Question about lathe tool presetter
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Question Question about lathe tool presetter

    Machine: Hyundai Kia SKT 460 Lathe
    Control: Fanuc 21i-TB

    First time with having the luxury of an automatic tool presetter, only problem is it doesn't exactly seem all that automatic other than being provided the Mcodes and a little switch on the controller. I know I'm missing something here so I'm hoping someone can point me in the direction.

    My question is, how do I use the presetter comparable to the way HAAS runs theirs? Such as the Z axis automatically jogging the tool to the presetter and touching the tool off both while setting up the tool before a program and while in mid program?

    I tried my best to look through the vast depths of the internet before I bother anyone with the question, but I wasn't able to come across anything. Thanks for anyone who can give me a hand.

  2. #2
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    355
    Post Thanks / Like
    Likes (Given)
    236
    Likes (Received)
    145

    Default

    Does your machine have any tool probing macros loaded in the control? If it's a Renishaw tool setter the programs will be in the 9000 range and be called something like "REN AUTOSET".

  3. #3
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Thank you for your reply. The controller has macros installed in it, they are 9005, and 9007 which don't have a comment with them so not sure what exactly they are. There are also macros for the tail stock, but I don't use them, and quite honestly, I wouldn't exactly know how even I wanted to. Not going to pretend I know something that I truly don't. I haven't had the chance to enlighten my self into the macro capability world quite yet, we've been pretty busy so haven't really got to stumble my way through all that.

    As for the probe, it is a Marposs A90K probe.

  4. Likes DeSelle liked this post
  5. #4
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,656
    Post Thanks / Like
    Likes (Given)
    1007
    Likes (Received)
    1887

    Default

    You should get some documentation from the dealer. None of this is standard.

    For example, on a C-axis VTL with an 0i-TD:

    G202 TXXXX - flips down the arm, requires user to jog the tool to the probe tips manually
    G200 TXXXX - flips down the arm and automatically touches off the tool based on previous offsets

    A tool type number in the tool table indicates which sides of the probe the tool touches off of. E.g. "7" on this aforementioned machine indicates an RH turning tool, so the tool touches off in X- and Z-. Another tool type, e.g. "8" might indicate a RH boring bar where the tool touches off in X+ and Z-.

    A parameter can be changed such that the G200 overwrites the offset, checks the previous offset, or both. Another parameter can be changed such that there's a tolerance limit between the current and previous offset, and if the new measurement exceeds the tolerance, the machine alarms out, indicating an overly worn or broken tool.

    Again, it's probably different with every machine and the implementation is not tied to the control and definitely not tied to the probe, so some documentation will save you a lot of time and aggravation.

  6. Likes Joseph61189 liked this post
  7. #5
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Quote Originally Posted by Joseph61189 View Post
    Thank you for your reply. The controller has macros installed in it, they are 9005, and 9007 which don't have a comment with them so not sure what exactly they are. There are also macros for the tail stock, but I don't use them, and quite honestly, I wouldn't exactly know how even I wanted to. Not going to pretend I know something that I truly don't. I haven't had the chance to enlighten my self into the macro capability world quite yet, we've been pretty busy so haven't really got to stumble my way through all that.

    As for the probe, it is a Marposs A90K probe.
    Hi Joseph,
    The two Macro Programs Numbers you list are numbers that are associated with Subprogram call via "M" code. Take a look if any numbers are registered in parameters 6075 and 6076. If yes, then these numbers will be the M codes assigned to call these Macros.

    Post a listing of the two Macro Programs here. If they're only for tool setting, they shouldn't be too hard to decipher.

    Regards,

    Bill

  8. #6
    Join Date
    Mar 2006
    Location
    Columbus, Ohio
    Posts
    1,111
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    124

    Default

    I have trained shops on KIA lathes with tool presetter for many years, the manual made it fairly easy to figure it out the first time I tried it.
    Put the arm down manually, the screen changes to the present tool highlighted on the Offset page.
    Use the handwheel to get close, then switch to Jog, its automatically a slow jog.
    Do X or Z first, then the other.
    Do all tools, set the face, check the method in your manual, its a little different than Fanuc.
    The way I remember it, it was simple and fast.
    Good luck, for program examples, look on my website: doccnc.com
    Heinz.

