Is Brother speedio tool load monitoring possible?
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Jan 2012
    Location
    Tampa, FL usa
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Is Brother speedio tool load monitoring possible?

    Got our first brother R450X1 and really like the machine. Spent time figuring out all the differences from our other brands in the shop (Haas, Okuma, and Mori) and got everything pretty well setup and our cam spitting out ready to go code. We ended up creating a switch in our cam to use M265 for roughing and M260 for finishing and have been happy with the results.
    Now to my problem, I utilize max tool loads on the other brand machines as a safety to catch inserts that chip or to know when a end mill is about to give up the fight. Brother sold me a separate box that I found out later can only be programmed to look for no tool load (I guess for parts loaded twice in high production situations) but does nothing for my situation. So I did not have it installed and was wondering if someone out there using these machines, knows a way to trigger a alarm if a max tool load is reached and set a separate limit for each tool? I feel like there has to be some creative way to do this and I am always eager to learn new stuff.
    Thanks in advance for any replies!

  2. #2
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    256
    Post Thanks / Like
    Likes (Given)
    98
    Likes (Received)
    138

    Default

    I've looked at the Caron Engineering offerings and have heard good things about them. They have a TMAC system that sounds like what you are looking for.
    Home - Caron Engineering

    On another note, have you made any adjustments to the parameters for the M26_ High Accuracy mode? I find that setting the Corner, Arc and Curve settings for M265 to around 700 to 800 works well for roughing. It's about balancing cycle time vs accuracy. Those settings are user adjustable to suit your needs.

  3. #3
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,711
    Post Thanks / Like
    Likes (Given)
    6202
    Likes (Received)
    2233

    Default

    I've done a little bit of this on some Fanuc controlled lathes, but I know its possible for their mill controls as well. Although this is specifically about the brother control, I'm leaving this here for fuel for the conversation as well...

    On Fanuc, to run any kind of load monitoring, two things have to happen within the programming, and consequently, the ladder must be changed to suit as well. The first, is that a macro-interrupt option must be installed, and the ladder modified to allow this. The macro interrupt is what allows the control to "jump out" of the main program, and execute a macro-program if an overload event happens. The ladder must be modified, so that when macro-interrupt mode is turned "ON" via M-code, the ladder is looking for the overload signal so that it can execute the macro-program.

    What that means, is when you exceed the tool load, the control jumps from the main program, and executes the macro. On our lathes, if the spindle load got to high (broken insert) the control would jump to the O9--- program that we had specified, then retract (incrementally) from the workpiece 10mm in X, 5mm in Z, stop the spindle, home the machine, and then execute a custom alarm. On a mill, it could look however you want - rapid +Z, stop spindle, whatever else, etc, then custom-alarm...



    Once you have the Macro-interrupt established, then you could look at the load-monitoring aspect. This is when you need the software that monitors the channel (spindle motor, axis motor, coolant condition, etc...) - whatever the input is, compares it to timer parameters, and then sends the output signal that an overload condition has occurred, and begins the macro-interrupt sequence. The caron-engineering software probably handles the load-monitoring aspect by reading reading the output signals from the axis motors, plots the signals against your settings/parameters, and then sends the output signal to the control to execute the macro-interrupt.

    Okuma has the load-monitoring built into the control, but I'm not sure about the macro-interrupt. From my experience anyway, the controls would simply stop the program, and then go into an alarm state. Mazak also has load-monitoring as an option, but it's G/M code driven, and again, I don't know about the macro-interrupt.

    On Fanuc, we purchased an aftermarket option called "i_something_" which was the basic package, and was capable of monitoring the spindle axis, and a couple other optional channels. Their "iAdapt" software was capable of monitoring any axis channel, as well as adaptive feedrate, to keep one of these axis/servo channels within limits. The Caron Engineering will of course work on Fanuc, but the nice thing about the Fanuc optional software, is that everything is run within the control - there's no external hardware to interface or reference, so it's nice & tidy.



    Again, I'm only posting this to fuel the conversation. I'm sure the macro-interrupt signal would be easy enough to mimic on the Brother control, and the Caron Engineering may be able to handle the load monitoring.



