584,812 active members*
5,312 visitors online*
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > What secret options in an OMD control system, helix?
Page 1 of 2 12
Results 1 to 20 of 40
  1. #1
    Join Date
    Sep 2010
    Posts
    34

    What secret options in an OMD control system, helix?

    Hi Guys,
    I'm new here obviously. I am completely new to CNC machines so I am incredibly pleased to find a site with so many helpful people and so much knowledge.

    I have a Kent bed mill with a Fanuc OMD control system that I run from Dolphin CAD/CAM. I think I will need a memory upgrade because the Dolphin CAM produces masses of code for any helical move.

    Because of my memory problem I was interested in the posts concerning upgrades and "optional" modes that are built into the Fanuc control system. Is there likely to be any helical options on my control system that could be turned on? Does anyone know what options are asleep in the control system or is this totally maker dependent? In view of the age of the control system can I still get the options activated?

    Thanks, Brian

  2. #2
    Join Date
    Dec 2003
    Posts
    24216
    The Helical can be turned on by parameter but you also need the spindle encoder and spindle controller capable of using the feature.
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  3. #3
    Join Date
    Sep 2010
    Posts
    34
    Thanks Al.
    The machine has a notched belt drive from the VFD motor to the pulley/spline assembly.
    There are no connections to the spindle cartridge or the pulley assembly that I have seen. There are some extra wires going into the VFD motor that I have not identified (no circuit diagram).

    Does the spindle controller card need to know a simple rotation count (ie 1 pulse per rotation) or does it need to know exact spindle angular position?


    No point in getting excited about options if I do not have the hardware. I will investigate further thanks.
    Brian

  4. #4
    Join Date
    Dec 2003
    Posts
    24216
    In most commercial CNC's with this capability there is feedback from motor to Spindle controller or VFD etc, and also an encoder on the final spindle shaft, this encoder is used to gear the Z axis motor off it, for tapping or helical operation.
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  5. #5
    Join Date
    Sep 2010
    Posts
    34
    Al, hope you see this

    I am lucky in that I have a complete set of manuals with my machine. The Fanuc "Operations" and "Maintenance" manuals plus the "Manufacturers" manual.

    I checked my machine. it is fitted with a A16B-2201-0103 memory card that includes connector M27. The book shows some sort of spindle control on the memory card and also shows M27 connecting directly to something called a "Position Encoder" apparently attached to the spindle intermediate drive (on my machine where the belt pulley adapts to the spindle splined shaft). The card diagram says this is an "analog" spindle arrangement.

    A further nearby diagram showing pin connections titled "Position Coder Interface" shows M27 connecting to a unit called the "Position Coder". There is no part number on the position coder block.

    It looks to me that if I can find a "Position Coder" and a suitable cable then I can get my mill operational in true helical movement (after paying Fanuc's extortion). The manufacturers manual actually lists G codes 33 and 95 in their g-code list.

    Thanks for the info provided so far.

    Brian

  6. #6
    Join Date
    Dec 2003
    Posts
    24216
    The encoder is a standard differential encoder, IIRC the resolution is 1000cts/rev, I will see if I have the info.
    The other information I sent you may not require Fanuc getting involved.
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  7. #7
    Join Date
    Mar 2003
    Posts
    2932
    Quote Originally Posted by Al_The_Man View Post
    The Helical can be turned on by parameter but you also need the spindle encoder and spindle controller capable of using the feature.
    Al.
    Just curious, Al.

    Why would he need a spindle encoder for helical interpolation? It's just 3-axis milling, isn't it? I understand if he wanted rigid tapping, but I could swear I've done helical on old Matsuura's that didn't have spindle encoders.

    Please enlighten me, o Swami...

  8. #8
    Join Date
    Dec 2003
    Posts
    24216
    Yes your right of course, For the last few weeks I have been working on writing a threading routine for a lathe and somehow it given me a brain freeze.
    Thats my excuse anyway.
    Helical milling involves 3 XYZ axis interpolation overall.
    So Brian, you may be able to get away with the info already supplied!!
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  9. #9
    Join Date
    Sep 2010
    Posts
    34
    dcoupar

    I'm new at this but my original need was to reduce the amount of code generated by my CAM program for threadmilling. Someone was kind enough to write a sample threadmill example for me and the threading part of the program took 3/4 of the code yet most of the actual work was contained in the first quarter. Since the helical interpolation would be built into the CNC I am imagining that the amount of code required to threadmill would be much reduced. Would this be correct?

    If helical would help me out I am really interested in this since my present project involves cutting a couple of largish diameter none-standard threads to match the threads on parts made by suppliers so I am focused on threadmilling right now. A memory upgrade is in the future also.

    Actually my original question was more generic. I was just wondering how many options there were on the OMD control since I have never seen these mentioned until I joined this forum and there is no information in my manuals.

    Learning as much as I can about codes and machines is great in itself.

    Brian


    .

    edited for crossing posts.

    Thanks Al, the more I learn the better.

  10. #10
    Join Date
    Mar 2003
    Posts
    2932
    Brian,

    Yes, helical interpolation will give you much smaller programs than a bunch of linear moves approximating a helix.

    Just out of curiosity, have you tried to MDI in a helical move? Position XYZ in the middle of the travel, then execute the following in MDI.

    M03 S200;
    G3 G91 X1. Y1. J1. Z0.5 F20.;

    See what happens when you hit cycle start. If you don't get an "Invalid G-code" alarm, then the helical interpolation option is probably turned on. Let us know.

    There are dozens of options in the control that you probably won't see much about here because the owner of CNC Zone has asked that we not post proprietary information (such as Fanuc options) on the site. This was "suggested" by Fanuc's lawyers.

    Dave

  11. #11
    Join Date
    Mar 2003
    Posts
    2932
    Quote Originally Posted by Al_The_Man View Post
    Yes your right of course, For the last few weeks I have been working on writing a threading routine for a lathe and somehow it given me a brain freeze.
    Thats my excuse anyway.
    Helical milling involves 3 XYZ axis interpolation overall.
    So Brian, you may be able to get away with the info already supplied!!
    Al.
    Al,

    Brain freeze? You? I doubt it. Brain fatigue, maybe. My suggestion is that we should all take Fridays off from now on.

    Dave

  12. #12
    Join Date
    Sep 2010
    Posts
    34
    I am not trying to dodge Fanuc's control. I was just wandering what options there may available be that I did not know about. Not making this information easily available is a bit like having a retail store and never unlocking the door so potential customers can see what you have for sale. I have the full OMD manuals, Fanuc and manufacturer, and none of them mention available options.

    Dcoupar, I will try your suggestion. Since I bought my mill used I have no idea what options may be on or off.

    Does Fanuc still support options for a 2000 machine?

    By the way - Fridays are "off", that's the day to play with my new toy

  13. #13
    Join Date
    Dec 2003
    Posts
    24216
    Quote Originally Posted by dcoupar View Post
    . My suggestion is that we should all take Fridays off from now on.

    Dave
    Is today Friday??
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  14. #14
    Join Date
    Mar 2003
    Posts
    2932
    Quote Originally Posted by Al_The_Man View Post
    Is today Friday??

    Yes, it's Friday. Take the rest of the weekend off and recharge.

  15. #15
    Join Date
    Sep 2010
    Posts
    34
    Well Dcoupar,

    I ran your little piece of code and there was no warning and the position display showed a very satisfactory 3 axis movement. I guess I have helical after all - now I need to learn how to use it.

    Since we have touched on the subject could someone please explain briefly the difference in machine operation between having helical active in the parameters and having the hardware option we have previously discussed? What will one do that the other will not do?

    Thanks to both Al and Dcoupar. It has been a good Friday for me.

    Brian

  16. #16
    Join Date
    Dec 2003
    Posts
    24216
    With the helical option, everything should be in place, hardware wise, so you probably have the option in the 900 parameters.
    Hopefully you have all the parameters backed up, including the 900's?.
    You can print them out to a hard copy if you have them in a file.
    The other hardware option you mentioned involving a spindle encoder will give you rigid tapping and synchronous feed, it can also give position orientation in the case of auto tool changer.
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

  17. #17
    Join Date
    Sep 2010
    Posts
    34
    Thanks Al,

    I just got the RS232 working recently so I have not backed everything up yet. I realize that that is the first thing I should have done but I have to read up on how to do this.

    I have been reading all the information I could get and it appears that I need a parameter change to back up the 9000 series parameters. I have looked at the parameter list in my control unit and I can see 8000 parameters but no 9000 parameters. I am thinking that these will probably pop into view when I change the access parameter.

    Another website post says that for the OMD I should change parameter 10 by changing bit(4) to a zero while I do the backup. I will try this by daylight and try to backup ALL parameters to the old laptop that I am using as a file server (had to go back about three generations of laptop computers to find one with an RS232 port !!!!)

