584,826 active members*
5,293 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Dolphin CAD/CAM > Threading function for Lathe Help?
Page 1 of 2 12
Results 1 to 20 of 23
  1. #1
    Join Date
    Dec 2006
    Posts
    947

    Threading function for Lathe Help?

    I've got a pretty good start on using Dolphin CAM for my lathe turning project, but I'm having some confusion about the threading.

    So I define the start and end points, I take it X stays the same (unless it's a tapered thread) as I don't need to calculate the depth the threads are going to take up?

    Next it lists TPI, is this threads per inch or turns per inch? It seems as though I can select one value either Lead, Pitch or TPI, which should I be using?

    Also where do I find specs for different threads? I have a program called ME Consultant by Mike Rainey and it gives a ton of different specs but I have no idea what I'm looking at, plus they don't as high as I need. Basically I need to know how deep the threads are for a metric thread 45mm? Also what is the depth of cut on a 16ER triangle style insert? I've looked everywhere I even downloaded Iscar and Kenmetal's catalogs and it mentions nothing about depth of cut. Can a 16ER insert do metric threads?

  2. #2
    Join Date
    Mar 2003
    Posts
    4826
    What kind of a threading cycle is your CAM going to produce? Lathes commonly use G76 threading cycles, which are kind of a shorthand code that invokes a macro that causes the machine to execute all the moves necessary to finish the thread.

    The long hand way would be G33 single pass threading, where every movement is written out in full by your CAM program.

    In either situation, you generally will need to tell the program what the finish depth of the thread is. I don't have ME consultant handy, but I believe it should have some factor similar to the minor thread diameter or full depth of thread, which would be a starting point for a thread depth figure.

    The lead of the thread is how far along the axis the tool must move while the thread makes 1 revolution on the part. 10 threads per inch (aka TPI or 10 pitch) = 0.100 lead, or 0.100 pitch.

    It is possible for some types of parts to have multiple parallel threads, commonly called 2 start (or 3 start or more) threads, because the designer wants the nut to travel fast on the part, but does not want to cut a huge, deep coarse thread to accomplish this. If you look at such a part, you might count 10 threads in one inch, but because it is a two start thread, the lead is 0.200", and the nut will wind on 1" of length with only 5 turns. The pitch of a multistart thread generally ignores the lead, and just counts how many threads per inch. So a two start, 10 pitch thread can be computed to have a 0.200 lead. Clear? If you know the lead, that is what is really important for the thread cycle.

    Metric thread pitches are always based on the lead of the thread. Your 45mm example, you did not state the pitch of the thread. Nonetheless, for a given pitch, the incremental depth (depth from the Outside Diameter) of the thread is always the same regardless of the diameter of the part, so you can figure out the correct cutting depth from other thread examples within the range of the chart you are looking at. This is known as interpolating or extrapolating the chart.

    I'm not certain about your 16ER insert designation. Is that a thread tool or a triangular turning insert?

    As for the incremental step down for depth of cut, that is a matter of judgement. Most machinists thread with multiple passes which decrease in incremental depth because the cutting load gets higher as the tool gets deeper. What this stepdown amount should start at depends on the thread pitch and how sturdy your tool and machine and setup are.

    An added wrinkle, if your machine is set to work in inches, then you'll need to convert your metric thread pitch into either TPI or the actual pitch in inches per turn, when you input your thread cycle data into your CAM. I don't run Dophin, so if you post more specifics of the actual thread you will be cutting, the next guy may be able to help you with more specific instructions.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Join Date
    Dec 2006
    Posts
    947
    Hu, thanks for the lengthy explanation. I'd rather do a conversion anyway as I don't care if it's metric or not and I'd rather use amercain standard as I understand it better, I just didn't know if making a custom thread from 1.7716" diameter was going to be hard or not, sounds like it doesn't matter it's all the same to the machine.

    I'll use 1.7716 as the diameter and do 16 threads per inch. I don't understand the thread app below is a screen shot, what are the actual height of the threads?

    As for the depth the tip of the tool can go, yes I was talking about a 16er triangle insert with the little 60 degree point on each corner.

    As for the cycle I have no idea as this is my first time using anything Dolphin.
    Attached Thumbnails Attached Thumbnails threads.jpg  

  4. #4
    Join Date
    Jun 2004
    Posts
    6618
    I have Dolphin as well, but won't get into threading for some time.
    I still have a little manual minilathe I can thread with in the meantime.
    It helps to understand or to have seen what threading looks like on a manual lathe. This will help to visualize what the CNC should be doing.

