
    Last Post: 10-18-2008, 06:49 AM
  4. Rigid tapping or tapping head
    By wildcat in forum Charter Oak Automation Support Forum
    Replies: 7
    Last Post: 09-24-2006, 06:08 PM
  5. tapping head vs hand/cordless tapping machine....
    By InspirationTool in forum Uncategorised MetalWorking Machines
    Replies: 6
    Last Post: 09-13-2005, 02:10 AM

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
  •