Single point threading, you can use a single insert for multiple threads?
Close
Login to Your Account
Results 1 to 4 of 4
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    44
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    2

    Default Single point threading, you can use a single insert for multiple threads?

    Trying to learn to single point thread g-code and it looks like it's going to be a bit more difficult. The part has a 4-40 OD thread. I'm being told a 16ER 32UN and maybe it was a 16ER 12UN pitch SP insert could be used. How is this done? I'm uncertain on how to do it even with a 16ER 40UN insert. When it comes to SPT I don't understand how the overall speed of the passes is set. What is the limit of the machine? Is the feed, F0.025" if it was a 4-40 insert? (Is this IPR?... If I'm thinking right) Then it goes off of the rpm I'm running? In both X and Z it can rapid over 900IPM. 2500 RPM X 0.025" = 62.5" Rapid. 73~ SFM so the insert should be fine there, but I don't think I've seen threading faster then 800~rpm on a lathe. Am I heading in the totally wrong direction here? I was being told you could technically thread any thread with any insert, but the top of the threads might be slightly off.

    Thanks,
    Higgins909

  2. #2
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    532
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    186

    Default

    Quote Originally Posted by Higgins909 View Post
    Trying to learn to single point thread g-code and it looks like it's going to be a bit more difficult. The part has a 4-40 OD thread. I'm being told a 16ER 32UN and maybe it was a 16ER 12UN pitch SP insert could be used. How is this done? I'm uncertain on how to do it even with a 16ER 40UN insert. When it comes to SPT I don't understand how the overall speed of the passes is set. What is the limit of the machine? Is the feed, F0.025" if it was a 4-40 insert? (Is this IPR?... If I'm thinking right) Then it goes off of the rpm I'm running? In both X and Z it can rapid over 900IPM. 2500 RPM X 0.025" = 62.5" Rapid. 73~ SFM so the insert should be fine there, but I don't think I've seen threading faster then 800~rpm on a lathe. Am I heading in the totally wrong direction here? I was being told you could technically thread any thread with any insert, but the top of the threads might be slightly off.

    Thanks,
    Higgins909
    as far as rpm I try to stick around 500rpm depending on material and start at .300 to .500 away from z0
    a 4-40 thread is F.025 on a lathe use g97 only NO g96
    Any 60 degree threading insert will almost due any normal 60 degree thread. (watch out of J threads as its a controled root rad.)
    the topping part is for specific thread sizes ie due to the depth of thread but they will work on other threads you can go small but not bigger( in lead).
    I personally never liked them I always liked to cut my own major.but for inconel they work fantastic and pretty happy with them.
    Small threads I wont use topping inserts and I make sure I have the sharpest tip allowable especially for 6's and below. we do thousands of 4-40 o.d. threads and I use a basic 60 degree carbide insert with a sharp tip. I generally have to shave the front side off so not to nick a shoulder.
    Many different ways to make a 60 degree thread, 2 things to remember dont change feed rate ie 1/TPI and RPMS always use g97

    read post 3 and 9
    g76 for dummies

  3. #3
    Join Date
    Oct 2010
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    5,007
    Post Thanks / Like
    Likes (Given)
    4169
    Likes (Received)
    1808

    Default

    Look, you are not going to get satisfactory 40TPI threads from a 12TPI insert! The root radius of the 12TPI insert is practically 100% the size of the full 40TPI space. Imagine you had a perfectly sharp 60 degree tip. To cut good 40TPI threads, you can only remove just the very point of the tip. To cut 12TPI (or 16TPI) threads, you'd truncate and radius much more of the tip.

    Put another way: you can cut coarse threads with an insert sharp enough to cut fine threads, but not the other way around. And if your customer is fussy about the root profile, you might not be allowed to use the fine thread insert for coarse threads, either.

    If you are going to cut 40TPI threads, either use the 16ER 40UN topping insert, or the sufficiently sharp "partial profile" (non-topping) 60 degree insert 16ER A60. (Note: if you're buying Vardex inserts, they are 3ER instead of 16ER.)

    As far as your G code goes, the machine doesn't care what insert you've mounted. Just program a proper thread cycle for the diameter and pitch. You can always start with speeds SLOW so as to be confidently within the machine capability, and increase the speed later once you have the geometry right. You can probably steal a thread cycle from 20 or 50 different CAM textbooks, instructional handouts or G-code recipe cheatsheets.

  4. Likes jancollc, NAST555 liked this post
  5. #4
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,605
    Post Thanks / Like
    Likes (Given)
    1179
    Likes (Received)
    664

    Default

    I used to predominantly use open form inserts but have moved away from them as form inserts for the correct pitch sure do work well. Getting the form correct helps a lot, just make sure that the tool is square to the part. I generally cut it 0.1mm oversize on the OD and let the insert clean it up to size.

    I like what others said about on speeds and so on, start SLOW, if it is a one or even 2off part it sure sucks having chatter and having to put it in the manual to clean it up. I much rather prefer to let it take a bit longer than sitting with threads that look terrible.

    sfriedberg put the Vardex name out there... I used to only use Iscar threading inserts but after using Vardex or Mitsubishi I won't go back. Their general chip "breaker" is terrible compared to Vardex/Mits. And on a small side note... Apparently Widia get their threading holders/inserts from Vargus. Not sure how true that is but I got a bit of inside information. A bit of "scratch my back and I will scratch yours" situation.


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
  •