    For just standard threads, it is really very simple. Outside and inside are basically the same passes. The tools are different of course. I think feed, speed and tools are the most critical.
    Then travel extents.

    For any new cod on my lathe, I always test it in the middle of the bed first cutting air.
    I have no tailstock, so all my parts are cut as close to the chuck as I am comfortable with. That close is no place to go testing code.

    I look forward to your results. Good luck with it.
    Lee

  5. #5
    Join Date
    Mar 2003
    Posts
    4826
    The number from the chart you want to refer to is called "Height", and this is a radial value, since it is the height of the cross section of the thread form. So for programming the cnc, the final X position will be:
    Major Diameter - 2*height

    Notice the value called "Flat". The standard thread form is not razor sharp, but is flat on the top. The width of flat is different for an external thread than it is for an internal thread. Internal threads have a wider flat, which is actually a result of what size the hole is drilled or bored. For the purpose of tapping threads, it takes a lot less power to tap a thread if you increase the size of the drilled hole.

    Anyway, the reason I mention that, is if you use standard turning inserts, or general purpose thread inserts, the width of the tip is probably going to be incorrect for the particular pitch you are going to cut. This has the effect for throwing off the X endpoint of the thread, because your touch-off point (in X) does not coincide with the assumed correct toolpoint form that the ME Consultant is assuming you are going to use.

    If you use a general purpose turning tool to cut threads and it has a .015 or .031 tip radius, you will most likely overcut the thread width if you use 2*Height. If you use a sharp pointed thread tool, you will likely have to cut deeper than 2*Height because the tip is almost sharp.

    But, you can trial cut the threads, and measure the pitch diameter with thread wires to see where you are at. A set of PeeDee thread measuring wires is relatively inexpensive and well worth having to check the pitch diameter of trial cut threads to that you can adjust your program without so much guesswork.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  6. #6
    Join Date
    Dec 2006
    Posts
    947
    OK, more confused than ever LOL. I think I'm getting it DAM TERMINOLOGY.

    Hu, you said the final X position will be major - 2*height, I understand what you're saying but in Dolphin unless it's a tapered thread the X never changes, it just asks for final depth and it does the rest.

    So how would I go calculating a custom UNC (american thread) for my 1.7716? If I start off with this diamter and cut threads the outside diameter will still remain fairly close to 1.7716, granted I haven't taken the tops off of the threads (flats) for external threads? Should I just look at the depth of threads for a 1.75" thread and copy that? Because all I can find is 1 3/4"-5, I want a fine thread something like 16 to 32.

    I'm using these inserts, would these do the job? http://www1.mscdirect.com/CGI/NNSRIT...MT4NO=63079878
    I have to do at least 16 TPI for these inserts.

  7. #7
    Join Date
    Mar 2003
    Posts
    4826
    Check ME consultant for the data on a 3/8 UNC thread, which is 16 tpi. You can get the thread height from that. Then, you might have to run a couple of experimental sessions in Dolphin, to know whether it can handle the single thread height value, or whether you need to double it, in order to get the correct output.

    If you double the thread height, and subtract it from 1.771, you will get the final X diameter for the tool at the bottom of the thread. You can then scan through the nc code and see if it outputs values in the correct range of final values. It should be easy to spot a major error because X final depth will be half or double what you'd expect from the results of the calculation.

    The thread insert you have chosen perfectly matches the thread form and pitch, so you're good to go.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  8. #8
    Join Date
    Dec 2006
    Posts
    947
    Thanks. I'll try that. How do I calculate the ID of the piece I want to thread internally to screw onto the part we just talked about? Should I use the same specs as the 3/8 UNC because it's height and bore will be about the right proportion? The nut is the less hard part to me as it won't take a lot of material and if I mess it up who cares. I'll definately have to run some test.

  9. #9
    Join Date
    Mar 2003
    Posts
    4826
    For the nut ID, you look at the ME consultant "Internal Data", minor diameter, of the 3/8 UNC. Take the difference between the major and the minor diameter, and subtract that from your 1.7717 major OD, to find the bore size for your nut.

    Notice that the minor diameter for the internal thread is larger than the minor diameter for the "External Data". This represents additional clearance for the root of the external thread, and also explains why the internal thread has a wider looking flat on the crest, than the external thread.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  10. #10
    Join Date
    Dec 2006
    Posts
    947
    Cool thanks. I knew once I started getting into threads it was going to be confusing and hard, but I'm slowly learning.

