584,874 active members*
5,364 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > BobCad-Cam > Thread Milling NPT
Results 1 to 18 of 18
  1. #1
    Join Date
    Feb 2007
    Posts
    55

    Thread Milling NPT

    Hi,
    Can anyone help me with a threadmilling problem.
    I'm needing to produce a 1" NPT Thread, on a part and don't know if or how to produce it with BobCad.
    I hope someone can help, as I'm getting desperate to do this

  2. #2
    Join Date
    Aug 2005
    Posts
    300

    Trhead milling

    Hi,

    I copied and pasted this from the BC24 help files. Hope it helps.

    Ernie


    Thread Milling
    The Thread feature allows the user to create a thread milling procedure. When a Thread feature is added to the CAM tree, the system will also add the following items:



    Start Point - This item in the CAM tree allows the user to specify a location for the tool movement to start.



    Thread - Right click on this item in the CAM tree to produce a pop-up menu with three options for the user to choose from:

    Edit - Allows the user to modify the settings that are used when calculating the tool movements. See The Thread Mill Wizard for detailed explanation of this dialog and all of the options available for this feature type.

    Compute Toolpath - When this option is selected from the pop-up menu, the system will begin calculating the toolpath.

    Post Yes/No - This option allows the user to determine whether a feature in the CAM tree will be included in the code that is posted by the system.



    Mill Thread - Right click on this item in the CAM tree will produce a pop-up menu with two options for modifying the visibility and color of the toolpath that is created:

    Color - When this option is selected from the pop-up menu, a dialog will appear allowing the user to change the color of the selected threading toolpath.

    Blank - When this option is selected from the pop-up menu, the system will hide the selected threading toolpath if it was previously hidden or show the threading toolpath if it is visible in the Workspace.

  3. #3
    Join Date
    Apr 2009
    Posts
    3376
    To do a NPT thread in Bob,here is a brief explanation on how.Let me know if you need more in depth explanation.
    From the other menu,pick spiral,fill in the Wizard.For example figure how much length you want,starting at x amount of depth of thread,and from there you can figure out if you start out at x amount,and if the pitch of thread is this per inch,it is just a matter of simple math to fill in the end depth.Now pick 3d engraving.Hint in Wizard,when asked for total depth put like .001.Tool pick is not possible to do correctly so that it back plots right.Pick like .010 or whatever,compute tool path.You will have to watch out to make sure it retracts right or may have to manually edit code.
    Attached Thumbnails Attached Thumbnails 1.000 npt.JPG   npt spiral.JPG  

  4. #4
    Join Date
    Feb 2007
    Posts
    55

    NPT Spiral

    Hi jrmach and ErnieD,
    Thanks for your help, not 100% sure about the spiral info needed, could you give me an example based on the following info -
    1" X 11 1/2 NPT
    depth = 25.5mm (1.004")
    cutter Dia 17mm (if its needed)
    Pitch = 2.2086 (0.0869")
    Hole Dia = 29.4 (1.5/32 or 1.156")

    I hope if you can do me this as an example, I can work out how to do other spirals for NPT, such 3/4" NPT and 1 1/4" NPT
    Thanks again

  5. #5
    Join Date
    Apr 2009
    Posts
    3376
    hI segengineering ,to do this all the way correct,the hole diameter you are stating 1.156 is a tap drill size.A true NPT would have a tapered bore with taper being .750 per foot or 1 degree,47 minutes per side.If you go ahead and use a tap diameter straight hole,it is hard on thread mill as it will cut deeper towards end of hole than need be.Not as big issue with softer materials or limited part runs.Anyhow,if we are going to use a "tap drill" hole,the size 1.156 is correct.What we need to know from here is what most outward part of the cut ,the major diameter, is going to be,both at the beginning of hole and end of hole.At beginning of cut ,the major diameter of thread would be about 1.3086.At end of hole it would be 1.3086-.0625(taper effect on diameter)equals 1.2461.Now I have the basic numbers to do a spiral.In black is spiral I did reflecting these numbers.In blue is the same but also taking in consideration for tool diameter.Since there is no tool offset in cam,we need to make spiral with radius of tool also subtracted.Second pic shows this,if I did my metric conv. right.A few things to note:when doing cam,for depth of cut put .001.For tool info does not matter,but put feeds and speeds you want.Watch the end of cut,then lead out.Will have to edit manually.Will Bob do NPT threads,answer kinda of.Leaves alot to be desired.
    Attached Thumbnails Attached Thumbnails 1.JPG   2.JPG  

  6. #6
    Join Date
    Apr 2009
    Posts
    3376
    I tried to attach a Bob file and zipped it.Can not seem to do.Some one help please.

  7. #7
    Join Date
    Feb 2007
    Posts
    55

    Thanks

    Hi,
    Thanks for all the help I will give this a try on next NPT thread I need to produce.

  8. #8
    Join Date
    Sep 2006
    Posts
    296
    Do yourself a favor. Buy an inserted thread mill tool. They are relatively cheap $150 for a tool holder and insert is about the range. Ive thread milled NPT thread numerous times and it is so easy i wish id have tried it a decade ago. The NPT taper is built into the insert and all you have to do is drop down in the hole, feed over on X or Y to the diameter you need, then G02 360deg and move down on Z the pitch of the thread in the same move. Thats it. Its that easy.

