Results 1 to 9 of 9

Thread: Tapping problem!

  1. #1
    Join Date
    Feb 2009
    Posts
    11
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Tapping problem!

    I am having trouble tapping a 10-32/.500 deep in 316 stainless,my rpm is 300 with a feed of 9.375 with a three flute tap. Any advice!!

    Thanks,
    Mike

  2. #2
    Join Date
    Nov 2006
    Location
    Lewisville(New Castle Area), Indiana
    Posts
    233
    Thanks
    0
    Thanked 14 Times in 12 Posts

    Default

    Your feedrate is correct for your spindle speed. What's happening when you try to tap?

    I'm assuming this is on your Haas machine?

    One thing I always do is change to feed per revolution when I'm tapping so that if I have to play with my spindle speed I never have to worry about my feedrate.

    Also, there's a setting on the control to allow you to re-tap the same hole. I use it quite a bit on aluminum if I have tap fairly deep.

    G00 X0. Y0.;
    G95 M03 S300;
    Z.1;
    G99 G84 Z-.1 F.03125 R.1;
    X0. Y0. Z-.2;
    X0. Y0. Z-.3;
    G80;
    G94;
    Cody Stamper



    (Note: The opinions expressed in this post are my own and are not necessarily those of cnc-professional-forum.com and its management)

  3. #3
    Join Date
    Feb 2009
    Posts
    11
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Cody

    Hi,breaking alot of taps,I just change the rpm to 150 and it seems to be working better! Only tapping about .55 deep!

  4. #4
    Join Date
    Aug 2008
    Location
    huber heights, ohio
    Posts
    179
    Thanks
    2
    Thanked 12 Times in 12 Posts

    Default

    have you checked to ensure your spindle is turning at the correct programmed speed we had a machine that kept breaking taps we found the belt on the spindle drive worn out causing incorrect rpm's changed out the belt machine taps great now.

  5. #5
    Join Date
    Feb 2009
    Posts
    11
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default

    The spindle is ok,I just talk to the Guhring(10-32 spiral 3 flute) about the tap I purchase from them,they said I should use sf of 25 ,that would make the rpm around 500,that seems way to fast,what do you guys think?

    Mike

  6. #6
    Join Date
    Nov 2006
    Location
    Lewisville(New Castle Area), Indiana
    Posts
    233
    Thanks
    0
    Thanked 14 Times in 12 Posts

    Default Spindle Speed

    500 doesn't sound awful really. I'd give it a try and see how it works. I've had tooling reps give me numbers that made me laugh in their face, and try to prove them wrong, but most of the time they win.

    They've made me a little less conservative on my numbers. For instance:

    I had to make a plate that had 50 1/4-20(TIN Coated HSS) holes .5 deep last week, and I tapped those at 750RPM. I'm not sure what grade it was, just free machining CRS. And today I tapped a 5/8-18(Uncoated 3 flute HSS) hole 2.4 deep @ 1000 RPM .6 peck in H13 on a Haas TM-1.
    Cody Stamper



    (Note: The opinions expressed in this post are my own and are not necessarily those of cnc-professional-forum.com and its management)

  7. #7
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default

    I would thread mill it as long as it is cost effective. 316 or any SS for that matter is pretty rough on taps. I am a bit bias as I have always threadmilled. It was never cost or time effective for us to tap. Anyway that’s not to say that it can’t be done. When we started outsourcing some of our larger work they were tapping it. They were nice enough to give us some info on what they were using for tooling as when we tried we could not get anything to hold up. I however left that outfit before we got that program in full swing.

    They were using YMW Stainless Ground Spiral Semi Bottoming taps from KM Tool. They say they also used Greenfield taps. These taps were specific for SS.

    That's my .02

    Stevo

  8. #8
    Join Date
    Feb 2009
    Posts
    11
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Stevo?

    Hi,how well will the threadmill hold up,I have about 500 plus holes to tap?Who do you buy your threadmills from?

    Thanks,
    Michael

  9. #9
    Join Date
    May 2008
    Location
    Great State of Wisconsin
    Posts
    1,211
    Thanks
    7
    Thanked 134 Times in 112 Posts

    Default

    I use “scientific cutting tools” thread mills through MSC. The problem is going to be your hole size and the depth of cut. That is a small hole so the smaller you go with the threadmill the less the length is offered in. I don’t think that Scientific offers that range of .5 deep. You could try Emuge but they are going to be more expensive.

    How many holes will you get??? Sorry I can’t answer that for you. The smallest that I have thread milled is 1/4-28. We could get anywhere from 30-300 holes depending on how we set our pick and how fast we wanted to get through the part. I have a very good thread mill macro that I wrote that you can adjust the pick to were you need it. Your other option is to use a single profile tool to create your threads. This will eliminate trying to find a thread mill that will go that deep. These processes will take time so it might not be cost effective for you to do. The thread mills will probably run you anywhere from $150-200 each and the single profile around $50 link below.

    MSC Item Detail

    A lot of people say thread milling is not the way to go and not cost effective. Sometimes there right…however I was told that it will never work thread milling 1/4-28’s now we run them all day long in high nickel alloys and SS. So you will never know until you try. Sorry I couldn’t give you experience advice but your running hole sizes I have not tried with a thread mill "yet".

    Stevo

Similar Threads

  1. Makino seiki tapping problem
    By venuengg in forum Machine Repair & Troubleshooting
    Replies: 0
    Last Post: 09-22-18, 12:46 AM
  2. Problem during tapping process
    By angelito in forum Machine Repair & Troubleshooting
    Replies: 6
    Last Post: 02-13-12, 03:12 PM
  3. Tapping Problem
    By Grinder in forum General CNC & Manufacturing Discussion
    Replies: 6
    Last Post: 12-13-09, 06:56 PM
  4. FADAL rigid tapping problem
    By andatek in forum Machine Repair & Troubleshooting
    Replies: 6
    Last Post: 01-16-08, 05:57 PM

Posting Permissions

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