  9. Likes Joseph61189 liked this post
  10. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Quote Originally Posted by Heinz R. Putz View Post
    I have trained shops on KIA lathes with tool presetter for many years, the manual made it fairly easy to figure it out the first time I tried it.
    Put the arm down manually, the screen changes to the present tool highlighted on the Offset page.
    Use the handwheel to get close, then switch to Jog, its automatically a slow jog.
    Do X or Z first, then the other.
    Do all tools, set the face, check the method in your manual, its a little different than Fanuc.
    The way I remember it, it was simple and fast.
    Good luck, for program examples, look on my website: doccnc.com
    Heinz.
    Hi Heinz,
    I'd suspect that the two programs 9005 and 9007 would automate the process; one may be for setting X the other Z. If these programs are being called via an "M" code, then its probable that the tool has to be manually positioned and then an "M" code via MDI is executed to drive the tool onto the setter and set the Offset. The reason is that both these programs are being called as Subprograms and not as Macro Programs. Accordingly arguments can't be passed to possibly position the tool automatically.

    To Joseph
    The parameter that corresponds to O9007 is 6077, not 6076 as I stated in Post #5.

    Regards,

    Bill

  11. Likes Joseph61189 liked this post
  12. #8
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Thanks for everyone's responses! I dug out the manual that is machine specific, I'll try and post what it says and see if someone can help me make sense of it. A lot of it seems to deal with tool life management and if you want the probe to be used in a program it provides a short example (off the top of my head) M12 M98 P9005 T0101 T0202 M99. My guestamation would be that by providing the two tool offset numbers, the machine will automatically touch off each tool in that range. Anyway, I know on our Mori Mills that has the tool touch off probe, it works with simple G code.

  13. #9
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Quote Originally Posted by Joseph61189 View Post
    Thanks for everyone's responses! I dug out the manual that is machine specific, I'll try and post what it says and see if someone can help me make sense of it. A lot of it seems to deal with tool life management and if you want the probe to be used in a program it provides a short example (off the top of my head) M12 M98 P9005 T0101 T0202 M99. My guestamation would be that by providing the two tool offset numbers, the machine will automatically touch off each tool in that range. Anyway, I know on our Mori Mills that has the tool touch off probe, it works with simple G code.
    Hi Joseph,
    The two program numbers you supplied in your Post #3 can only be called as Subprograms, not Macro Programs, if called via "M" code. That being so, arguments can't be passed to them; accordingly, only one tool number will be seen by the Subprogram if the Subprogram refers to System Parameter #4120 to get the last "T" Code executed. I understand that your example in Post #8 was off the top of your head, but its definitely not the way in which a Tool Range for setting would be made. In Tool Measuring Macros I've written, and its the same with Renishaw and others, I use an address to pass the Lower Bound and another to pass the Upper Bound of the Tool Number range. I use either a Custom "M" code or a "G" code that can call the program as a Macro and therefore, be able to pass these arguments via the "M" or "G" code.

    Do as I suggested in Post #5 and check to see what values, if any, have been registered in parameters 6075 and 6077 to determine what "M" code, if any, is being used to launch programs O9005 and O9007. The code for a Tool Setting Macro, or Sub, is fairly simple, therefore, Post programs O9005 and O9007 here and someone will be able to tell you what and how the programs do what they do.

    Regards,

    Bill

  14. #10
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Here are the Macros.

