584,830 active members*
5,676 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Milltronics > Tool Setter M Codes! For Centurion 5, and probably 6 and 7.
Results 1 to 7 of 7
  1. #1
    Join Date
    Jun 2010
    Posts
    116

    Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Ever since I got my Partner 1D with a Centurion 5 controller I've hated the way you have to set tools and part Z zero, it never made sense and if the top of your part gets removed you're screwed if you have to re-set a tool. I come from Fanuc machines with M codes to set tool length and part height. I spent the past few days finding all the Parameter locations, etc... and created my own! I figured I'd share since I've seen a bunch of posts from others who have the same issues with it as me. The attached files will allow you to set the tool setter zero height (M52), set the tool length from the gauge line of the spindle (M50) and set G54 Z from any tool (M51).

    All you have to do is activate level 3, parameters, setup, PROTO3, Level 3. Then go to MISC parameters, page down to the Custom M Codes and set O9025 to M52, O9026 to M50 and O9027 to M51. If you are already using those programs or M codes just change the program name and/or set that program to whatever M code you need. When done go back to Level 1.

    Once you've set the M Codes do the following:
    To set the tool setter you have to bring the spindle with no tool in it down on the tool setter until it reads Zero. I'm talking about the flange on the bottom of the spindle. Once it is at zero type M52 in MDI and press start. It will update an unused parameter to the machine Z position of the tool setter zero.
    I'm not sure how to incorporate a number after the M code into a program to allow for using a gauge block between the spindle and tool setter so I made a little program to do it. Open program O1000 and change where it says (PUT GAUGE BLOCK HEIGHT HERE) to the gauge block height. Then run that program after you have set your Z zero on the setter. If you don't use a gauge block ignore this part.

    Once you have done that you can set tools on your tool setter by bring the tool down on it to zero and type M50 in MDI. This sets the actual tool length from the spindle gauge line.

    Once the tools are set you can set G54 Z by bringing a tool down to the part like normal. Then, in MDI, enter M51 and Start to set your offset. This is the distance from machine zero.

    FYI, if you have to modify one of the M code programs for whatever reason you have to reboot the machine after you save it or the M code will not use the new program. It seems that on boot the controller puts those programs into RAM and will not refresh them until you reboot. Also, if you didn't already know, User Parameters P0-P99 are reset to 0 on boot. Some of the others as well, that's why I had to use an unused protected Parameter for the tool setter zero.

    I hope this helps everyone out. If you find any bugs or issues please let me know. They all worked correctly on my machine, but I don't have a 6 or 7 controller to test them on.

    Mike Roth.

  2. #2
    Join Date
    Jun 2010
    Posts
    116

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    I'm curious if anyone has tried this yet and if so what you think?

    Thanks,
    Mike

    Sent from my LG-H830 using Tapatalk

  3. #3
    Join Date
    Jun 2010
    Posts
    116

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Thought I'd leave an update on this. I've been using it for over a month now and it is working great. I haven't had a single issue.

    Mike

  4. #4
    Join Date
    Jul 2010
    Posts
    548

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Hi Mike, That just goes to show you how "powerful" the Milltronics control is. There are so many ways to make it "Your way". No other control can make it that way. Milltronics view is OK, we will start with "this" but HEY there is more the one way to "skin a cat". Check out the parametric programming options. The world it "now wide open".

    The NEW 9000 control is ever MORE SO.

    It's why WE love them.

    I like that you are exploring the "well" it's this way on this, Why can't I do ???? you are finding there is a way. And, you are letting others know what you find,,it expands that "knowledge base" .

    Thy this kind of stuff on any other control and see what you get. ( road block, ,after road block, after road block.)

    Milltronics, ya gota love it.


    Mike, Keep on exploring and keep on telling "us" what you find,. It helps all concerned, Because you never know when ,you have solved a problem, someone else has be "chasing the "how do I"

    Also, don't be afraid to ask the form, "how can do ????"

