Page 1 of 2 12 LastLast
Results 1 to 12 of 14

Thread: Thread Milling 3/8-18 NPT

  1. #1
    Registered
    Join Date
    Jul 2005
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Question Thread Milling 3/8-18 NPT

    Does anyone have an incremental program for a 3/8-18 NPT using a multi tooth threading tool. The diameter of my tool is .371". I am using a Tool Flo tool.

    Similar Threads:
    Last edited by shawn; 08-25-2006 at 12:45 PM.


  2. #2
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    Try this...BE CARFUL! this is for a .31 dia. thrd mill but should work if you add .035" to cutter comp offset #1 (D1)

    %
    O151
    (NO TOOL RADIUS COMPENSATION D1=0)
    (ADJ. D1 PLUS .035 AND WORK TO SIZE)
    N1 T1 M6
    G90 G0 G54 G17 X0.0000 Y0.0000 S???? M03
    G43 H1 Z1.
    Z0
    G01 G91 Z-0.4149 F200. M08
    G01 G41 D1 X0.0839 Y-0.0839 F??
    G03 X0.0839 Y0.0839 Z0.0069 I0.00000 J0.08390 F??
    G03 X-0.1678 Y0.1682 Z0.0139 I-0.16823 J0.00000
    G03 X-0.1687 Y-0.1682 Z0.0139 I0.00000 J-0.16866
    G03 X0.1687 Y-0.1691 Z0.0139 I0.16909 J0.00000
    G03 X0.1695 Y0.1691 Z0.0139 I0.00000 J0.16953
    G03 X-0.0848 Y0.0848 Z0.0069 I-0.08476 J0.00000
    G01 G40 X-0.0848 Y-0.0848 F200.
    G01 Z0.5417
    X0.0000 Y0.0000 Z1.
    M30
    %



  3. #3
    Registered
    Join Date
    Jul 2005
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    Thank you very much worked perfect. I ended up at .021 in the offset but it worked great. My only question would be the depth? .4149 seems kind of Shallow. I run my 1/4-18 NPT@ z-.522? Since the program is incremental could I drop the Z lower and just increase my D offset to compensate?



  4. #4
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    Yes, by all means , if you need more thrds. do exactly that. BTW, that came from a cd-rom I got from my Iscar rep. if you have one in your area he/she should be able to set you up with one. Its "geared" for there product line but, I've found it works well for others as well



  5. #5
    Registered
    Join Date
    Jul 2005
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    Oh ok. Thanks again. We dont deal much with them but I will give it a shot.



  6. #6
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    One other thing, the cutting length of your tool would be the determining factor as to how deep you can thrd. mill. I have a prog. for a 1-11.5 NPT that cuts the hole with a .625 dia bull nose e.m. using virtual axis interpolation to put a chamfer on the tappered hole before thrd. milling it. Note speed and feed on the bull mill it has cut at least 350 holes and shows no signs of wear!

    M1
    M6
    G90 B90000 M42
    T76 S5000 M3
    (TOOL-94 = .625 BULL MULTI MASTER)
    (B90 DEG/ G54)
    G0 G90 G17 G95 G54 X-2.75 Y-3.5
    Z1. M8
    Z.1
    G91 G1 G95 F.02 Y.5488
    G3.1 X0 Y-.2713 J-.5488 Z-.3 P10
    G3.1 X0 Y-.0375 J-.2775 Z-.65 P18
    G3 J-.2485
    G1 Y-.2485
    G90 G0 Z1.
    X-4.75 Y0
    Z.1
    G91 G1 G95 Y.5488
    G3.1 X0 Y-.2713 J-.5488 Z-.3 P10
    G3.1 X0 Y-.0375 J-.2775 Z-1. P18
    G3 J-.24
    G1 Y-.24
    G90 G0 Z1.
    G91 G30 Z0
    G30 X0 Y0
    M1
    (TOOL-95 = ISCAR THRD MILL .625 DIA./.08696 PITCH)
    M6
    G90 G0 G54 X-2.75 Y-3.5 Z1.9685 S3033 M03
    Z1. M8
    Z0
    G01 G91 Z-0.7339 F196.8 M08
    G91 G94 G01 G41 D1 X0.3067 Y-0.3067 F56.5
    G03 X0.3067 Y0.3067 Z0.0109 I0.00000 J0.30674 F38
    G03 X-0.6135 Y0.6142 Z0.0217 I-0.61417 J0.00000
    G03 X-0.6148 Y-0.6142 Z0.0217 I0.00000 J-0.61484
    G03 X0.6148 Y-0.6155 Z0.0217 I0.61552 J0.00000
    G03 X0.6162 Y0.6155 Z0.0217 I0.00000 J0.61620
    G03 X-0.3081 Y0.3081 Z0.0109 I-0.3081 J0.00000
    G01 G40 X-0.3081 Y-0.3081 F196.8
    G00 G90 Z1.
    G90 G0 Z1.
    G91 G30 Z0
    G30 X0 Y0



  7. #7
    Registered
    Join Date
    Jul 2005
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    Wow thatís pretty impressive. What material are you cutting? We specialize in plastic so we never even cut a taper for an NPT thread on the mills. We just use the recommended size on a drill chart. But like I said thatís plastic. Now on a lathe itís different we always turn or bore the correct taper.



  8. #8
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    Class 30 gray iron. We rarely taper ream either, I was just learn'in/play'in with the G3.1 virtual axis function on our new Mazak FH8800 machining ctr.



  9. #9
    Registered
    Join Date
    Jul 2005
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    yeah you threw me for a loop I had never even seen a G3.1 before Mazak has their own controls right? We use Fanuc we have a couple of Haas' a Fadal and a couple of older smaller machinig centers.

    Last edited by shawn; 08-25-2006 at 05:05 PM.


  10. #10
    Registered
    Join Date
    Jul 2003
    Location
    New Zealand
    Posts
    1173
    Downloads
    0
    Uploads
    0

    Default

    Is boring the tapered hole a problem if you don't have a reamer?

    I have a program that can generate a helix path to cut the taper. If a chamfer is required this can be generated and added.
    The program is listed here.

    http://www.cnczone.com/forums/showth...404#post190404
    Just ask if more info required.



  11. #11
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by shawn
    yeah you threw me for a loop I had never even seen a G3.1 before Mazak has their own controls right? We use Fanuc we have a couple of Haas' a Fadal and a couple of older smaller machinig centers.
    Mazak does have their own controls but as an option they can use "G-code" as well. If I'm not mistaken Fanuc has somthing like G3.1 probably an option though



  12. #12
    Registered
    Join Date
    Jun 2006
    Location
    USA
    Posts
    478
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Kiwi
    Is boring the tapered hole a problem if you don't have a reamer?

    I have a program that can generate a helix path to cut the taper. If a chamfer is required this can be generated and added.
    The program is listed here.

    http://www.cnczone.com/forums/showth...404#post190404
    Just ask if more info required.
    Cool prog. how do tell it different dia. tools or do you just use cutter comp.?



Page 1 of 2 12 LastLast

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
  •  


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed