Matrix Nexus - Setting a Tool Load Limit?
Close
Login to Your Account
Results 1 to 14 of 14
  1. #1
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default Matrix Nexus - Setting a Tool Load Limit?

    Hello. I was wondering if it's possible to set a tool load/torque limit for each tool? So for instance, let's say my roughing WNMG tool is sitting at 30% spindle load I know something went wrong if it suddenly hits 40+%. I want the machine to stop if this happens.

    I had a pretty nasty crash the other day because the insert broke and the machine kept going, throwing the entire tool revolver out of alignment. Not good! I'm sure this could have been prevented if I had a way to limit each tool. Maybe it's even possible to limit the Z-axis motor as well? What do you think?

  2. #2
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    412
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    165

    Default

    This can be done for any spindle and any axis with the overload detection option. You can check if you have it by going to the Diagnosis page -> Version -> Option. If option #47 "2nd Auxillary Functions" is turned on then you have it. If not, it's an easy software option to add in the field. If you do have it, there should be a separate small manual that describes it in detail.

    You get a set of M codes that let's you set up a table for different tools with maximum load, how long it can be in that load before stopping, and how you'd like the machine to stop (feed hold only, or feed hold and spindle stop). Up to 10 monitoring tables can be set. So you can set spindle load to 30% and Z axis load to 45% for example for the roughing tool.

  3. Likes Isak Andersson liked this post
  4. #3
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default

    Thank you. Turns out we do have option #47. Now I just need to find the right M-codes...

  5. #4
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    412
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    165

    Default

    Here's some more info. I believe your machine will use "A" codes instead of "B" codes. It will make a lot more sense if you can find the manual.

    (LOAD DETECTION SAMPLE)

    (SET PEAK LOAD TO 999)
    M378 B999 (999 IS MAX LOAD)

    (SET UP TABLE 1 WITH LOAD AND TIME)
    M376 B100 (100 PERCENT)
    M377 B20 (2 SECONDS)
    M379 B01 (TABLE 1)

    (SET UP TABLE 2 WITH LOAD AND TIME)
    M376 B50 (50 PERCENT)
    M377 B40 (4 SECONDS)
    M379 B02 (TABLE 2)

    (UP TO 10 TABLES CAN BE SET)

    (START DETECTION)
    M371 B201 (DETECT Z-AXIS ACCORDING TO TABLE 1)
    (M374) M375 (CONDITION FEED HOLD, OR FH WITH SP. STOP)

    (!!! INSERT ROUGH MACHINING OPERATION HERE !!!)

    (START DETECTION)
    M371 B602 (DETECT SPINDLE-1 ACCORDING TO TABLE 2)

    (!!! INSERT ROUGH MACHINING OPERATION HERE !!!)

    (PAUSE DETECTION)
    M370 B602 (PAUSE DETECTING SP1 ACCORDING TO TABLE 2)

    (!!! INSERT FINISH MACHINING OPERATION HERE !!!)

    (CANCEL ALL LOAD DETECTION)
    M370 B0 (CANCEL FOR ALL AXES)

    (INSERT OTHER MACHINING OPERATIONS NOT REQUIRING LOAD DETECT)

    M30 (PROGRAM END)




    (M-CODES)
    (M370 AXIAL LOAD DETECTION INVALID)
    (M371 AXIAL LOAD DETECTION START)
    (B-CODES, OR A)
    (0** = ALL AXES)
    (1** = X AXIS)
    (2** = Z AXIS)
    (3** = C AXIS)
    (4** = 4TH AXIS)
    (5** = 5TH AXIS)
    (6** = SPINDLE 1)
    (7** = SPINDLE 2)
    (8** = MILLING SPINDLE)

    (M372 AXIAL LOAD DETECTION TEMPORARILY INVALID)
    (M373 AXIAL LOAD DETECTION RESTART)

    (M374 FEED HOLD ON OVERLOAD, CLEAR TO CONT. OR RESET)
    (M375 FH AND SP STOP ONOVERLOAD, MUST RESET)

    (M376 DETECTION LEVEL PERCENTAGE)
    (M377 DETECTION TIME SETTING)
    (M378 DETECTION PEAK PRECENTAGE)
    (M379 DETECTION TABLE NUMBER REGISTRATION)

    (FOLLOW THESE M-CODES WITH A OR B CODE)


