Fanuc control handling of IPM / IPR
Close
Login to Your Account
Likes Likes:  0
Results 1 to 8 of 8
  1. #1
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Fanuc control handling of IPM / IPR

    I normally work with Mastercam for lathe work, and all speeds post as IPR. I'm messing with Fusion 360 to see if it's feasible to use for turning. When I post with Fusion, all OD, face and ID work post with familiar IPR for speeds. When drilling however, it posts IPM, so my drill that I'm targetting for .005 IPR is posting with F3.5, the IPM calculation for my RPM.

    Oddly, the Fanuc controller handles it fine without specifying G94 and the effective feed is the .005IPR I need, the next toolpath moves as expected with the feed in IPR.

    Anyone know what is going on here? Just want to know for the sake of consistency. Below is the drilling op and the op before it:

    (CHAMFER OD)
    G99
    G97 S182 M4
    G0 Z0.405
    G0 X16.8
    G50 S800
    G96 S800 M4
    G0 Z0.0283
    G1 X15.456 F0.04
    Z0.0146
    X15.5891 Z-0.052 F0.013
    G0 X16.8
    Z0.405
    G97 S182 M4
    M1
    M9
    M5
    G0 X20. Z15.

    (2.375 DRILL THRU)
    M1
    T0404
    G54
    M8
    G98
    G97 S700 M3
    G0 X0. Z0.605
    G0 Z0.405
    Z0.1
    G1 Z-3.545 F3.5
    G0 Z0.405
    Z0.605
    M1
    M9
    M5
    G0 X20. Z15.

  2. #2
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    244
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    81

    Default

    Quote Originally Posted by Matt81 View Post
    Oddly, the Fanuc controller handles it fine without specifying G94 and the effective feed is the .005IPR I need, the next toolpath moves as expected with the feed in IPR.
    Unless you're using Fanuc Lathe G Code system B or C, why the need for G94 in a drilling cycle, or the worry that it has worked without it?

    Your post processor has handled the drilling move as a simple linear move (G1) with feed and a rapid (G0) retract. No big. Your G97 (Constant Spindle) and G98 (Feed per Minute) have all those ducks in a row for things to act as you need then to when the drill comes around. I guess just throw a G99 in there at the end of a tool or the beginning of the next tool to put the machine back into the default mode you like to be in.

    One suggestion relating to your code. You might want to get into the practice of using G53 for your safe area retracts. A little safer, (No pun intended) especially if you have an active work offset set somewhere. G53 will ignore all that. Just sayin.

    Dave
    Last edited by 13engines; 10-21-2019 at 12:11 PM. Reason: error in content

  3. #3
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,233
    Post Thanks / Like
    Likes (Given)
    5506
    Likes (Received)
    7943

    Default

    The G98 and G99 in your post are the G94 and G95 that you are used to in your mill.

    I have no clue why those are not the same tho?


    ------------------

    Think Snow Eh!
    Ox

  4. #4
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    33

    Default

    Just delete the G98 code from the drill operation (or change it to G99) and change the feed from F3.5 to 0.005.

  5. #5
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    83
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    33

    Default

    Quote Originally Posted by Ox View Post
    The G98 and G99 in your post are the G94 and G95 that you are used to in your mill.

    I have no clue why those are not the same tho?


    ------------------

    Think Snow Eh!
    Ox
    G98 and G99 are Fanuc System A, G94 and G95 are Fanuc system B. I run a lathe at work that uses G94 and G95 instead of the usual G98 and G99. It all depends how it's set in the parameters.

  6. #6
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    25,233
    Post Thanks / Like
    Likes (Given)
    5506
    Likes (Received)
    7943

    Default

    Quote Originally Posted by Fancuku View Post
    G98 and G99 are Fanuc System A, G94 and G95 are Fanuc system B. I run a lathe at work that uses G94 and G95 instead of the usual G98 and G99. It all depends how it's set in the parameters.
    I understand that, but I doubt he does, and I doubt that his machine is set that way as I am sure that yours is one of very few.


    ---------------------

    Think Snow Eh!
    Ox

  7. #7
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the responses. I showed it to my boss and he confirmed the G98 and G99 sets IPR and IPM. Regarding G53, the post processor was setup to use those, but I modified the post to output what you see there. I've never used G53, but reading into it, it does seem safer. We've had operators crash machines in the past when the code G0'd to home, after an offset was cleared, so the tool made a check mark shaped movement to head home while on the back side of a flange.

  8. #8
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    244
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    81

    Default

    Hello Matt81,

    Good to see you're looking into G53. In mill work, once the cutting is done and the tool has retracted to a clearance plain, you'll seldom get into trouble by programming a G53Y0Z0 to send the spindle home and bring the table forward for work piece change. On a lathe, it would not be uncommon to send the turret to a safe place with two lines of G53. Remember G53 is a "one shot" code and is effective only in the block it's present in. So on your lathe you might try:

    G53X0
    G53Z0

    Don't forget you can also include M codes in the same block to speed things up. For example:

    G53X0M9
    G53Z0M5

    The work area on my lathe is very tight, and a very usable and quicker to reach safe area is more like the following, which also stands clear of the 2nd spindle:

    G53X0.Z-7.5

    Good luck with it.

    Dave


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
  •