    %
    :9005
    #520=#3902
    IF[#520EQ0]GOTO190
    #521=#3901
    #522=#521-FIX[#521/#520]*#520
    IF[#522NE0]GOTO190
    G30U0W0
    M5
    M9
    G40
    M41
    N10
    #523=#100
    #524=#101
    #525=#523+#524
    IF[#525LE0]GOTO20
    T0101
    #133=#2301
    #134=#2901
    M98P9007
    #526=ABS[#2001]
    #527=ABS[#2101]
    IF[#526GT#100]GOTO200
    IF[#527GT#101]GOTO200
    N20
    #523=#102
    #524=#103
    #525=#523+#524
    IF[#525LE0]GOTO30
    T0202
    #133=#2302
    #134=#2902
    M98P9007
    #526=ABS[#2002]
    #527=ABS[#2102]
    IF[#526GT#102]GOTO200
    IF[#527GT#103]GOTO200
    N30
    #523=#104
    #524=#105
    #525=#523+#524
    IF[#525LE0]GOTO40
    T0303
    #133=#2303
    #134=#2903
    M98P9007
    #526=ABS[#2003]
    #527=ABS[#2103]
    IF[#526GT#104]GOTO200
    IF[#527GT#105]GOTO200
    N40
    #523=#106
    #524=#107
    #525=#523+#524
    IF[#525LE0]GOTO50
    T0404
    #133=#2304
    #134=#2904
    M98P9007
    #526=ABS[#2004]
    #527=ABS[#2104]
    IF[#526GT#106]GOTO200
    IF[#527GT#107]GOTO200
    N50
    #523=#108
    #524=#109
    #525=#523+#524
    IF[#525LE0]GOTO60
    T0505
    #133=#2305
    #134=#2905
    M98P9007
    #526=ABS[#2005]
    #527=ABS[#2105]
    IF[#526GT#108]GOTO200
    IF[#527GT#109]GOTO200
    N60
    #523=#110
    #524=#111
    #525=#523+#524
    IF[#525LE0]GOTO70
    T0606
    #133=#2306
    #134=#2906
    M98P9007
    #526=ABS[#2006]
    #527=ABS[#2106]
    IF[#526GT#110]GOTO200
    IF[#527GT#111]GOTO200
    N70
    #523=#112
    #524=#113
    #525=#523+#524
    IF[#525LE0]GOTO80
    T0707
    #133=#2307
    #134=#2907
    M98P9007
    #526=ABS[#2007]
    #527=ABS[#2107]
    IF[#526GT#112]GOTO200
    IF[#527GT#113]GOTO200
    N80
    #523=#114
    #524=#115
    #525=#523+#524
    IF[#525LE0]GOTO90
    T0808
    #133=#2308
    #134=#2908
    M98P9007
    #526=ABS[#2008]
    #527=ABS[#2108]
    IF[#526GT#114]GOTO200
    IF[#527GT#115]GOTO200
    N90
    #523=#116
    #524=#117
    #525=#523+#524
    IF[#525LE0]GOTO100
    T0909
    #133=#2309
    #134=#2909
    M98P9007
    #526=ABS[#2009]
    #527=ABS[#2109]
    IF[#526GT#116]GOTO200
    IF[#527GT#117]GOTO200
    N100
    #523=#118
    #524=#119
    #525=#523+#524
    IF[#525LE0]GOTO110
    T1010
    #133=#2310
    #134=#2910
    M98P9007
    #526=ABS[#2010]
    #527=ABS[#2110]
    IF[#526GT#118]GOTO200
    IF[#527GT#119]GOTO200
    N110
    #523=#120
    #524=#121
    #525=#523+#524
    IF[#525LE0]GOTO120
    T1111
    #133=#2311
    #134=#2911
    M98P9007
    #526=ABS[#2011]
    #527=ABS[#2111]
    IF[#526GT#120]GOTO200
    IF[#527GT#121]GOTO200
    N120
    #523=#122
    #524=#123
    #525=#523+#524
    IF[#525LE0]GOTO130
    T1212
    #133=#2312
    #134=#2912
    M98P9007
    #526=ABS[#2012]
    #527=ABS[#2112]
    IF[#526GT#122]GOTO200
    IF[#527GT#123]GOTO200
    N130
    #523=#124
    #524=#125
    #525=#523+#524
    IF[#525LE0]GOTO140
    T1313
    #133=#2313
    #134=#2913
    M98P9007
    #526=ABS[#2013]
    #527=ABS[#2113]
    IF[#526GT#124]GOTO200
    IF[#527GT#125]GOTO200
    N140
    #523=#126
    #524=#127
    #525=#523+#524
    IF[#525LE0]GOTO150
    T1414
    #133=#2314
    #134=#2914
    M98P9007
    #526=ABS[#2014]
    #527=ABS[#2114]
    IF[#526GT#126]GOTO200
    IF[#527GT#127]GOTO200
    N150
    #523=#128
    #524=#129
    #525=#523+#524
    IF[#525LE0]GOTO160
    T1515
    #133=#2315
    #134=#2915
    M98P9007
    #526=ABS[#2015]
    #527=ABS[#2115]
    IF[#526GT#128]GOTO200
    IF[#527GT#129]GOTO200
    N160
    #523=#130
    #524=#131
    #525=#523+#524
    IF[#525LE0]GOTO180
    T1616
    #133=#2316
    #134=#2916
    M98P9007
    #526=ABS[#2016]
    #527=ABS[#2116]
    IF[#526GT#130]GOTO200
    IF[#527GT#131]GOTO200
    N180
    M42
    GOTO190
    N200
    #3000=480(TOOL LIFE IS OVER)
    N210
    #3000=470(INPUT DATA IS WRONG)
    N190
    M99
    %