    (SAMPLE DATA TABLE FROM EXAMPLE ABOVE)
    ( # - PERCENT - SECONDS)
    (01 100 2 )
    (02 50 4 )
    (03 )
    (04 )
    (05 )
    (06 )
    (07 )
    (08 )
    (09 )
    (10 )


    (ALARM EXAMPLE)

    (#253 OVERLOAD DETECT 1, , )

    (--ALARMS STATUS--)
    (AXIS - TIME - LOAD)
    ( X 1 11 )
    ( Z 2 12 )
    ( C 3 13 )
    (4TH 4 14 )
    (5TH 5 15 )
    (SP1 6 16 )
    (SP2 7 17 )
    (MILL SP 8 18 )

  6. Likes Isak Andersson liked this post
  7. #5
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default

    Thank you very much for the help. I still haven't found any of this in the manual so this is a huge help.

    Stupid question, tho. How would you do any of this in a Mazatrol program? I know about the M CODE unit but this only takes M-codes with no extra values. MANL PRG doesn't seem to take M-codes at all. Is there a different unit I'm missing?

  8. #6
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,247
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    330

    Default

    I think you could do a sub program in mazatrol


    For the poster that posted the code what do you mean by A codes vs B codes? I know this was a thing on Fanuc but Im confused does mazatrol have different types of codes aswell?

    Ive just always had trouble with getting fusion to post code that my integrex can read without having to heavily modify it. My machine just has a matrix control 2007 vintage.

  9. #7
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    412
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    165

    Default

    You can do it in mazatrol just using M code units.

    A codes are used on a machine with a B axis, B codes are used with a machine with an A axis more or less.

    overload-mazatrol.jpg

  10. #8
    Join Date
    May 2020
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    16

    Default

    screenshot-2021-12-29-16-09-33-operating-manual-h747s40020e-pdf.jpg This is from a HCN 6000 smooth manual but I believe your control has the same. Should be easy to set with conversational tool data. As you can see in the picture one setting is for the feed axis (X,Y,Z) the other is for spindle load. With active feed control it will dial the feedrate back to maintain desired load and if it gets too far out and over a time limit it will fault and feed hold.

    Working on uploading clearer picture but in tool data there is a thrust force setting( feed axis) and a horse power ( spindle load )

  11. #9
    Join Date
    May 2020
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    16

    Default

    Attempt #4 screenshot-2021-12-29-16-09-33-operating-pdf.png

    Seems as good as I can figure out for the moment. If values are left at 0 the AFC is off. So if you think it should be at 30% spindle load then set it to 30%. When it goes above that it will dial the feedrate back until 50% feedrate for 5 seconds then it will feed hold. That is what my 2019 manual says. Can't say for sure the older machine will work the same but I'm confident you have these data boxes for each tool and it likely will function the same. Look in your book for AFC ( Active Feed Control)
    Attached Thumbnails Attached Thumbnails screenshot-2021-12-29-16-09-33-operating-manual-pdf.jpg  

  12. #10
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default

    Sorry, I couldn't see the image you posted. Where do I put the A (or B) codes if I cant put them in the program? I've checked the tool data page also but I don't see anything there relating to "Active Feed Control".

    This is what my Tool Data page looks like:

  13. #11
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    412
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    165

    Default

    Active feed control (AFC) is only for milling tools. You have to use overload detection for turning operations.

  14. #12
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default

    Sorry, I'm still confused. If it just takes the M-codes then where do I enter the actual percentages and timings?

    Could you upload the image to Postimages — free image hosting / image upload (or a similar site)? I can't make out anything in the image you posted.

  15. #13
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    412
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    165

    Default

    Ok try this out. The 4th M code in each block is how you set the percentages, that's why they are a different color, they will show up in yellow on your machine. There should be a soft key for "Other Code" or something along those lines when you're in the field.

    Overload Mazatrol — Postimages

  16. #14
    Join Date
    Nov 2021
    Country
    SWEDEN
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    4

    Default

    I see. So only the 4th, 8th, and 12th codes can be used for "Other Code". No wonder I didn't find it. But then how am I supposed to read what the "Other Code" is if it's only marked in yellow? Very unintuitive I must say.

    Edit:
    By the way. When I try to input an "Other Code" with a value lower than 100 it gives me "401 Illegal Format". What's that all about?

    Edit2:
    Ok, so it turns out you're not supposed to enter the actual code, just the value. I guess Mazatrol will know automatically which code to use based on the M-code? Do I have that right?
    Last edited by Isak Andersson; 01-03-2022 at 08:04 AM.


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
  •