584,846 active members*
4,202 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Uncategorised CAM Discussion > Fanuc 0T Stock Removal Cycles
Results 1 to 5 of 5
  1. #1
    Join Date
    Oct 2003
    Posts
    38

    Fanuc 0T Stock Removal Cycles

    I machine a lot of these forgings as shown in the picture (See Attachment).

    I use a G72 to machine the face down to size and a G71 to rough the shaft and put the front angle on. But we have to dig the profile out long-hand and it's line after line after sodding line of programming which is tedious to write aswell as time consuming.

    Does anyone know of a canned cycle to cut a profile into a long shaft. I know there's a grooving cycle but it will only do straight line whereas we need a profile with a few radii in.
    Attached Thumbnails Attached Thumbnails weldoflange.gif  

  2. #2
    Join Date
    Oct 2003
    Posts
    263
    Have you tried just continuing the profile definition in your G71 cycle? I've done lots of profiling that way with G71 (Fanuc) or G85 (Okuma 2200 or 3000) cycles.

    Or, if the tool that faces the end and turns the angle won't clear down in the profile, you could call up a separate tool (VNMG, DNMG, etc) to rough it out with a G71 cycle.

    The G71 would cut a lot of air on some forgings. I think there's a separate cycle for stock removal on forgings/castings, but I haven't used it. The G86 cycle on older Okumas did that, but I seldom found it very efficient. Used to result in a really wide chip that didn't break well and kept the coolant off the tool.

    G71 is better suited to solid bar, but sometimes a little air cutting is an ok tradeoff.

  3. #3
    Join Date
    Jun 2003
    Posts
    205

    Try G73 - Pattern Repeating

    You may want to try the G73 cycle - Pattern Repeating -- This cycle is designed for cast shapes and basically repeats the contour shape as it brings the "rough" stock to finish dimension.

    Here's a long explanation from our Protalk - CNC Programming Training & Reference Software - Hope it helps.

    The G73 cycle is used to remove rough stock on part shapes where the material to be removed is not in a bar or solid shape. This cycle is most often used for machining casting type rough stock where the best way to remove the rough material is to simply follow the part shape and keep bringing the tool in step by step. By commanding the G73 cycle and then programming the finish part shape, rough cutting shape will be automatically calculated and executed by the control. Rough cutting depth of cut, feedrate and amount of finish stock to leave can all be commanded, and therefore easily altered, using the G73 cycle.

    The command block for a G73 cycle is :

    G73 Pxxx Qxxx Uxxx Wxxx Ixxx Kxxx Dxxx Fxxx ;

    P = Sequence (N) number of the first block of the finish shape program.

    Q = Sequence (N) number of the last block of the finish shape program.

    U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
    programming ).

    W = Amount and direction of the finish allowance in the Z axis.

    I = Amount and direction of the rough stock in the X axis (radius value)

    K = Amount and direction of the rough stock in the Z axis.

    Note : It is possible to have a different amount to remove from the diameter than the faces in this cycle by commanding a different value in the I an K command.

    D = # of cuts to take in removing the rough material.

    F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.

    Option :S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

    When the above G73 format is commanded, the control looks between the sequence numbers P and Q and looks at the desired finish shape. It then calculates and executes roughing passes to rough the material from that finish shape by repeating the finish shape for the D number of times. The control takes the I and K removal amounts, divides that by the D number of cuts, and then determines the depth of each cut independently for the X and Z axis. No semi-finish pass is done in this cycle as in G71 and G72 but it does leaving the U and W values for the finish pass. No finishing is executed and either a finishing pass must be programmed or the G70 (finishing cycle) must be commanded.

    Good Luck
    Real world Machine Shop Software at
    www.KentechInc.com

  4. #4
    Join Date
    Oct 2003
    Posts
    38
    Thanks mate but i don't think the G73 will work. It is a forging but its not shaped, its just a flat long shaft coz we can make like 10 different components from one type of forging. Thats why they're not shaped.

    I may try the but i'm not sure that will work either. Cant believe fanuc haven't put this in their systems yet

  5. #5
    Join Date
    Oct 2003
    Posts
    263
    Look at this. It's been a few years since I've used these cycles, but this looks pretty familiar to me. No attemptt made to allow for some of the realities of machining - just a simple format.

    If it's not legible on your screen, you can download it:

    http://bellsouthpwp.net/r/s/rsnmar/G71.png
    Attached Thumbnails Attached Thumbnails g71.png  

Similar Threads

  1. Fanuc 3M DNC operation
    By max_c in forum Uncategorised MetalWorking Machines
    Replies: 3
    Last Post: 07-05-2010, 01:11 AM
  2. Fanuc motor ???
    By jevs in forum Servo Motors / Drives
    Replies: 3
    Last Post: 03-16-2005, 11:47 PM
  3. Fanuc 0-2000M motor ??
    By jevs in forum Servo Motors / Drives
    Replies: 6
    Last Post: 02-18-2005, 08:46 PM
  4. head stock and tail stock chucks
    By mocnc in forum DIY CNC Router Table Machines
    Replies: 3
    Last Post: 10-20-2004, 03:16 AM
  5. FANUC coding compatability??
    By m1911bldr in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 3
    Last Post: 04-24-2004, 11:10 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
  •