  11. #11
    Join Date
    Apr 2009
    Posts
    6
    I have a old book from the henry ford trade school, formula for thrds are as such, cos. 30 deg, is .86603= thrd form. male thrds are 75 percent= .64952 female thrds are 62.5 percent .54127 take 1" divided by # of thrds then multiply by these values, it will give you single depth of thrd. If you have a fish tail, or thrd gage as some call it you can use this formula and multply by two and it will show you the values that it has written on the gage. now this is only for the od. the ID you will double and subtract from the dia. you wish to cut. Good luck. Minard

  12. #12
    Join Date
    Dec 2006
    Posts
    947
    Thanks everyone, I've just looked at the meconsultant and reread this thread. I'm slowly starting to understand.

    Hu, I understood what you said about the flats on the internal thread and how to calculate the starting bore for the internal threads, but I don't understand how the flats get made. The internal boring threading tool I have uses the same inserts as the outside. Is it just a fact of boring to the correct ID and then cut the threads a little less using the "height" in the meconsultant to get the flats?

  13. #13
    Join Date
    Mar 2009
    Posts
    23
    Cartierusm,

    A quick formula for threading is Major-pitch=minor.

    3/8"-16 thread. 3/8"(.375) -16TPI (1"/16threads=.0625) = .3125 diameter.

    Turn your material to .375, make your last thread pass @ .3125 dia. (then offset down according to the tool push off)

    For internal, bore to .3125, and make your last thread pass @ .375. (and offset up for tool push off.)

    On o.d threads start your x initial point well above the major dia. so if you have to offset down for tool push off, you wont trail across the top of your threads on retreat.
    On i.d. threads, make x initial well below the minor for same reasons.

    If your doing commercial work this should get you there. If you need something more precise, check your software, or a machinist hand book for thread specs. Always be mindful of which class thread(1-2-3) is being called for.

    As for topping inserts, have seen some programmers leave .01 on diameter, and then thread with a topping insert until the major is to size. I have had some unsatisfactory results with that as on some threads you cannot utilize the full tolerance of the pitch without undercutting the major diameter. As well as on some material when the insert starts cutting the major, it sets up a chatter in the threads.

    Apologies for the length of this.
    Paul G.

  14. #14
    Join Date
    Sep 2008
    Posts
    229
    Quote Originally Posted by Cartierusm View Post
    Also where do I find specs for different threads
    There are many compliations of thread data on the internet. This is just one of them (that I compiled myself many years ago).
    http://www.bodgesoc.org/thread_dia_pitch.html
    It isn't entirely exhaustive but it does cover 0.01" instrument threads to 6" pipe threads. M45 coarse (including thread depth) is included.

  15. #15
    Join Date
    Mar 2003
    Posts
    4826
    Quote Originally Posted by Cartierusm View Post
    Thanks everyone, I've just looked at the meconsultant and reread this thread. I'm slowly starting to understand.

    Hu, I understood what you said about the flats on the internal thread and how to calculate the starting bore for the internal threads, but I don't understand how the flats get made. The internal boring threading tool I have uses the same inserts as the outside. Is it just a fact of boring to the correct ID and then cut the threads a little less using the "height" in the meconsultant to get the flats?
    The flats are a specification for the threads, and they are the result of, as you say, turning and boring to the correct diameter. A topping form insert will begin cutting the top of the thread flat for you, if you get too deep.

    Typically, a threading tool raises a bit of a burr on the top of the thread anyway, so a topping insert will trim that burr off. Otherwise, it is necessary to file the burr off the top of the external thread (PS: learn to file with your sleeves rolled up, and hold the file left-handed. Threads can easily snag lose clothing with dire consequences). Thread burrs can easily fool you into thinking that you need to be cut deeper, when in fact, the burrs cause interference in the guage.

    Because the specification for internal threads is a flat width that is 1/4 of the pitch, the burrs on internal threads generally do not need to be removed, because they are still well below causing interference with the gauge.

    It is good to know about the proper look of the finish threads, and knowing that the flat crests are part of the specs will help.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  16. #16
    Join Date
    Dec 2006
    Posts
    947
    Hu, I've understood a lot since I last posted. It's weird seems so obvious now LOL. Anyway, I do have some more questions. Remember I'm using 16 ER Triangle Threading Inserts, they are labeled partial profile, what ever that means. In the Kennametal catalog it says these inserts are used to create multiple threads from 16-48 TPI. What that means is that it's a general inserts as opposed to an insert designed specifically for 32 TPI. At least that's the way I understand it.

