508,289 active members
2,838 visitors online
Register for free
Login
IndustryArena Forum > CAM Software > Dolphin CADCAM > Threading function for Lathe Help?
Page 1 of 2 12
Results 1 to 12 of 23
  1. #1
    Registered
    Join Date
    Dec 2006
    Posts
    926

    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
    Moderator HuFlungDung's Avatar
    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
    Registered
    Join Date
    Dec 2006
    Posts
    926
    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
    Gold Member
    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
    Moderator HuFlungDung's Avatar
    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
    Registered
    Join Date
    Dec 2006
    Posts
    926
    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
    Moderator HuFlungDung's Avatar
    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
    Registered
    Join Date
    Dec 2006
    Posts
    926
    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
    Moderator HuFlungDung's Avatar
    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
    Registered
    Join Date
    Dec 2006
    Posts
    926
    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
    Registered
    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
    Registered
    Join Date
    Dec 2006
    Posts
    926
    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?

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 General Metalwork Discussion
    Replies: 11
    Last Post: 07-28-2008, 08:32 PM
  3. CNC Lathe Threading
    By lathe guy in forum General Metalwork Discussion
    Replies: 9
    Last Post: 03-19-2007, 11:21 AM
  4. Threading on a CNC lathe
    By Mcgyver in forum General 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
  •