Programming an Angle using A on a Fanuc Controller
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Aug 2018
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    1

    Default Programming an Angle using A on a Fanuc Controller

    Can anyone explain to me how to program an angle using A? For example A135.0

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,872
    Post Thanks / Like
    Likes (Given)
    2311
    Likes (Received)
    2914

    Default

    G0 G90 A135.

    ?

    Program an angle for what? A probe routine, a G68 rotation XYR (R value not A for this), an angle on your 4th axis?

  3. #3
    Join Date
    Aug 2018
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    1

    Default

    Either an ID or OD angle turning on a lathe.

  4. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,872
    Post Thanks / Like
    Likes (Given)
    2311
    Likes (Received)
    2914

    Default

    Quote Originally Posted by ljeremy578 View Post
    Either an ID or OD angle turning on a lathe.
    You wouldn't use an A, you would do it using X and Z values....

    Maybe using conversational it is an A value, I don't know..?

    I am thinking longhand in CAM....

  5. #5
    Join Date
    Aug 2018
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    1

    Default

    I have seen it done just was curious how to do it personally. I know its been done with CAD.

  6. #6
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,915
    Post Thanks / Like
    Likes (Given)
    12760
    Likes (Received)
    4639

    Default

    Quote Originally Posted by Mike1974 View Post
    You wouldn't use an A, you would do it using X and Z values....

    Maybe using conversational it is an A value, I don't know..?

    I am thinking longhand in CAM....

    On my Mits, and I believe on the Fanucs that were on Citizens before the Mits, you can make a chamfer or an angle by specifying an A or C value, and the controller does the math.

    So you could:

    G1 X.240 F.002
    Z.500
    X.270A60

    and the control would calculate the Z endpoint to move X to .270 at a 60 degree angle

    G1 X.2 F.002
    G1 X.5 E.001, R.015

    The control moves to X.5 but automatically puts a .015R on the the .5 diameter. The E value gives the feedrate used during the G2, in case you want to slow down.

    You can use C in the same way as R to create a 45 degree chamfer of a specified size, automatically.

  7. Likes pcasanova liked this post
  8. #7
    Join Date
    Mar 2008
    Location
    vacaville ca
    Posts
    532
    Post Thanks / Like
    Likes (Given)
    79
    Likes (Received)
    144

    Default

    teachme is on it with the a movement, but machine in air first to make sure the angle goes the way you want. 0 on the compass may not be where you would assume.

  9. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,469
    Post Thanks / Like
    Likes (Given)
    989
    Likes (Received)
    3054

    Default

    There is an optional function called Direct Drawing Dimension Programming that allows combinations of X,Z,A,R values to be entered to define the profile. Never tried turning it on to see how it works. IIRC, the FAPT version controls output used that function. Seems like it could be handy if ones trig and geometry skills were a bit rusty.

  10. #9
    Join Date
    Jun 2016
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    240
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    107

    Default

    If I remember I manage to do it with a chamfer.

    1/32 chamfer 1" shaft:
    Blah blah
    G1 X.936 Z0.0
    G1 X1.00 A-45.0
    blah blah

  11. #10
    Join Date
    May 2005
    Location
    Ohio
    Posts
    426
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    120

    Default

    On my Nakamura I program using A like this..
    G0X1.Z.05
    G1Z-.458F.004
    X1.21, A105.
    Z-1.58

    This code is creating a 15° from vertical as the tool moves up in the X direction(0° is on centerline sticking out of the spindle, 90° is perpendicular to centerline, 180° is on centerline going towards the spindle, 235° would be a 45° going back towards centerline, etc...)

    It requires the comma after the X or Z command.
    I use A commands whenever I can... makes it easier to read the code afterwards.

  12. Likes ljeremy578 liked this post
  13. #11
    Join Date
    Nov 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I have a Nakamura WT150.
    Have a ''Y'' axis on the upper and life tool on upper and lower

    Now, I try to figure out how to use that kind of G-Code in my program that I do by hand.