  9. #9
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by GITRDUN View Post
    ..... then G02 360deg and move down on Z the pitch of the thread in the same move. Thats it. Its that easy.
    Not really. Just doing a full 360deg at the same radius is not correct. The radius at the end of the 360 has to be about 0.005" smaller than at the start due to the thread taper. Advent threadmilling programs approximate the taper by doing four 90deg partial circles that step inwards.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  10. #10
    Join Date
    Sep 2006
    Posts
    296
    Quote Originally Posted by Geof View Post
    Not really. Just doing a full 360deg at the same radius is not correct. The radius at the end of the 360 has to be about 0.005" smaller than at the start due to the thread taper. Advent threadmilling programs approximate the taper by doing four 90deg partial circles that step inwards.
    As i stated, the threads taper is ground into the insert. The insert is the length of the effective thread, so it cuts all threads in one pass, you arent chaseing one thread from top to bottom. It cuts the top of the thread off. Thats what makes it so easy. Any NPT thread over maybe 1/4" i use an inserted thread mill.

  11. #11
    Join Date
    Jul 2005
    Posts
    12177
    Yes the taper is ground into the insert but for it to cut a correct thread during each circle the tool must follow that taper. In other words it must spiral in or out depending which direction the tooling is moving and whether it is an OD or ID thread.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  12. #12
    Join Date
    Feb 2007
    Posts
    55
    Hi GITRDUN,
    What Geof says about the insert tapered tip having to follow the spiral is correct, what your saying is how you do thread milling for all non-taper threads.
    Thanks for your input.
    segengineering
    PS thanks to you to Geof, and jrmach and anyone else that as or can continue to help, someone may know an easier or simple way to do these tapered threads

  13. #13
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by segengineering View Post
    .... simple way to do these tapered threads
    The simplest way I know about is to get the program from the tool supplier.

    The alternative is not simple, calculating the radial increase and hand coding a dozen quarter circles gets tedious.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  14. #14
    Join Date
    Sep 2006
    Posts
    296
    I dont want to start an argument here, i just posted to try and help a guy out. But you are over complicating something that just isnt that complicated. With a tapered insert, start with the top thread of the insert one pitch above the surface, make one 360deg pass and down on Z the pitch depth. Its just that simple. To cut deeper than the effective thread for a second pass just calculate how much you need to step in to keep the angle correct. Thats where it gets complicated and drawing it up to get dimensions helps.

  15. #15
    Join Date
    Apr 2009
    Posts
    35
    Hi Git-R-Done.

    Not trying to be complicated. I have programmed the taper threads single point and tapered insert. If you would code a single point thread you would see that that the circle the radius follows is continously increasing as you raise Z. That's why to create the 'perfect' npt with a tapered insert, the tapered insert tool need to increase the radius as you raise Z. Not much mind you... and in all practicallity it doesn't need to change. I understand the need, but never do when I use the tapered insert tool.

    segengineering, if you are using a Fanuc, there are some macro programs that can do all the math for you. In the macro you would enter a few variables and the fanuc would do all the math to continously decrease the spiral as you dropped Z.

    Let me know if you are planning to single point instead of tapered insert, and you are using a Fanuc. I'll see if I can find the macro and attach. It's probaby on the CNC zone in the Fanuc section.

    Best regards,

    Robert

  16. #16
    Join Date
    Mar 2010
    Posts
    1852
    I have never heard this made so complicated. I'm sure a single pass will suffice for almost all applications. Never heard otherwise. That is why they make these single pass inserts.
    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28

  17. #17
    Join Date
    Feb 2007
    Posts
    55
    Hi,
    My mill is siemens control with shopmill, but it doses have a mode to run FANUC programs, so if you do have any FANUC programs that will help I can give them a try.
    I do my threadmilling with either solid carbide or insert style multi toothed cutters.

    Quote Originally Posted by robrea View Post
    Hi Git-R-Done.

    Not trying to be complicated. I have programmed the taper threads single point and tapered insert. If you would code a single point thread you would see that that the circle the radius follows is continously increasing as you raise Z. That's why to create the 'perfect' npt with a tapered insert, the tapered insert tool need to increase the radius as you raise Z. Not much mind you... and in all practicallity it doesn't need to change. I understand the need, but never do when I use the tapered insert tool.

    segengineering, if you are using a Fanuc, there are some macro programs that can do all the math for you. In the macro you would enter a few variables and the fanuc would do all the math to continously decrease the spiral as you dropped Z.

    Let me know if you are planning to single point instead of tapered insert, and you are using a Fanuc. I'll see if I can find the macro and attach. It's probaby on the CNC zone in the Fanuc section.

    Best regards,

    Robert

  18. #18
    Join Date
    Aug 2008
    Posts
    93

    Re: Thread Milling NPT

    Quote Originally Posted by Geof View Post
    The simplest way I know about is to get the program from the tool supplier.

    The alternative is not simple, calculating the radial increase and hand coding a dozen quarter circles gets tedious.
    That's what I did, BobCad made a mess of it. I just edited the program and pasted in G-code I got from the tool maker. I have yet to get a program from BobCad that runs without edits to it.

    Their G-code for a NPT thread was about a hundred lines long. The tool providers was about 7. ( solid carbide multi-tooth cutter.)

Similar Threads

  1. Thread milling with x z c
    By murrayclair in forum Mazak, Mitsubishi, Mazatrol
    Replies: 3
    Last Post: 04-16-2011, 03:03 PM
  2. Thread milling on X2
    By webgeek in forum Benchtop Machines
    Replies: 10
    Last Post: 04-02-2010, 02:13 AM
  3. Thread Milling
    By sambo67 in forum MetalWork Discussion
    Replies: 7
    Last Post: 02-13-2010, 07:10 AM
  4. 0M-Thread milling?
    By mikul in forum Fanuc
    Replies: 1
    Last Post: 12-06-2006, 06:56 AM
  5. thread milling
    By STS_Kevin in forum Daewoo/Doosan
    Replies: 0
    Last Post: 11-29-2006, 01:50 AM

Posting Permissions

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