    The one thing I'm not sure if "we" can make it do is " Heard cats" ; - 0


    Sportybob

  5. #5
    Join Date
    Jun 2010
    Posts
    116

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Thanks SportyBob! Overall I really am liking this control so far. I love how easy it is to do things like it did. Main thing I would like if it did is display more than just the current line of code, tech support said you can't with this version though. Would be nice to see the position from machine zero too.
    Thanks again,

    Mike

  6. #6
    Join Date
    Jul 2010
    Posts
    548

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Hi Mike, If you go to display and select distance, it will show 5 lines of code. ( newer software will show more. moves)
    In Graphics it will only show the "current" "move". on the MDI line. So, it is a "choice: between seeing the "M&G code on the screen or the graphics of what the control is "doing"
    Graphics has the options, of , zoom , window, pan, tilt, rotate. ( newer software is faster, with these options.) You get to a point in software ~ version X.119 and the control processor REALLY starts to make a difference for display functions. not so much for the cutting capabilities as you can only cut a material so fast. ( It's the spindle speed and feed thing)

    Newer software also offers ALOT of conversational programming functions.
    If you are doing Cad/Cam programming, maybe some additional parts storage. would be available with a SBC ( single board computer) update.

    Again, distance will show the "value" from home. or look at the G5X ( 4-9) value and you will see the machine "off set" from home.

    Sportybob

  7. #7
    Join Date
    Jun 2013
    Posts
    36

    Re: Tool Setter M Codes! For Centurion 5, and probably 6 and 7.

    Thanks for the tips Mike. You inspired me to work on my own macro program. I've got a couple things sorted out, but I'm still not able to get a custom M code to work for some reason. I've got a Macro program now for:

    Offsetting Tool Lengths
    Offsetting WCS
    Using an edge finder to Set X/Y or store the number in a parameter
    Calculate center between two points and set a WCS
    Set WCS Z using the active tools length similar to your macro
    Setting tool lengths
    Driving the tool over to the gage
    Calibrating the gage position


    For the most part, the macro calls work a lot like a Fanuc.
    I'm able to call a program using a G65 and pass variables to it with letter words.

    For example: G65 P9028 S10 X.2 W1
    Will execute program 9028 and set parameters P19=10, P24=2, and P26=1

    This is another way you could possibly add a gage length to your Macro.


    However, I put 055 in the 9028 custom m code section under the Power settings and it doesn't seem to work for some reason. I can call my program with the G65, but M55 isn't working. I cycled power but still nothing. Looking in the programming manual it says it should work in the Parts directory, did you have to put your programs somewhere else to get them to work with the M codes?


    Also, does anyone know of a way you can use variables for system parameters or GOTO statements?

    P418 will work for WCS2 X
    P[412+6] - Does not work

    Also,
    P1=10
    GOTO P1 - Does not work

    This is slightly annoying, I was able to do what I wanted by adding more labels and logic, but if anyone knows a way to use variables like this that would be awesome!


    Thanks,
    -Steve
    Attached Files Attached Files

Similar Threads

  1. Replies: 1
    Last Post: 03-04-2014, 01:08 AM
  2. Tool Length Offset Tool Setter
    By CNCneeds in forum News Announcements
    Replies: 0
    Last Post: 01-03-2014, 06:27 PM
  3. Tool Setter Macro for M-V60C and Metrol Setter
    By mitshack in forum Mazak, Mitsubishi, Mazatrol
    Replies: 1
    Last Post: 02-02-2013, 12:08 PM
  4. Tool setter macro for M-V60C and Metrol setter
    By mitshack in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 0
    Last Post: 10-06-2008, 02:38 PM
  5. Centurion 5 vs. Centurion 6 and validation codes
    By Turbo VW in forum Milltronics
    Replies: 2
    Last Post: 02-11-2007, 09:35 PM

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
  •