Newbie Okuma OSP5000 - Tool table.


Results 1 to 16 of 16

Thread: Okuma OSP5000 - Tool table.

  1. #1
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Okuma OSP5000 - Tool table.

    So in the tool table there is 32 tool places..
    But when looking at the tool definition page, i can only edit 12 tools by using page up and page down.

    Looking at the offset table tho i find 32 tools..

    How can i set tool types for the other 20 slots?
    Okuma OSP5000 - Tool table.-20210916_195840-jpg


    And also what does the "P" column represent for the tools?
    Okuma OSP5000 - Tool table.-20210916_195727-jpg

    Similar Threads:


  2. #2
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    hy
    ... 12 is turret capacity, more precise is how many different turrent index positions are there, or, if you wish, is magazine capacity
    ... 32 is the number of available offsets; if it was lower, like 12, thus equal with magazine capacity, then perhaps it would have made more sense

    the reason why 32>12, is there in order to allow using more than 1 tool / turret index, like dual/stacked toolholders, or live tooling with more than 2 shafts/chucks

    P is the compensation quadrant, so for the machine to know how to calculate tool nose center: let's say that you just mounted an external and an internal tool, and you just measured them, then you executed the program; machine will call each tool as T020202 and T060606, then it will need to compute tool nose center, as appropiate for each operation; for example :
    ... for external cilindrical cutting, tool nose center = X offset + 2*radius
    ... for internal cilindrical cutting, tool nose center = X offset - 2*radius, and so on, combinations appear

    machine has no clue if to use "+" or "-", even if you measured those 2 tools, on X, at different positions on the touch setter; the one that tell's the machine where to use +/-/do nothing, is the P argument

    so P argument will help the machine locate tool nose center, in respect to offset data i don't have time now, but if you search a bit on the forum you can find images that show how P actually corelates those datas; also, at least on newer machines, there is an on-screen guide

    with/without such images, i can tell that for normal ( asimetrical tools ), P numbers are shifted trigonometic quadrants, starting from 180*
    ... asimetrical tools will always use "+" or "-" when computing tool nose center in X and Y
    ... simetrical tools will use "+" or "-" only once, like when computing tool nose center in X or Y, while Y or X will be equal to offset value
    *do you need more infos on this topic ?




    [ extra infos here ]

    to use a tool inside the program, then you have to call turret station and offset : Taabbcc, where:
    ... bb is turret station, thus between 01 and 12
    ... cc is offset, thus between 01 and 32, more precise is the sum of main offset + wear
    ... aa is radius, thus also between 01 and 32, more precise is referring to nose radius and compensation quadrant, or P

    in other words, T is a macro comand, that assings like this T[ radius & P ][ turret index/station ][ main offset + wear ], towards data from your tool offset table

    is not a must to always use T with all those 3 arguments, for example :
    ... if your turret is allready indexed at position 2 and you wish to cut a face in mdi, then T020202 and T02 will both do just fine; calling T with a single argument, is like calling only the last one[ main offset + wear ], and since turret is allready indexed at position 2, then you no longer need to index it at position 2; also, if you face cut in mdi-manual, then you won't use radius compensation, so no reason to use [ radius & P ] argument;
    ... if your program does not use radius compensation, then T020202 and T0202 ( or T202 ) will all do just fine; calling T with a 2 arguments, means that a 3rd one, [ radius & P ] argument, is ignored; how the code does not use rad compensation, then calling, or not calling, [ radius & P ] is irrevant, since this is not needed; as a consequence, if data from offset table has wrong inputs for radius and P, then you can simply leave them as they are, only if you don't need them, so no need for extra care, or keeping tool data table updated unnecesary; this allows to set up a turret using minimal amount of data, and, for example, on a newer machine, you simply autoload all this informations inside the controller

    as a short brief conclusion :
    ... Trto : rad, station, offset
    ... Tto : station, offset
    ... To : offset
    * maybe you shouldn't bother right now with such things, unless you are coding yourself and wish for tricks; igf and other software will define automatically their needed T format

    T0202, T202 and T000202 are equivalent / kindly

    Last edited by deadlykitten; 09-17-2021 at 01:35 AM.