    I ran that simple test just to see if my code was good.

    For any reason when I run that program I have an error that say ''57 no solution for block end''...
    So I don't know if the way I doing the code for the angle is not good or I need to activate something somewhere in the controler of the machine (Fanuc 18i-TB)

    Program :

    O0011(test with id statements)
    (10-12-2020)

    (UPPER TURRET PROGRAM)


    N1 M41(ROUGH TURN TURN_OD_ROUGH_1)
    G54
    (PLT-CNMG432-PR GR4315_C4)
    (UPPER TURRET)
    (MAIN SPINDLE)
    G28 U0
    G28 V0
    G28 W0
    M981 (SECURITY CHECK)
    G18
    G0 G40 G80 T1111
    G08 P1
    G99
    G50 S2500
    G96 S450 M3
    M07
    G0 X.5 Z0.0756
    G1 Z0 F.012
    Z-1.0,A165.0 F0.001
    X3.0
    G0 Z0.05
    M09
    G28 U0
    G28 V0
    G28 W0
    G08 P0
    M1

  14. #12
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,915
    Post Thanks / Like
    Likes (Given)
    12760
    Likes (Received)
    4639

    Default

    Try changing the angle to something simple like 90, see if it can calculate it then.

  15. #13
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,347
    Post Thanks / Like
    Likes (Given)
    752
    Likes (Received)
    568

    Default

    On Okuma OSP giving an "X" or "Z" target point and an "A" - the control will generate an angle. It's called "Auto Any-Angle" and it's standard on OSP. "0" degrees is 3: O'Clock, and it goes CCW from there.

    On Fanuc it's an option called something like "Direct Drawing Input" and I believe it works the same.

  16. #14
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,161
    Post Thanks / Like
    Likes (Given)
    645
    Likes (Received)
    656

    Default

    On some Fanucs, it is an option, but a lot of MTB provided it standard. But on some models a parameter controls how it is programmed. I remember needing a comma before the letter address. Like,C or ,R. I found the below graphic a Fanuc manual.

    optional-chamfer.jpg

  17. #15
    Join Date
    Aug 2008
    Location
    Philadelphia,PA
    Posts
    135
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    16

    Default

    Quote Originally Posted by DouglasJRizzo View Post
    On Okuma OSP giving an "X" or "Z" target point and an "A" - the control will generate an angle. It's called "Auto Any-Angle" and it's standard on OSP. "0" degrees is 3: O'Clock, and it goes CCW from there.

    On Fanuc it's an option called something like "Direct Drawing Input" and I believe it works the same.
    Is this working in minutes or degrees? I have an Okuma and this would be kind of slick. Wish I had known it. So going in the negative Z direction on a face if I wanted a 45 chamfer and I doing A 225 or 37.5 if we are going in minutes? (only asking because you said 3 o'clock as the start so I figured maybe we are using minutes.

  18. #16
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,469
    Post Thanks / Like
    Likes (Given)
    989
    Likes (Received)
    3054

    Default

    It is in degrees and CCW is positive from 0 at 3 o'clock.

  19. Likes EnginCycles liked this post
  20. #17
    Join Date
    Jun 2016
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    59
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    29

    Default

    Quote Originally Posted by EnginCycles View Post
    Is this working in minutes or degrees? I have an Okuma and this would be kind of slick. Wish I had known it. So going in the negative Z direction on a face if I wanted a 45 chamfer and I doing A 225 or 37.5 if we are going in minutes? (only asking because you said 3 o'clock as the start so I figured maybe we are using minutes.
    It's all done in degrees.
    If you want a 45 on the face to OD in the Z minus and X positive direction you would say A135.
    .....
    X.9 Z0.0
    Z-.1 A135 (from Z0 to Z-.1 (X is automatically calculated) you go at 135 degrees from straight out of the spindle being 0, vertical towards your upper turret being 90)
    Z-1
    .....


Tags for this Thread

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
  •