    This 9000 backup looks pretty important since I see that a lot of people have got into deep trouble when they lost these parameters. Seems strange that vital operating information cannot be backed up easily. This also makes me think that I should carry out a parameter backup battery change.

    Thanks again.

    PS I see that you refer to 900 parameters. I can see 900 parameters in my parameter list but no 9000 parameters. Do I have 900 parameters or 9000 parameters on the OMD?

  18. #18
    Join Date
    Mar 2003
    Posts
    2932
    Brian,

    Be very careful what buttons you push at this point.

    On the 0M-D, setting parameter 10 bit 4 to 0 unlocks the 9000 PROGRAMS (O9000-O9999) so you can edit them, delete them, punch them out, etc. It has nothing to do with backing up parameters.

    Some builders use macro programs for tool change, etc. For example, if you wanted the M06 in the program to call macro O9020 (which would stop and orient the spindle, return Z to home, execute another M06 to put the next tool in the spindle...) you would set parameter 0230 to 06.

    0230 specifies m-code that calls O9020
    0231 specifies m-code that calls O9021
    ...
    ...
    0239 specifies m-code that calls O9029

    So, when you're ready to punch out your programs for backup, you should set parameter 10 bit 4 to 0, punch out all programs, then immediately set that parameter back to 1 so any macro programs stored in the control can't be edited or deleted accidentally.

    If you have 0230 set to 06 and someone has deleted O9020, when you try to run an M06 in your program, you'll get an 078 "NUMBER NOT FOUND" alarm.

    As Al said your parameters should be backed up (immediately, if not sooner), and that file should be saved somewhere secure. The option parameters are in the 900's to 915's (maybe higher). I believe these have to be entered manually if you ever lose all your parameters, so printing them out makes sense, too.

    And don't, under any circumstances change the option parameters unless you know what you're changing. I've had at least one customer who completely disabled his machine by changing the wrong option parameter.

    Anyway, glad Friday was good for you.

    Dave

  19. #19
    Join Date
    Mar 2003
    Posts
    2932
    Brian,

    Let's say you want to thread mill a 2"-12 thread 1" deep at X0 Y0, using a 3/4" shank 12-pitch thread mill that has 0.827 depth of cut

    http://www.stellram.com/Milling/Thre...MITMX21ENI.PDF

    This will take 2 depth passes due to the depth of the thread being greater than the max cutting depth of the inserts. I use G91 for the helical so I can do the same thread at any XY location on the part. Here's one example:

    %
    O1001 (THREAD MILL 2.00-18)
    (SET D53 TO 0.375)
    G00 G91 G28 Z0
    T03 M06 (0.750 DIA 12-P THREAD MILL)
    G00 G54 G90 X0 Y0 S2000 M03 (POSITION TO CENTER OF HOLE)
    G43 Z0.1 H03 M08
    G01 Z-0.5 F100. (FEED TO FIRST PASS DEPTH)
    G41 G91 X1.0 F10. D53 (FEED TO OD OF THREAD & TURN ON CRC)
    G03 I-1.0 Z0.08333 (1 REVOLUTION)
    G01 G40 X-1.0 (FEED BACK TO CENTER)
    G90 Z-1.0 (FEED TO SECOND PASS DEPTH)
    G41 G91 X1.0 F10. D53 (FEED TO OD OF THREAD & TURN ON CRC)
    G03 I-1.0 Z0.08333 (1 REVOLUTION)
    G01 G40 X-1.0 (FEED BACK TO CENTER)
    G00 G90 Z0.1 M09 (RETRACT OUT OF HOLE)
    G91 G28 Z0 M05
    G90
    M30
    %

  20. #20
    Join Date
    Dec 2003
    Posts
    24216
    This is how to back up and load 900's included.
    Al.
    Attached Files Attached Files
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

Page 1 of 2 12

Similar Threads

  1. Secret to plastic?
    By Crawler374 in forum DIY CNC Router Table Machines
    Replies: 6
    Last Post: 01-25-2010, 02:21 AM
  2. Replies: 2
    Last Post: 01-30-2009, 06:35 PM
  3. Servo system questions options abound
    By forgedcu in forum CNC Machine Related Electronics
    Replies: 0
    Last Post: 01-15-2008, 03:18 PM
  4. Control options for hexapod?
    By punisher454 in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 2
    Last Post: 01-08-2007, 02:00 AM

Posting Permissions

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