  3. #3
    Member Algirdas's Avatar
    Join Date
    Mar 2009
    Location
    United Arab Emirates
    Posts
    1681
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    I want to try to explain it in a little bit more simple way.
    Calling the tool you need to indicate:
    1. Tool number in the turret. Can't be ommited.
    2. Tool offset number. You can assign tool offset number "02" to the tool number "01". This is not practical however. Tool number 1 can be used together with tool offset number 1 and 11 and 21 and 31 - up to you. Tool offset number can be omitted, then the "zero" tool offset will be used.
    3. Tool nose radius compensation number. The same story as tool offset number. Can be omitted.

    What I would like to emphasize. Take a look into the manual. There is very good illustration showing where is what. Like in the lines:
    T011121
    and
    T0111
    where the tool number is and where the tool offset number is. It's possible that these two lines are calling different tools.



  4. #4
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Quote Originally Posted by Algirdas View Post
    I want to try to explain it in a little bit more simple way.
    Calling the tool you need to indicate:
    1. Tool number in the turret. Can't be ommited.
    2. Tool offset number. You can assign tool offset number "02" to the tool number "01". This is not practical however. Tool number 1 can be used together with tool offset number 1 and 11 and 21 and 31 - up to you. Tool offset number can be omitted, then the "zero" tool offset will be used.
    3. Tool nose radius compensation number. The same story as tool offset number. Can be omitted.

    What I would like to emphasize. Take a look into the manual. There is very good illustration showing where is what. Like in the lines:
    T011121
    and
    T0111
    where the tool number is and where the tool offset number is. It's possible that these two lines are calling different tools.
    Thanks.. I find it strange tho that i cannot punch in T0101 and have it change it has to have the third P number for some reason.

    And really thanks to Deadlykitten, complicated but gave me some food for though.



  5. #5
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Quote Originally Posted by deadlykitten View Post

    as a short brief conclusion :
    ... Trto : rad, station, offset
    ... Tto : station, offset
    ... To : offset
    * maybe you shouldn't bother right now with such things, unless you are coding yourself and wish for tricks; igf and other software will define automatically their needed T format

    T0202, T202 and T000202 are equivalent / kindly
    My initial thought around this were "do P need to be set".. and i guess the answer is "yes, but it depends" on how you get the program into the machine.
    As you said i would drive this machine from CAM, specifically Fusion360.. and i just rewrote some Okuma post processor to deal with this LB15 more correctly.. And why i started eyeballing the tool table and felt bamboozled.

    Last edited by NeoTech; 09-17-2021 at 04:43 AM.


  6. #6
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    hello again pls check attached stuff on P quadrant

    i cannot punch in T0101 and have it change it has to have the third P number for some reason
    over time, tool definitions changed, as they where merged, or completely independent from virtual tool library

    My initial thought around this were "do P need to be set".. and i guess the answer is "yes, but it depends" on how you get the program into the machine.
    i don't know exactly for you machine, but is possible to entirely avoid P, even on a code that uses G41/G42; depending on control generation, this may not work, or, contrary, it may be done in different manners

    i just rewrote some Okuma post processor to deal with this LB15 more correctly
    if i may ask, how long did it took you to learn how to edit the post processor, and change it, in order to deliver what you want ? and please, what is machine configuration : 1-2 spindles, dual turret, y, full progamable / quill extent tailstock ?

    really thanks to Deadlykitten, complicated but gave me some food for though
    i simply shared a bit more infos, trying to show that there are more things possible

    for example, you deal with tool initializations, and cam edit, etc, but entire control can be by-passed, data being sent to/from it

    for example, an okuma automated cell, programed remote ( with full integration ), do you think that someone is actually doing setup on it ? is all robotic, even setup & tooling change operator intervene in case of a failure, or an alarm being popped up

    Calling the tool you need to indicate:
    1. Tool number in the turret. Can't be ommited.
    2. Tool offset number. You can assign tool offset number "02" to the tool number "01". This is not practical however. Tool number 1 can be used together with tool offset number 1 and 11 and 21 and 31 - up to you. Tool offset number can be omitted, then the "zero" tool offset will be used.
    3. Tool nose radius compensation number. The same story as tool offset number. Can be omitted.
    hy mr bunny i will talk only from p300 perspective (things may differ for other generations):


