Results 1 to 10 of 10

Thread: Multiple Lead Threads

  1. #1
    Registered
    Join Date
    Jan 2007
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Question Multiple Lead Threads

    Hello everyone. I am running a Leadwell LTC-15 2-axis lathe with a Fanuc-OT controller. I have used G32/G76 for thread cutting in the past and it has worked out fine. Now, I need to cut a thread with 4 leads. I am reading through my operators manual (CNC Bible!) and the only thing I see regarding multiple lead threads is about half a page that says " Variable Lead thread cutting" Is this the same as multiple lead thread cutting? Also, could someone elaborate on the code for me a little bit. It is extremely vague. The only thing I am reading right now is : G34 IP_F_K_; and it tells me that F = Lead in Longitudinal axis direction at the start point, and K=Increment and Decerment of lead per spindle revolution. Nothing about the I or P. Im not even sure if this is the correct code to be using, it was my first guess. We have a manual lathe that can cut multiple lead threads, so Im almost positive that this CNC should be able to do it. Anyways, thanks for any help ahead of time, you guys always come through. Thanks.

    Similar Threads:


  2. #2
    Registered Get lucky's Avatar
    Join Date
    Jul 2008
    Location
    us
    Posts
    109
    Downloads
    0
    Uploads
    0

    Default

    This is how I made a acme 6 lead internal thread on kia turn 21 with a Fanuc oi-tb


    N500M01
    N4(I.D.THREAD TOOL)
    G0T1000M8
    G97S300M3
    G0X.41Z.375T1010
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z.5
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z.625
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z.75
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z.875
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z1.
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z1.125
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G0Z1.25
    G76P010000
    G76X.52Z-1.39P510Q250F1.
    G28U0W0T1000

    If this helps

    You must remember that 99% of my posts are Bullchit!


  3. #3
    Registered beege's Avatar
    Join Date
    Feb 2008
    Location
    USA
    Posts
    566
    Downloads
    0
    Uploads
    0

    Default

    Variable is NOT the same as multiple. Variable has a different lead at the start than it does at the finish.

    To create multiple start, create one thread at say, Z.250. Calculate the second thread pitch difference, and add that to the start of the Z.250, That is, if the pitch of each thread is .040", position the second thread start at Z.270 (that's for a double start thread, modify as needed for other multiple thread types)



  4. #4
    Registered dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2709
    Downloads
    0
    Uploads
    0

    Default

    I believe if you set your control up to use 11T program format (TAPEF=1), you can use a shift value instead of backing Z away for each thread.

    G76X_Z_I_K_D_F_A_P_Q_;
    I : Difference of radiuses at threads
    K : Height of thread crest (radius)
    D : Depth of the first cut (radius)
    A : Angle of the tool tip (angle of ridges)
    P : Method of cutting
    Q: Shift angle of thread cutting start angle

    Attached Thumbnails Attached Thumbnails -0t-tapef-setting-jpg  


  5. #5
    Registered
    Join Date
    Jan 2007
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    Im back again, and I think I am pretty close. I decided to go against changing paramaters, and using a shift value; Time is Irrelevant here, I just backed it away. I dont think its perfect, but I know im close. I just want to verify that I am doing the correct thing. I have no clue what the actual thread I need to cut is, I am simply trying to see if I can make a 4 start thread right now; and I had a piece of 2" hanging around, so I am trying to cut a 2"-1 TPI 4 start thread. I read a programming manual and it says I need to do 4x the lead to get my feedrate, which is where I got the 4 IPR from. It makes sense in my head, but when I run it it looks like the 4 starts are not equal. There is certainly 4 distinct threads, but like I said they are not equal. I know the depths are all wrong, I just wanted to mark my piece and see if it was correct. Anyways, heres my code, let me know if Im on the right track here :

    G0 T0404
    G97 S250 M3
    G99 Z.250 X2.5
    M08
    G76 X1.995 Z-2.5 F4.0
    G76 X1.990 Z-2.5 F4.0
    G01 Z1.250
    G76 X1.995 Z-2.5 F4.0
    G76 X1.990 Z-2.5 F4.0
    G01 Z2.250
    G76 X1.995 Z-2.5 F4.0
    G76 X1.990 Z-2.5 F4.0
    G01 Z3.250
    G76 X1.995 Z-2.5 F4.0
    G76 X1.990 Z-2.5 F4.0
    G0 T0404
    G28 X0
    G28 Z0
    M09
    M05
    M30

    Thanks a lot, hopefully I can figure this all out before the holiday break. Thanks again.