  15. #11
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    %
    :9007
    #516=#512+#2601
    #147=#5221
    if[#133le0]goto990
    if[#133ge9]goto990
    if[#133eq1]goto110
    if[#133eq2]goto120
    if[#133eq3]goto130
    if[#133eq4]goto140
    if[#133eq5]goto150
    if[#133eq6]goto160
    if[#133eq7]goto170
    if[#133eq8]goto180
    goto9999
    n110
    #132=#513/2
    #135=#134*2
    #136=#514/2
    #137=#516-#132
    #138=#510-#514-#147
    #139=#136+#132
    #140=#514+#513
    #142=#516-#513
    #143=#142-#136
    #144=#137+#134
    #145=#140+#135
    #146=#139+#134
    g0x#138
    z#144
    if[#523le0]goto111
    g36x[#510-#147]
    g4x0.1
    g0u-#514
    n111
    if[#524le0]goto112
    w-#146
    u#145
    g37z#142
    g4x0.1
    g0w-#136
    u-#145
    n112
    g30w0
    g30u0
    goto9999
    n120
    #132=#513/2
    #135=#134*2
    #136=#514/2
    #137=#516-#132
    #138=#510-#514-#147
    #139=#132+#136
    #140=#514+#513
    #141=#137-#134
    #142=#140+#135
    #143=#139+#134
    g0x#138
    z#141
    if[#523le0]goto111
    g36x[#510-#147]
    g4x0.1
    g0u-#514
    n111
    if[#524le0]goto112
    w#143
    u#142
    g37z#516
    g4x0.1
    g0w#136
    n112
    g30w0
    g30u0
    goto9999
    n130
    #132=#513/2
    #135=#134*2
    #136=#514/2
    #137=#516-#132
    #138=#511+#514-#147
    #139=#132+#136
    #140=#514+#513
    #141=#137-#134
    #142=#140+#135
    #143=#139+#134
    g0z#141
    x#138
    if[#523le0]goto111
    g36x[#511-#147]
    g4x0.1
    g0u#514
    n111
    if[#524le0]goto112
    w#143
    u-#142
    g37z#516
    g4x0.1
    g0w#136
    n112
    g30u0w0
    goto9999
    n140
    #132=#513/2
    #135=#134*2
    #136=#514/2
    #137=#516-#132
    #138=#511+#514-#147
    #139=#132+#136
    #140=#514+#513
    #142=#516-#513
    #143=#139+#134
    #144=#137+#134
    #145=#140+#135
    g0z#144
    x#138
    if[#523le0]goto111
    g36x[#511-#147]
    g4x0.1
    g0u#514
    n111
    if[#524le0]goto112
    w-#143
    u-#145
    g37z#142
    g4x0.1
    g0w-#136
    n112
    g30u0
    g30w0
    goto9999
    n150
    #132=#513/2
    #136=#514/2
    #142=#516-#513
    #143=#142-#136
    #144=#511-#513-#147
    g0z#143
    if[#524le0]goto112
    g0x#144
    g37z#142
    g4x0.1
    g0w-#136
    n112
    g30u0
    g30w0
    goto9999
    n160
    #132=#513/2
    #138=#510-#514-#147
    #137=#516-#132
    g0x#138
    z#137
    if[#523le0]goto112
    g36x[#510-#147]
    g4x0.1
    g0u-#514
    n112
    g30w0
    g30u0
    goto9999
    n170
    #132=#513/2
    #136=#514/2
    #137=#516+#136
    #140=#511-#513-#147
    g0x#140
    z#137
    if[#524le0]goto112
    g37z#516
    g4x0.1
    g0w#136
    n112
    g30w0
    g30u0
    goto9999
    n180
    #132=#513/2
    #136=#514/2
    #137=#516-#132
    #138=#511+#514-#147
    g0z#137
    g0x#138
    if[#523le0]goto112
    g36x[#511-#147]
    g4x0.1
    g0u#514
    n112
    g30u0
    g30w0
    goto9999
    #3000=50(ttype is wrong)
    n9999
    m99
    %