    1) can be ommited; for example:
    ... for a groove tool, if Trto is active, then is possible to comand block in_position To, thus simply changing only the offset, in order to finish the 2nd flanc/wall
    ... for a live tool, like a drill that uses a chamfer attachemnt, again, if Trto is active, then, is possible to change to To, in order to switch from drill nose to chamfer insert; if changing is not done through To, but other statment, then live spindle rotation will stop, M spindle will orient to turret index position, turret index will perform, only that it won't rotate since it is allready where it should be, and then, M spindle rotation will be restored; all these is time loss

    conditions for this to work :
    ... Trto active before To
    ...... or
    ... turret allready indexed at working station, then To being called

    if someone has doubts, then i will simply share codes and machine behaviour


    2) is not possible to omit the offset number; for example, possible combination for T comand are : Trto Tto To, thus, in all of them, there is o = offset

    *Trto = rad station offset

    if someone has doubts, simply mdi T00 and see what happens


    3) just like you said, rad can be omited


    it may seem a bit too much, i don't know, but in the end, is all about T comands, knowing how different formats works (TD TL), or control a machine that has no wear, or has wear, or maybe even other 2 extra levels of offsets / kindly

    Attached Thumbnails Attached Thumbnails Okuma OSP5000 - Tool table.-p-value-okuma-jpg  
    Attached Files Attached Files


  7. #7
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Quote Originally Posted by deadlykitten View Post
    If i may ask, how long did it took you to learn how to edit the post processor, and change it, in order to deliver what you want ? and please, what is machine configuration : 1-2 spindles, dual turret, y, full progamable / quill extent tailstock ?
    Well it took me about 20min to figure out howto rewrite the postprocessor for this machine.. I wrote a scratch one for my old Siemens 810M a couple of yers ago (it circulates on the forum)..
    And i rewrote the 810D one to be more parametric for my milling machine..

    For this okuma machine i downloaded the official one, identified all the crap in it and threw it out and rewrote some of the threading stuff so it fits this older system.
    My machine is a single spindle, single turrent, fully programable chuck and tailstock. (with some hardware issue atm).

    But.. i have been a systems developer for banks and meditech the past 22 years.. so bit of javascript in fusion is not the big issue for me, its more of a understanding what the heck im implementing. D



  8. #8
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    i have been a systems developer for banks and meditech the past 22 years.. so bit of javascript in fusion is not the big issue for me
    okey i recently started creating an okuma postprocessor, and i realized that most of it's complexity comes from integration of okuma special functions, that are not on other machines, so making it run a non okuma cnc would mean to simply disable all those okuma specifics, then change the syntax of simple g-code

    as a consequence, i realized that this kind of approach will work on a more general case, like fixing compatibity issue between any kind of cam and any kind of cnc

    i guess now you are after fixing those dnc and chucking issues, but, if anytime you will need something, or think of doing something that is not common, i will try to help / kindly



  9. #9
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    I fixed the serial transfer issue so i can now send code into the machine just fine actually.. now just the damn chucking issue to sort out.

    As most of the machine is kinda "basic" i just removed a whole lot of things i have no driven tools or anything.

    So in that regard this machine is kinda happy go lucky right.

    But when i got to tool table selection i got bit stumped cuz i wanted to make use of all the tool tables in a sane manner so now writing so that if tools are higher than 12 error but if offset is within 1->32 be happy about it..
    And then trying to see if i can just skip the whole P value all together.

    Idea is to be able to run a gang holder of spot, drill and ream/thread from one tool position with multiple offsets.



  10. #10
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    32 is default for 12 stations turrrets, but, if needed, there is spec for 64 96 or even 200 offsets

    max i have used is 16 offsets for a 12 station turret; however, if you will ever need more than 32 offsets, then it may be possible to make it work, even if there aren't more than 32 offsets available; for example, is possible to force 40 offsets into 32, by using kind of a custom approach; it may sound weird, but is less expensive than buying the update from okuma

    about that gang holder:
    ... it may be possible to avoid the spot, because carbide drills may spot themselves, if programmed corectly, and edge is sharp, and L/D is still reasonable; so far, i have drilled without spoting up to 6.2 D, stable, long term series
    ... for ream/thread, you may need to consider a floating/compensation chuck; yes, it may work rigid if you aling them, but even so, if alignment is good, a floating chuck will prolong tool life; things may vary :
    ...... a reamer may need a floating chuck
    ...... a tap may need only an z adjsutment holder, while it's flexibility will act like a float; for example, even if a holder is not floating, it's construction may be flexibile enough for the tool to float

    things can be discussed, etc i have build such a gang for mulltiple drilling, thus up to 3 drills/post; all with internal coolant, clamped with er chuks, clumped with bronze screws, so to protect surfaces + quick hydraulic conectors, so to get coolant from the main toolholder is not hard to imagine it, only to machine it square, respecting all paralelism / perpendicular requirements, etc