    Now the questions I have are to make a custom thread, I've already tried and learned a lot, the external thread part is very complicated and it doesn't make sense to make that first even though from what I've been told external are easier to diagnose. So I would rather make the internal one first (the nut). Here some info; the diameter of the external thread is 1.6366" and 16 TPI. So from the threading info I have the thread needs to be .0383" deep. The bore of the nut then should be 1.569" and goes to a depth of .0338". I got this by taking the OD of the external thread and subtracting .0338" twice for the thread depth. This didn't work out so well.

    So what should I do to calculate the internal bore? Earlier you also talked about FLATS, and I understand what you mean but how are they make with the threading tool or a regular boring bar and how do you calcualte where they go?

    Then how do I test a custom internal thread with nothing to test it on? Thanks I appreciate the help.

  17. #17
    Join Date
    Dec 2006
    Posts
    947
    OK, I missed the second page of this thread, even though I read it originally. So disregard the post above and look at these questions.

    I've decided to get Full Profile inserts for the 16 TPI so I won't have to worry about the flats.

    So if my OD of my bolt is 1.6366", I cut to .0383" for 16 TPI. Then for the Nut I take 1.6366" and add .0338" and .0338" for an ID of 1.569" and cut to a depth of .0338" and because I'm using full profile insets I don't need to worry about extra clearance or the flats. So for the internal just make sure that at the last pass or so that the threads are deep enough to reach the part that trims the flats. Then when making the external threads make sure they come to a point. Does that sound correct?

  18. #18
    Join Date
    Mar 2003
    Posts
    4826
    Make an external thread first, and use it to gauge the inside threads. I would get a set of thread measuring wires, so that the correct pitch diameter of the external gauge can be calculated. PeeDee thread measuring wires are inexpensive and indispensible for thread cutting.

    The full form external thread is not sharp pointed. I think I explained this above, the full form thread has a flat that is 1/8 of the thread pitch wide. The internal thread has a flat that is 1/4 of the thread pitch wide. This is assuming that you begin with ODs and ID's that are standard. The full form external insert will clean the OD of the external thread but will not touch the crest of the internal thread, unless you get a different insert for the internal thread. I am not sure if they make these full forms in external and internal forms. I've always cut threads with partial profile inserts.

    When boring a thread, you would generally know what diameter the tip is set at (in your touch off procedure). There is no point in trying a gauge in an internal thread until the tool has at minimum, advanced to the major diameter of the external thread. At this point it is going to be getting close, and the thread gauge will start to screw in but will get tight very quickly. So then you can adjust the threading program so that the final passes get a little bit larger, run through the whole program again and let it scrape out the final cuts and retest.
    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  19. #19
    Join Date
    Dec 2006
    Posts
    947
    Ok, but for a 3/8-16 thread the internal crest is .0156 and the thread height is .0338". So do I cut a .0338 thread depth then cut the crest .0156 deep or cut a thread .0494 (.0388 + .0156) deep then cut the crest so the final thread depth is .0388". Thanks.

  20. #20
    Join Date
    Dec 2006
    Posts
    947
    I ordered a set of the wire gauges. Now I understand you use 3 of them but I don't have a mic that big, the threads I'm making are in the 1.75" range. I have an accurate digital dial caliper can I use those? I mean you just need a measuring flat to hit those wires?

Page 1 of 2 12

Similar Threads

  1. ID threading lathe
    By 100 in forum Haas Lathes
    Replies: 9
    Last Post: 12-12-2009, 01:56 AM
  2. Threading on a lathe.
    By Nic Scheepers in forum MetalWork Discussion
    Replies: 11
    Last Post: 07-28-2008, 08:32 PM
  3. CNC Lathe Threading
    By lathe guy in forum MetalWork Discussion
    Replies: 9
    Last Post: 03-19-2007, 11:21 AM
  4. Threading on a CNC lathe
    By Mcgyver in forum MetalWork Discussion
    Replies: 6
    Last Post: 08-20-2005, 10:47 PM
  5. CNC Lathe Threading
    By DDM in forum Uncategorised MetalWorking Machines
    Replies: 5
    Last Post: 08-20-2004, 03:27 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
  •