527,821 active members*
2,197 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > Fanuc 16i-MB on Robodrill - a couple of issues!
Results 1 to 7 of 7
  1. #1
    Registered
    Join Date
    Jul 2011
    Posts
    71

    Fanuc 16i-MB on Robodrill - a couple of issues!

    Hi All,

    I've recently acquired a Robodrill with a Fanuc 16i-MB controller and have already hit some problems. I have tried searching the forum, but can't quite find what I need or answers were sent via PM so I can't see the resolutions.

    Problem 1:
    Helical interpolation - I get the "Alarm 021 - illegal plane axis command" despite the format of the G2/G3 movement looking correct and G17 active. I see talk of this being either a missing option or just a parameter change and need to work out which is the case for me. All threads I could find on this ended in a secret pm!?

    Problem 2:
    Jerky movement is 3D surface machining - I need to use High Speed Machining (G05 I believe?), but the controller does not recognise it? Does this mean I don't have this option or just another parameter? How can I find out?

    Any help would be very much appreciated!

    Best Regards
    Aussie CNC

  2. #2
    Registered
    Join Date
    Jul 2011
    Posts
    71
    Ok, the 1st issue is fixed after a little more digging on here. Parameter 9930 bit #3 set to 1 fixes the problem. Why wouldn't they be setup like this from the factory??

    I found the following thread very useful:
    http://www.cnczone.com/forums/fanuc/...rameter-2.html

    Still struggling with the high speed machining function though, and I little more confused after more reading and testing:

    G05 P2 (high speed linear interpolation on)
    G05 P0 (function off)
    ..........This gives me "improper gcode" error, but cannot be used with circular interpolation anyway!?

    G05 P10000 (High Precision Contour Control)
    ..........This gives me "improper gcode" error!

    G05.1 Q1 (Al contour control/nano contour ON)
    G05.1 Q0 (function OFF)
    ..........This gives me the same "improper gcode" error

    G05.4 Q1 (High Speed HRV function ON)
    G05.4 Q0 (function OFF)
    ..........This runs, but makes little difference?

    G08 P1 (Advanced Preview Control ON)
    G08 P0 (function OFF)
    ..........This runs, but makes little difference?

    Anyone doing any high speed cutting on a Robodrill that can share their experience?

  3. #3
    Gold Member
    Join Date
    Aug 2011
    Posts
    2517
    if you read the top sticky thread 'GE Fanuc & FANUC proprietary posts' you will see it's not a good idea to post option parameters on this forum and the administrator does not like it.

    as for 'why would they be set up like this from the factory'........... options are, well, ......... optional. If you want something extra the option needs to be purchased from Fanuc. Your machine simply does not have those options which results in the improper g-code alarm(s).

    This thread will probably end in a secret PM also ;-)

  4. #4
    Registered
    Join Date
    Jul 2011
    Posts
    71
    Hi,
    Thanks for your reply. I guessed HSM would be an option but not helical interpolation, and as I bought this machine second hand, I have no idea of which options it should have!? It seems I can't edit my post to remove the parameter details!? Can an administrator remove anything they feel I shouldn't have posted please?

    At this stage I'd just like to know the solution to my HSM issues, as in which G05 or other code someone else is using and whether I need to investigate the purchase of that option!?

    I suppose I could be asking too much, but I have seen similar slow/jerky movements solved on other machines (eg Haas, Okuma etc) with the use of a HSM option!?

  5. #5
    Gold Member
    Join Date
    Aug 2011
    Posts
    2517
    On Fanuc pretty much everything is an option. Even the manual pulse generator is an option. Of course there are many things required for basic operation and those are provided at the factory. Helical Interpolation is generally not provided unless requested. Same for High Speed Machining. I'll send you a secret PM...... ;-)

  6. #6
    Registered
    Join Date
    Jul 2011
    Posts
    71
    A quick update for those that may search later.....

    G05.1 Q1 gave me what I was looking for, but the twist is that you have to turn this on before Tool Length Comp (G43).
    The format I found worked for me was:

    G91 G28 Z0
    G90
    N1 T12 M6 (12.0 MM DIA MILL)
    G90 G40
    S10000 M3
    G54 G0 X-7.838 Y-11.152
    G05.1 Q1
    G43 H12 Z10.
    G0 Z2.
    G1 Z-1. F1000
    X-2.182 Y-5.495 F2000
    X5.495 Y2.182
    ....
    cutting
    ....
    G05.1 Q0
    G28 G91 Z0
    G28 G91 X0 Y0
    G90
    M05
    M09
    M30

    Hope this helps someone else at some point!

  7. #7

    Re: Fanuc 16i-MB on Robodrill - a couple of issues!

    Hi fordav11 you can help me ?

    I have same problem abot High Speed G5.1. I use Robodrill with a Fanuc 16i-MB controller.
    Cam 3d does some F cut to F8, I set it to F1000.
    Most of the time that f decreases in the arc.
    What parts of the parameters can I modify?
    I am using Robodrill T14ia control 16ima.

    Thanks.

    picture https://ibb.co/nc3SLHK

Similar Threads

  1. Replies: 1
    Last Post: 04-14-2014, 07:41 PM
  2. Couple issues with new SS install...
    By mcphill in forum SmoothStepper Motion Control
    Replies: 9
    Last Post: 02-14-2012, 02:03 AM
  3. Having a couple of issues that need solving
    By strohkirchw in forum Taig Mills / Lathes
    Replies: 0
    Last Post: 03-10-2011, 05:37 AM
  4. Couple startup issues, and some resolutions
    By mcphill in forum Mikinimech
    Replies: 12
    Last Post: 11-15-2010, 06:25 AM
  5. FANUC ROBODRILL NEED HELP
    By WJ MARK in forum Fanuc
    Replies: 4
    Last Post: 01-01-2010, 09:31 AM

Tags for this Thread

Posting Permissions

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