  11. #11
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    hello pls find attached infos for a custom gang toolholder

    er chucks can be replaced with simple reduction sleeves, or whatever clamping system you wish / kindly

    Attached Thumbnails Attached Thumbnails Okuma OSP5000 - Tool table.-g01-png   Okuma OSP5000 - Tool table.-g02-png   Okuma OSP5000 - Tool table.-g03-png   Okuma OSP5000 - Tool table.-g04-png  

    Okuma OSP5000 - Tool table.-g05-png  


  12. #12
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Quote Originally Posted by deadlykitten View Post
    hello pls find attached infos for a custom gang toolholder

    er chucks can be replaced with simple reduction sleeves, or whatever clamping system you wish / kindly
    And they are mounted as a normal cutter would be right but you zero it up as a boring bar essentially??



  13. #13
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    yes in image 3, the width of the gang is 50, and this will put all the bore center among x axis, just like a stacked internal toolholder

    if you mount, inside each one:
    ... a small boring bar / picco, then you will zero each one just like you said
    ... a drill, or whatever similar tool, then you will need to ensure that it is coaxial with the spindle, and only after that proceed to offset declaration

    however, before measuring the tools, it is ok to check the gang itself, empty, without tools in it; this is because normal alignment procedure is targeting coaxiality inside the bore of an internal toolholder, that has it's axis at X0, while the gang may have bores at X<>0; it may not seem important, unless you use small tools; as you increase tool size, then also they will be able to handle more missalignment; in reality, there is a big chance that the gang won't be aligned, even if your turret alingment is ok; maybe, at this moment, it is too soon to talk about this, but just be carefull, because skiping this step may break some tools or maybe it won't happen

    considering that gang is at post 1, then you may use offsets :
    ... 1 13 and 14, thus inside the program will be needed T010101 T130113 and T140114
    ...... or
    ... 1 21 and 18 : T010101 T210121 and T180118

    some persons preffer to always use the 2nd offset as being 1st offset + 20; this is kind of a simple rule, so to keep offsets number organized, but it works only for 2 edges / turret post ( like only dual gang toolholders ), and only for simple lathes; it may seem to be a limitation, but truth is that most lathes are simple, and there are rare cases when is neded to use more than 2 edges / post for example, there are rare cases when someone uses a gang, just like you wish

    Last edited by deadlykitten; 09-18-2021 at 03:35 PM.


  14. #14
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Quote Originally Posted by deadlykitten View Post
    yes in image 3, the width of the gang is 50, and this will put all the bore center among x axis, just like a stacked internal toolholder

    if you mount, inside each one:
    ... a small boring bar / picco, then you will zero each one just like you said
    ... a drill, or whatever similar tool, then you will need to ensure that it is coaxial with the spindle, and only after that proceed to offset declaration

    however, before measuring the tools, it is ok to check the gang itself, empty, without tools in it; this is because normal alignment procedure is targeting coaxiality inside the bore of an internal toolholder, that has it's axis at X0, while the gang may have bores at X<>0; it may not seem important, unless you use small tools; as you increase tool size, then also they will be able to handle more missalignment; in reality, there is a big chance that the gang won't be aligned, even if your turret alingment is ok; maybe, at this moment, it is too soon to talk about this, but just be carefull, because skiping this step may break some tools or maybe it won't happen

    considering that gang is at post 1, then you may use offsets :
    ... 1 13 and 14, thus inside the program will be needed T010101 T130113 and T140114
    ...... or
    ... 1 21 and 18 : T010101 T210121 and T180118

    some persons preffer to always use the 2nd offset as being 1st offset + 20; this is kind of a simple rule, so to keep offsets number organized, but it works only for 2 edges / turret post ( like only dual gang toolholders ), and only for simple lathes; it may seem to be a limitation, but truth is that most lathes are simple, and there are rare cases when is neded to use more than 2 edges / post for example, there are rare cases when someone uses a gang, just like you wish
    gotta say i like this, its very clever i need to make a couple in my milling machine..