    You may also be able to mimic this if you have the torque-skip option on the machine. This would be more challenging from a program perspective, but probably do-able. With drilling, you could probably do a...

    G31 Z-_
    G0 Z1.0

    setup, although you probably couldn't do this with tapping. Also, you'd have to work out how to stop the entire program at each hole, if the drill did in fact break - so that's a challenge from the programming aspect.

  4. #4
    Join Date
    Jan 2012
    Location
    Tampa, FL usa
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thank you both for the replies. I beifly looked at the Caron engineering link but ultimately was hoping to find a solution that is built in to the control I just was not aware of or a way of doing this through macros added to the program. The Caron option sounds like it can be costly incorporating external equipment and is not controlled through the machine control (I could be wrong and will have to research it more next week). Jashley73 it sounds like you did something similar to what I am trying to accomplish, but scare me when you talk about changing the plc ladder because I have no experience doing this and don't really want to mess something up. I really don't even need the machine to retract. I just want it to sense the load limit and stop the machine and display a alarm. My cheapest machine in the shop our Haas mini mill has this standard and is easily set for each tool. One of the nice things available on the Haas control. I accomplish the same function on our okuma and mori mills by turning the load monitoring on with m codes and setting other parameters (not as easy as the Haas tool load monitoring).
    So I guess I was wondering if the brother control is capable of doing something similar. It displays spindle loads and axis loads on one of the position screens, so I know the machine is monitoring them. I just need to peice together how to trigger a alarm if a load is exceeded. (Note my macro background is limited and I have never done nothing more than simple if and equal to statements)

  5. #5
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,711
    Post Thanks / Like
    Likes (Given)
    6202
    Likes (Received)
    2233

    Default

    I don't have the experience to change the ladder's either. The Fanuc tech made the changes, and was baked into the price of the option.

    Like I said, you could technically do this with torque-skip, but you'll have to get up to speed on macro programming. I'm also not sure if torque-skip works with the spindle axis, or if it's available on a Brother control. If so, then you'll have to write the program so, that if it does not exceed the torque limit, the program continues on as normal. If the torque-skip limit is made, then the program will have to stop & throw an alarm.

    After thinking a little bit about it, maybe a G66 sub-program could contain all the logic. I'm struggling to find an application where you'd use this outside of a drilling, or routine facing operation...

    Something like...

    O1234 (MAIN PROGRAM)

    G66 P1235 Z R F T (Think of this like a G81 cycle, that calls your custom program O1235...)
    X Y
    X Y
    X Y
    X Y
    X Y
    G67 (Think G80)



    O1235 (SUB PROGRAM)
    M-- (TORQUE SKIP ON)
    G90 G0 Z#18 (R-PLANE)
    G31 Z#26 F#9 T#20 (drill to "Z" depth, at "F" feed, watch to exceed "T" torque from main program, G66 line...)

    IF[#(whatever the variable for z-axis skip location) EQ #26] GOTO 99

    G0 Z#13 M9 (RAPID TO R-PLANE)
    M19
    #3000=(ALARM - Z-AXIS OVERLOAD)

    N99 (CONTINUE ON...)
    G0 Z#13 (R-PLANE)
    M-- (TORQUE SKIP OFF)
    M99

  6. #6
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    505
    Post Thanks / Like
    Likes (Given)
    339
    Likes (Received)
    188

    Default

    I haven’t dug too deep into it but every time I ask around the answer is, “nope!” for the Brother controls load monitoring...especially as a more-or-less “standard” option. Frank would know for sure.

    I end up using a combination of work probe and tool probe routines to check for broken/worn tools. I almost check every drill op with the tool probe before tool change and for em’s I tend to probe a feature on the workpiece and update the wear comp accordingly...once the offset exceeds some amount, say -.005”, I’ll force the tool change, alarm out, or whatever.

    I have a Fanuc-controlled Takisawa lathe with load monitoring and I think it’s real slick. My fav is the “sample” mode...I turn it on after putting a new insert in and it samples the highest load during the first toolpath and then automatically adds 10% to that, which becomes the “abnormal load” amount that will stop the machine or force a tool change or whatever. It’s nice when batch to batch material varies so a set-in-stone load amount wouldn’t really be apt for the application.

    So the short answer is, “no.” I hope they include it soon.

