3dprintforums logo



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

Thread: G76 threading

  1. #1
    Registered
    Join Date
    May 2007
    Location
    Denmark
    Posts
    51
    Downloads
    0
    Uploads
    0

    G76 threading

    Hi.
    When threading, I use G76.
    I know of 2 ways to descripe the syntax for the thread, but I can only find the right syntax for single line G76.
    I have G76 X8. Z-10. P613 Q250 F1 A60 for an internal M8*1 thread.
    I would like to try to use the dual-line G76, but whats the syntax?
    I need it to be able to switch between ways to execute the way the thread is made (front of insert, back of insert, etc.)

    Similar Threads:


  2. #2
    Registered
    Join Date
    Jan 2005
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    G76

    G76- Canned threading cycle

    G76 P010010 Q0020 R0005 (first G76 sets parameters for threading)
    G76 X Z P Q F R (cuts the thread)

    The first G76 isn't needed but is recommended.
    - G76 P Q R

    P010010 sets 3 things
    - first 2 digits is the amount of finish passes - 01

    - second 2 digits is % of the lead or pullout exiting the thread- 00
    00 = almost no angle at pullout and 99 = 9.9 leads away start out

    - third 2 digits are the angle of infeed - 10
    0-99 are usable

    Q0020 sets the minimum cut amount during threading .002 but no decimal
    (Q00200 for sub inch)

    R0005 sets the cut amount of the last pass .0005 but no decimal
    (R00050 for sub inch)

    The second G76 cuts the thread.
    -G76 X.1876 Z.3 P0302 Q0010 F.05 (R-.002) FOR 1/4-20

    X.1876 =Minor Dia. of thread

    Z.3 or (W) =The ending Z of the thread

    P0302 =Height of thread in radius (Maj-Min)/2 (.0302)
    (P03020 for sub inch)

    Q0100 =Amount of the first cut. All the rest of the cuts are calculated.
    (.01)
    (Q01000 for sub inch)

    F.05 =Feed-rate 20 TPI 1/20=.05

    R = R is optional for tapered threading. R is the amount of
    difference in X from start to finish in Z. When cutting threads
    moving Z and X in a positive direction R is a negative value.



  3. #3
    Registered Karl_T's Avatar
    Join Date
    Mar 2004
    Location
    Dassel,MN,USA
    Posts
    1397
    Downloads
    0
    Uploads
    0
    Great info here, in a better format than I've come accross.

    I'm programming my <Camsoft> lathe to do G76.

    I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

    Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

    Karl



  4. #4
    Registered cnc-king's Avatar
    Join Date
    Jul 2003
    Location
    united states
    Posts
    263
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by Karl_T View Post
    Great info here, in a better format than I've come accross.

    I'm programming my <Camsoft> lathe to do G76.

    I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

    Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

    Karl
    i always set my z to start 1.5 turns from start of threads
    for left hand threads i use a holder that will accomadate both left and right thread inserts and all i have to do is reverse the spindle

    referring to cogsman the last 2 digits in the first g76 line is determined by the angle of your threads which is normally 1/2 of the included angle of the thread

    If you can ENVISION it I can make it


  5. #5
    Registered
    Join Date
    May 2007
    Location
    Denmark
    Posts
    51
    Downloads
    0
    Uploads
    0
    ...but how about the option of theading with the front or the back of your insert?
    BTW, thank you for info.



  6. #6
    Registered
    Join Date
    May 2006
    Location
    Sweden
    Posts
    265
    Downloads
    0
    Uploads
    0
    If you have the F10TA/F11TA you use P1 for one-side, constant cutting amount
    P2 zigzag with constand cutting amount
    p3 and p4 just like p1 and p2 but with constant cutting depth.

    for the F0TA I dont think you can apply type of cutting, but if you got special threading needs, use G32.

    G76 X27.4 Z-52 K1.3 D400 F2. A60 P1 --- F10TA style

    G76 P011060 Q50 R50
    G76 X27.4 Z-53 P1200 Q400 F2.0 --- F0TA style



  7. #7
    Registered
    Join Date
    May 2007
    Location
    USA
    Posts
    940
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by Karl_T View Post
    Great info here, in a better format than I've come accross.

    I'm programming my <Camsoft> lathe to do G76.

    I have a question on Z start. Will the control always start threading at the current Z position and then go to Z end speced in G76 line 2? Or will it error if you're too far away? In other words, how does the control know how long the threading pass is?

    Second, left hand threads. Do you just use all negative values and cut on the backside of your part?