    Being able to run gang groups, with a bar puller and a make shift "coolant" driven endmill spindles in this machine seem not be to hard..



  15. #15
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    3445
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    [ about gang ]

    please, if i may ask, why do you wish to go for a gang ? i have used such, when the turret was overloaded, thus really there was no more space to add something; i am not sure, maybe you wish to avoid loosing time, is your turret slow indexing ? even so, does it worth the effort ?

    [ about bar pullers ]

    be carefull with bar pullers, as they can damage your machine let me explain; there are barr pullers that grab the material, moving among :
    ... z axis : those can create a high effort peak, that is hard to detect, especialy if someone is not aware of it; for example, effort required to drill a o40 hole may be 80-100% load meter, while a bar puller can reach 150-200%; the difference is that the drill creates effort in a crescendo, slowly, while the puller will reach it's max value very very fast, even if it is programed with low feed; it is possible that the puller will reach >200, but for a such short period of time, that the machine won't stop ( normally, machine stops if effort is too big, for a period of time that is at least xyz miliseconds ); using it like this for too long, may lead to accelerated wear among machine parts related to z axis
    ... x axis : the same as above, only that wear will apear among machine parts related to x/y axis

    people, sometime, simply over tighten a bar puller, considering that this will guarantee that the puller will never slip, but truth is that you can achieve grip without over tightening ( like using custom profile claws, wear resistant, etc ), and/or by improving puller's alignment in respect to spindle; i have seen how, during a setup that lasted more than a few weeks, the barrpuler acted with asimetrical forces, leading to impregnating the turret oil grooves into the x saddle; marks where <0.03, but still visible and the distance between the marks was exactly equal with the puller travel : what a coincidence

    to avoid such cases, i use load monitor function, but there are cases that lead to wear, that the load function can not detect :
    ... if asimetrical forces appear, and they are not aligned with xzy axis, but perpendicular, then load function simply wont react; such forces will tend to raise/dissasamble the turret, and can not be easy detected; is like, when milling, you can see if the spindle effort is increasing and decide to lower the cutting specs, but, sometimes, even if spindle effort is ok, it may be subject to a force that has the tendency to bent it, and the load function simply won't detect it
    ... there are cases when wear manifests during a long period of time, such long, that one may think that everything is still ok for example, maybe you expect that an insert will last a few parts, or a few hours, etc, but a bar puller can manifest a wear curve that is a few weeks long, and until one figures out exactly what is hapening, he may try and test all kind of things; i use to measure ocasionally, the consistency of the bar puller travel, and once something changes, i will check if it is wear or something else

    [ about end mill spindle ]

    if i may ask, how will you be able to use them, if you don't have C axis / break ? or you have c axis, and if yes, then why do you wish for a coolant driven spindle ? high rpms ?





    by the way, this just crossed my mind :
    ... you could make a gang with end mill spindles
    ... if a gang idea seems too old school, you could customize kind of railways tooholders, that will clamp at an ajustable position, across the turret face
    ... is possible to craft, in house, a high performance tool quick change system, for static and live holders; a system that is similar in performace to anything else on the market, but cheaper
    ... quick change systems for the toolholders, like to achieve, on a bmt turret, a toolholder changing time that is similar to vdi
    ... and other things

    in short, is possible to create a high level of modularity, designed to minimize idle time / kindly

    Last edited by deadlykitten; 09-19-2021 at 12:09 PM.


  16. #16
    Member NeoTech's Avatar
    Join Date
    Aug 2007
    Location
    Sweden
    Posts
    73
    Downloads
    0
    Uploads
    0

    Default Re: Okuma OSP5000 - Tool table.

    Bar pullers, can be as easy as a bit of plastic that "flexes" around the bar stock tho and when unclamping not pulling off the bar.. and if its not unclamped properly will just "loose grip".. No fancy deal here..

    What i like with ganging up spot, drill and threading in one go and as such i can have multiple threading groups setup.

    Coolant driven endmill spindles just doesnt require anything to drive em.. from a machine point of view.. the C axis break tho is a different problem i need to adress in that case. i have a bunch of unused M codes so thinking of implementing a break that way..



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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Okuma OSP5000 - Tool table.

Okuma OSP5000 - Tool table.

Okuma OSP5000 - Tool table.