  7. Likes Jashley73 liked this post
  8. #7
    Join Date
    Jan 2012
    Location
    Tampa, FL usa
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Jashley73, I will read up on the G66 and see if it's possible to make it work. Even if I could atleast get it to work for the face mill op that would be useful. But seems too complicated to be practical for use on every tool like I am doing in the other machines. Thanks for the ideas though.

    Nerdlinger, I have pretty much been told the same thing by everyone I ask at Yamazen. But I like to not take no for a answer and dig because sometimes a solution pops up that someone found. So far no load monitoring is the only thing I'm not happy about. Hope it is something they add soon!

    Brotherfrank, responding to what you said earlier, I did see that you can change the settings for the M26_ codes and will mess with them some more as I get some free time. I did not purchase the mode B for the M28_ codes and was worried I messed up but it seems to do fine using the M260 for following the programmed contours. Maybe if I need to do more surfacing I will add the mode B later on.
    On another note, I think I saw you mention how to check pallets in the program in another thread. I am doing this now by checking the value of macro variable #5024 (QT axis position) and was wondering if your way was a cleaner solution? I don't think it was stated in the other thread. This works good for me but always like to see better ways of doing things. Thanks!

  9. #8
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,711
    Post Thanks / Like
    Likes (Given)
    6202
    Likes (Received)
    2233

    Default

    Just to be clear about G65 & G66. These are custom-macro program calls, and work similar to an M98 sub-program call.

    The difference between G65 & M98 however, is that G65 allows you to "pass on" local variable values to the sub program, via the letter/word "arguments."

    As an example, if you wrote...

    G65 P1235 X1. Y2. Z3. F50.

    in your main program, when the control then executed program O1235, it would "pass on" the values for local variables #24 (X) #25 (Y) #26 (Z) and #9 (F). (As a note, not all letters are available to use as arguments, and as a result, they're not always alpha-numerical equivalent... Reference a local-variable chart before you try to write one...)

    When your O1235 program ran, you could then program the machine to move however you'd like, but to keep it consistent, something like...

    O1235 (SUB-PROGRAM)
    G0 Z#26
    G1 X#24 F#9
    Y#25
    M99




    G65 works like M98, in that it works only once, on the line where it's programmed. G66 stays "active" like a drill cycle, and will execute on every line following, until canceled with G67. Something like...

    G66 P1235 Z R F
    X1.0 Y0.
    X 2.
    X3.
    X4.
    X5.
    X6.
    G67

    will execute program O1235 at every line, until canceled by G67 - much the same as any drilling cycle would. In fact, a perfect place to use G66, is if you had some crazy long drill, where you had to reverse, stop, forward the spindle, multiple feedrates & coolant on/off commands, at every hole location, to accommodate the long drill. With G66, you write that routine one time in the subprogram, and then let the control "repeat it" until you cancel it with G67.

    I hope that helps. - Best of luck.

  10. Likes Nerdlinger liked this post
  11. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    1,192
    Post Thanks / Like
    Likes (Given)
    1843
    Likes (Received)
    355

    Default

    Enshu wire in a gizmo like this for tool breakage detection,

    BK Mikro Broken Tool Detector Integrated with Enshu Machining Center - YouTube

    ^^^"BK mikro tool breakage detector" ^^^^

    And seems to be a close cousin of things like this

    Broken Tool Sensor for CNC machines.mp4 - YouTube


    Which is probably a knock off of something else that I'm not aware of.

    Maybe not too difficult to install? [No idea].

    Cheaper than a Renishaw laser probe, cuz small finishing tools + differences in spindle load would not be very detectable?

  12. #10
    Join Date
    Feb 2013
    Location
    Auburn, WA
    Posts
    694
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    822

    Default

    You do not need to buy Mode B, every C00 control includes it. The option is for an increase in look ahead over the default available when using Mode B.

    You should use the M28X codes for sure! The only issue is that the M280's cannot do a helix move, so make sure you post out anything with that type of move linearized.

    Generally speaking I rough without codes, and only use an M285 when I find I'm getting clipping which I usually fix in the CAM so I can keep the moves fast for the whole operation. I finish profiles with M281, and do helical bores or threading with M261.


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
  •