    Karl

    You program both the Z-axis start and finish positions. Machine threads between these 2 dimensions (minus compound infeed). One manual suggests 3 times the lead or .3 whichever is greater. At high RPM I usually start .5 in front of the thread. This is to allow the machine to accelerate to the correct feed. Machine will not error out because of thread length.

    Do not change start position, RPM, or compound infeed if re-threading. It will cause a double thread. Compound infeed on the 2-block G76 call is not adjustible from 0-99. At least not on the lathes I run. You are allowed 6 options: 0, 29, 30, 55, 60, or 80. The single block call has an A-value for the compond infeed which allows you to use any number between 0-99.

    For left hand threads, follow the advice already given. Use a left hand threading tool and reverse the spindle direction.

    Kai_DK asked about cutting with both sides of the tool. M-man's answer was correct. Notice that this option is only available in the single block call.

    You control (somewhat) how much the insert cuts on a side by using the compound infeed function of the last pair of values in the P word in the first block. 0 (zero) value has no compund infeed and cuts equally on both sides of the insert. This is a tough chip. Only used it once in 22 years of programming. 60 cuts only on the leading edge (for standard 60 deg. threads). This creates less tool pressure if you are having a chatter problem. Not the best for use on work hardening materials. Normally I stick with 29 or 55. Q in first block is minimum DOC. R is DOC of last pass. On work hardening materials you will need to keep a large enough value to make a decent cut if possible.

    As stated, the middle 2 values in the P word in the first block is for pull out. 00 will leave a ring on the last thread. I only use it with threads having a relief. I use 01 otherwise so the machine will pull out as quick as possible. Often I am threading to a shoulder and need to get as close as possible.

    Speaking of getting close to a shoulder, slow the RPM down if the 01 value won't get close enough. The slower RPM allows the insert to stay in the cut for longer. Not always best for the insert because it will be below its best operating range, but sometimes necessary.

    Hope this was of some help to you.



  8. #8
    Registered
    Join Date
    May 2006
    Location
    Sweden
    Posts
    265
    Downloads
    0
    Uploads
    0
    I always use a m-code to decide if there are chamfer or not at the end of thread, threads I make with P010060 makes a nice way out at the end even thou there shouldnt be any chamfer, mabe there are a parameter set for this amount if it is EQ to zero???. With the m-code I can make the right pitch closer to the shoulder.

    And there are actual formulas to calculate the exact amount of start and end distance of the acceleration of servo when threading at certain spindle speed.



  9. #9
    Registered
    Join Date
    Aug 2007
    Location
    USA
    Posts
    4
    Downloads
    0
    Uploads
    0

    G76 Taper

    I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

    G76 P040060
    G76 X.4392 Z-1.735 P0500 Q0100 F.05



  10. #10
    Registered Karl_T's Avatar
    Join Date
    Mar 2004
    Location
    Dassel,MN,USA
    Posts
    1397
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by habertt View Post
    I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

    G76 P040060
    G76 X.4392 Z-1.735 P0500 Q0100 F.05

    Try adding an R.003 to your second line. Should correct for your taper. You may have to experiment with the value for your control.

    Karl



  11. #11
    Registered
    Join Date
    May 2007
    Location
    USA
    Posts
    940
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by Karl_T View Post
    Try adding an R.003 to your second line. Should correct for your taper. You may have to experiment with the value for your control.

    Karl
    On our machines, this would make the taper worse. The X value in the threading cycle would be at the Z-1.735. A value of R.003 would increase the root diameter by .006 at the front of the part. (Maybe not exactly .006 because of tool pressure.) Check the manual for your machine to see how the R-value works for it.

    Karl is correct when he stated that you may have to experiment with this value. Just because it is mathematically correct doesn't mean it will work out. I usually find I have to go more than what the taper is...depending on the material and size of the tool.



  12. #12
    Registered
    Join Date
    Jan 2005
    Location
    USA
    Posts
    278
    Downloads
    0
    Uploads
    0

    Add "R-.004" on second G76 line to cut .004 taper.

    Quote Originally Posted by habertt View Post
    I have been having a problem with my thread getting a taper and causing issues with plating. The diameter is .003 smaller at z-1.735. I have made it, overall,.004 smaller but can't get rid of the taper. How do I do it. Here's my cycle for a 1/2-20 thread. (Mori ZL25-B500, Fanuc MF-D6 (16TTA) control)

    G76 P040060
    G76 X.4392 Z-1.735 P0500 Q0100 F.05

    Add "R-.004" on second G76 line to cut .004 taper.

    G76 P040060
    G76X.4392Z-1.735P0500Q.010F.05R-0.004



Page 1 of 2 12 LastLast

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