Results 1 to 7 of 7
  1. #1
    rfrink's Avatar
    rfrink is offline Cast Iron
    Join Date
    Nov 2005
    Location
    Ohio
    Posts
    290

    Post

    In a turning center, I'm trying to use G76 for the first time to cut 3/4-16 ID threads following an 11/16" drill.

    I don't understand a few things in the Fanuc OT manual:

    G76 P(m,r,a,) Q(dd-min)R(d)
    G76X(u) Z(w) R(i) P(k) Q(dd) F(L)

    There is an example in the manual written in mm. In the first line, I don't understand Q(dd-min) it cannot have a decimal...? Same with R(d)....?

    I think I understand the second line...

    Hmmmm....I think if a see and example written in "inches" it might help me.

    Can any one help?

    My control is a Fanuc OT


    edit: this is what I have so far: it stops with a p/s 007 alarm "illegal use of decimal point

    ...
    G76 P021060 Q.005 R.0005
    G76X.750 Z3.5 P.0338 Q.008 F.0625
    G28U0.W0.
    ..
    ..
    ...

  2. #2
    HuFlungDung is offline Diamond
    Join Date
    Jan 2005
    Location
    Canada
    Posts
    6,604

    Post

    Not sure, but I think the Q might be a degree offset angle for a multistart thread, so you would likely want that to be zero, until you started the second thread of a multi-start thread.

  3. #3
    mrainey's Avatar
    mrainey is offline Stainless
    Join Date
    Jul 2004
    Location
    Spartanburg, South Carolina
    Posts
    1,500

    Post

    I found this article at http://www.machinerynet.com/index.cf...rs=0&artid=171

    There are a lot more like this one.


    Conversion of Lathe Cycles

    Publish Date - 06/01/2005
    Source: Shop Talk Magazine
    Column: CAD/CAM and Related Software Packages

    By Peter Smid


    Email this to a friend
    Printer Friendly

    Most CNC lathe programmers would agree that the most useful features of a CNC lathe control system are the Multiple Repetitive Cycles. Multiple repetitive cycles for CNC lathes have been an important part of control systems since the mid 1980s. Still, to this day, they present the most innovative approach of material removal, particularly in the areas of turning, boring, and threading. Over the 20-plus years of their existence, multiple repetitive cycles have gone through only two major changes. Earlier controls require these cycles to be programmed in a single block; later controls require two blocks of program input. This difference in programming method often presents a situation when one type has to be converted to another type—usually from a single-block format to the double-block format.

    At the beginning, lets look at the word convert. Changing from one format to another is not a true conversion or, at least, it is not a complete conversion. The reason is that a double-block format offers more features than a single-block format. Also, keep in mind that you have no choice here; the control system determines the programming method. Typically, Fanuc control models 10/11/15 use a single-block format, other control models (0/16/18/20/21..) use the double-block format. What cycles are affected? All multiple repetitive cycles from G71 to G76 can be programmed in one or the other format, depending on the control. The finishing cycle G70 always uses a single-block format.

    The single-block format is older of the two, and relies heavily on the settings of system parameters, generally inaccessible to the machine operator. I will use the most commonly used G71 and G76 cycles as examples in this column, other cycles follow a similar pattern. The single-block format of the roughing cycle G71 is:

    G71 P.. Q.. U.. W.. D.. F..

    In this single-block format (spindle speed is assumed to be in effect), P and Q addresses refer to the block numbers defining the finish contour. U and W are specifications of stock amount left over for finishing, D address is the depth of cut (written without a decimal point), and the F address is the roughing feedrate. In addition, some controls also accept I and K addresses that control the distance and direction of semi-finishing.

    For controls requiring a two-block format, the G71 must be written at the beginning of each consecutive block:

    G71 U.. R..

    G71 P.. Q.. U.. W.. F..

    The programmed data are similar, but a bit more flexible. In the first block, the U address is the cutting depth (decimal point can be programmed), and the R address is the amount of retract from each cut. The second block has the same meaning as before—finish contour block number range P and Q, stock allowances U and W, and feedrate F. Apart from the more convenient way of programming the cutting depth, the addition of the R address represents the major change. In a single-block format, the retraction amount was controlled by a system parameter, in the double-block format, the programmer can specify such amount in the program directly.

    Even more profound change can be found in the threading cycle G76. In its single-block format, the cycle uses the following data:

    G76 X.. Z.. I.. K.. D.. A.. F..

    In this case, the X specifies the final thread diameter, Z is the position of the thread end, I specifies the amount of taper (if used), K is the thread depth, D is the depth of the first pass, A is the thread angle, and F is the thread lead (feedrate). The two-block version packs in a few more programmable features:

    G76 P.. Q.. R..

    G76 X.. Z.. R.. P.. Q.. F..

    The P address in the first block includes the number of finishing passes, length of lead for pullout at the thread end, and the thread angle all in one. The Q address specifies the minimum cutting depth, and R is the finish allowance. In the second block, X and Z are the same as before, R specifies the amount of taper (if used), P is the thread depth, Q is the depth of the first pass, and F is the thread lead (feedrate). Neither P nor Q in the second block accept a decimal point.

    As you see from the two examples, the main difference between the two cycle formats is the additional programmable parameters which make the cycles much more flexible than using internal parameter settings. In either double-block cycle, do not confuse the addresses in the first block with the same addresses in the second block. As you see, the conversion from a single-block format to a double-block adds certain features that are now programmable, offering more flexibility to the CNC programmer.

  4. #4
    nomgis is offline Cast Iron
    Join Date
    Dec 2005
    Location
    chicago
    Posts
    260

    Post

    Your code should read like this
    G76 P021060 Q0050 R.005
    G76 X.75 Z3.5 P0338 Q0080 F.0625
    No decimel on Q first line same on first P and first Q second line

  5. #5
    rfrink's Avatar
    rfrink is offline Cast Iron
    Join Date
    Nov 2005
    Location
    Ohio
    Posts
    290

    Post

    Sincere thanks Guys!!! Yep..it was the decimal points. I found another online discussion about the same topic and they clearly explained how to write dimensions w/o decimal points.

    .100 = 1000
    .010=100
    .001=1


    something like that...

    anyway, I got ran the aprts ..they look great...now I'm off to the next million dollar idea...


    Thanks again,
    Rob

  6. #6
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,874

    Post

    One of my machines uses 5 places right of the decimal point.

    Think Snow Eh!
    Ox

  7. #7
    MarkT is offline Aluminum
    Join Date
    Mar 2006
    Location
    USA
    Posts
    60

    Post

    Some controls provide for five places to the right within the feed command to allow for the most accurate thread possible when threading over long lengths in the "Z" axis. Minimizing natural rounding which would occur with 4 place to the right programming methods.
    Mark T

Bookmarks

Posting Permissions

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