  6. #6
    Registered dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2709
    Downloads
    0
    Uploads
    0

    Default

    If you're turning at 250 RPM's and your feed is 4" per rev, you're trying to get Z axis up to 1000 IPM in about 1/4". First, I don't believe your machine will feed that fast, let alone accelerate that fast. You might try 50 RPM's... that would give you a 200 IPM feedrate. Probably more manageable. Also, move your starting Z back a bunch. I used to use 3xP for most normal threads, but that would be a bit much here.



  7. #7
    Registered
    Join Date
    Dec 2008
    Location
    England
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default 4 start thread turning

    Hi Stuby,
    the code posted looks fine, but there may be other reasons why the thread starts to appear unequally spaced.
    1. The thread lead you have programmed (thread pitch x number of starts) could exceed the maximum slide velocity for your Z axis. The actual slide velocity programmed is thread lead x rpm - in this case 1000 inches per minute! Unless you have a very expensive, very quick control and axis drive system on this lathe, you are probably exceeding the limitations for the machine. If this is the case, you can reduce the rpm until the slide velocity falls within the permitted range.
    2. Ensure that there is sufficient slide acceleration distance between the start point of the threading pass and the position where the cutting edge engages the workpiece. There is usually a nomogram in the machine tool's manual wich will give recommendations, but if you do not have this information, a figure of around three x lead usually does the trick.
    Fred the thread



  8. #8
    Registered
    Join Date
    Jan 2007
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    Alright, this seems to make a little more sense now. When I originally tried this thread without any help from books, I had it at 1 IPM, which would be 250 IPM, it seemed very fast. Then when I moved it to 4 IPM, 4 times what it was before, it didnt seem that much faster; makes more sense now. I just threw 250 rpm out there as I usually do single start threads somewhere around there. Ill give this a shot as soon as I hit the shop floor, Thanks a lot you guys. really appreciate it.



  9. #9
    Gold Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12142
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by stuby View Post
    ....I am simply trying to see if I can make a 4 start thread right now; and I had a piece of 2" hanging around, so I am trying to cut a 2"-1 TPI 4 start thread. I read a programming manual and it says I need to do 4x the lead to get my feedrate, which is where I got the 4 IPR from....
    I could be misunderstanding what you mean; and I could be all wrong in the following.

    My understanding of TPI is that it means Turns Per Inch, i.e. 2"-1 TPI is one turn per inch or in other words the Lead is 1"; lead is the distance travelled in one revolution of the thread.

    Pitch is not always the same as Lead; the Pitch is the distance between adjacent threads.

    On a single start thread Lead and Pitch are the same.

    On a four start thread with a Lead of 1" the Pitch will be 0.25"

    When you multiplied the 1" by four you came up with 4" per turn which seems rather big for only 2" diameter; this gives a helix angle of about 32 degrees which is more like a milling cutter than a screw.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  10. #10
    Registered
    Join Date
    Jan 2007
    Location
    usa
    Posts
    56
    Downloads
    0
    Uploads
    0

    Default

    Im back again, and with much better results. The speed was much too high for my machine to handle, so I changed RPM's down to 50, and the machine can move fast enough for that, they are most certainly 4 equal threads now. Thanks for the help.

    Geof; you are correct in that TPI is Turns per inch (I say threads, same thing) thus giving me a 1.0 lead. I used my brothers friends programming book, and it says that Pitch=number of starts x lead. Thus 4 IPR feedrate. It sounded insane when I was programming it, however it did cut correctly. Also, the 32 degree helix is what it appears to have cut. This is simply a sample to see if its do-able. The customer a piece that is roughly 7" in dia, so it will look much more thread like in a piece of stock 3.5X bigger than what I have now. Anyways, everything worked out fine, thanks everyone for your input, its always appreciated.



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