  16. #12
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Hi Joseph,
    These Macro Programs are to do with Tool Life Management; particularly program O9005. System Variable #3902 at the start of O9005 specifies the Target Number of Parts required. If its Zero, the program falls through to N199 and ends without calling O9007 or doing anything.

    O9007 uses Automatic Offset Setting "G" codes G36 and G37. It is called by O9005 if there is a target number of parts to make, but could also be used for setting tools. Look up parameter 6077 to see what "M" code is being used to call this program.

    Regards,

    Bill

  17. #13
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Hey Bill,
    Went to parameter 6077, no value was entered into the parameter. However, I suspect that the Mcode might be M12. img_20140516_155652_777.jpgimg_20140516_154825_133.jpg

  18. #14
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Quote Originally Posted by Joseph61189 View Post
    Hey Bill,
    Went to parameter 6077, no value was entered into the parameter. However, I suspect that the Mcode might be M12. img_20140516_155652_777.jpgimg_20140516_154825_133.jpg
    Hi Joseph,
    What this means is that neither O9005 nor O9007 are being called by an "M" code. If these are the only Macro Programs that you know are registered in the control, its likely that there are other Macros you can't access. What are called "Built-In Macros" can be registered and protected via parameters starting at parameter 12001. You can determine if Built-In Macros are present by looking at parameters 12011 and 12012. These two parameters describe the First and Last program number respectively that represent the program numbers that have been reserved for Built-In Macros.

    If M12 calls a Tool Setting function, then it either calls a protected Macro or is a PLC function (less likely), but it doesn't call either O9005 or O9007.

    Regards,

    Bill

  19. #15
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Alright, thanks for your help. I had to go into the parameters to make these viewable so they are considered built in along with the macros that are used for the tail stock.

  20. #16
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,189
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1789

    Default

    Quote Originally Posted by Joseph61189 View Post
    Alright, thanks for your help. I had to go into the parameters to make these viewable so they are considered built in along with the macros that are used for the tail stock.
    Hi Joseph,
    No. The parameter bit you changed to be able to access these programs would have been bit 4 of 3202. This bit gives low level protection to programs in the number range O9000 to O9999. You can also set bit 3202.0 to Zero to see if there are any programs in the O8000 to O8999 range registered. None of the programs protected by parameter 3202 are Built-In Macros. Password protection is often set via the 12001 series parameters to protect Built-In Macros from being accessed.

    Regards,

    Bill

  21. #17
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    6

    Default

    Alright then, thanks.


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
  •