optimal clearance ?


Page 1 of 2 12 LastLast
Results 1 to 20 of 21

Thread: optimal clearance ?

  1. #1
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default optimal clearance ?

    hello i would like asking you about how much clearance do you use ...

    on lathe i use 2.5 mm

    on mill i use 5mm; i use more because i am not yet comfortable with the machine ... i worked more on lathes


    i am asking this like is there a minimal value, so the motors to speed up and reach optimal value before tool enters the material ?
    is my 2.5 too low ?
    should i consider a reaction time, for example, of 5 complete revolutions ? or 0.3 seconds ? kindly !

    Similar Threads:
    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  2. #2
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    my only "clue" is that minimal clearance must allow motors to reach optimal values

    i think that there should be no worries for the "rotary axis" :
    ... lathe :
    ...... S is stared when turret is at safe position
    ...... M is started same as S, or at least when tool is above the fixtures
    ... mill :
    ...... S is stared when tool is at max Z, right after a tool change procedure or
    ...... S is stared at least when tool is above the fixtures
    * this position where rotary axis starts is generally >>> clearance ( much GT clearance ), so no worries here if spindle can accelerate fast



    but what about "linear axis" ? i will check if my minimal clearances are enough for my highest cutting specs :
    ... lathe :
    ...... highest n * f : 2000 x 0.3 = 600 mm/min
    ...... clearance of 2.5 will be "vanished" in 2.5 / 600 * 60 = 0.25 seconds
    ...... note : highest n*f that i used for lathe is 2000x0.6, but this movement did not start with "f 0.6", but with a lower feed "0.2", and feed acceleration was while tool/knife was inside the material; if i would have started with highest feed, than tool may got broken when entering the material; is that "in" & "out" shocks

    ... mill :
    ...... highest n * fz * z : 1200 x 0.12 x 14 = 2016 mm/min
    ...... clearance of 5 will be "vanished" in 5 / 2016 * 60 = 0.15 seconds
    ...... note : i used 8000 x 0.08 x 14 inside aluminium, but i give up later, because parts were not payed well, and is not ok to go on such high rpm's on BT50

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  3. #3
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    so is 0.15 .. 0.25 seconds enough for a linear axis to speed up ? pls shoot me (**) i don't know ...

    if i think of the "load monitor imune time = 0.4 .. 0.8 ", than maybe would be ok to have enough clearance so the tool will enter the material after "imune time"

    Q&A
    1) what if the axis is still accelerating when tool is entering the material ?
    ... if cutting depth is ok, than i guess there is nothing to worry about ...

    2) what if the tool is entering the material before "imune time" ?
    ... then "entering" will not be monitored
    ... (*)

    3) is there a situation where clearance must allow motors to definetly reach optimal domain ?
    ... i think this matters only when surface quality is a must, like machining shiny parts with smooth surface



    ( * ) on mills "tool effort" must be > "limit" for at least 1 second, so this "greater effort minimal duration" of 1 second is actually a greater problem on mill than the idea of this thread; about mill reaction time of 1 second i read inside the manuals, so please, if someone has experience with monitoring on mills, please share if reaction time is really that big

    if a o25 drill goes broken, than :
    ... lathe will stop it after 0.1 seconds, enough to save the insert holder / tool
    ... mill will stop it after 1 second + reaction time; for a cutting spec of 1500 x 0.2 = 300mm/min, in 1 second, tool will travel 5 mm

    ( ** ) don't

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  4. #4
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello i found it : optimal distance ( δ ) should allow the "linear" and the "rotary" axis to get in sync :

    δ >= n * f * k / 1000, where :
    ... n * f : cutting specs
    ... k : cnc constant ( see attached image )

    for example, for a 2000o/min * 0.15mm/o : δ >= 2000 * 0.15 * 0.7 / 1000 = 0.21 mm



    on normal turning, when roughing or when finishing with common tolerances, there is no problem if the sync is achieved after the tool entered the material

    this applies also when direction varies, for example when taking a corner : acceleration and deceleration are done inside the material ( where else ? )

    M61 + G96 will boost things a bit also M63 modal + G97 might help a bit at the begining of the toolpath

    acc&decc is inside the material, and things mentioned above only reduce a bit the duration of this phenomen



    optimal clearance matters more when threading, because the f(pitch) is higher

    when threading, it matters before and after the thread, thus the toolpath is bounded between 2 danger zones

    i have a running setup that delivers pitch1.5 at 1000rpm : δ >= 1000 * 1.5 * 0.7 / 1000 = 1.05mm

    on this setup i have low clearances ( attached image )

    at this moment i am glad that i am doing this on an Okuma it may be possible that this setup will fail on another cnc, if sync is delayed kindly !

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  5. #5
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello mr Wizard good to see you

    Pretty much all of the Okumas now have high G servos so they can usually hit full rapid within about 12mm as a rule of thumb. That is usually only 1 rev of the ballscrew in most cases
    that's definetly mr Wizards experience

    I believe that the deceleration occurs quicker than the accel since it is being dynamically braked by the motor. I've heard 3 times faster but have not confirmed other than by actual trials where thread decel needed to be short and a good thread was still produced inside of the accel value that was calculated.
    yup, the hiG diagram is not symetric, and i really don't like when i have shocks durings turning, but in the end it delivers a good thread with low front/back clearances

    like how the "k = cnc constant" varies with machine type, also "acceleration" times varies with machine type : somehow is the same thing, a heavy turret will be slower than a light one, but still, the numbers are good, and i guess that anyone who delivered a thread with low clearances has saw that

    With a little creative thinking, you can calculate the needed value from your formula. I typically use 2mm clearance unless working with castings
    i use 5 and dynamic indexing after finding this chart, i will calculate those distances for my specs, and maybe i will also reduce this clearance

    On another note, the Load monitor immune time is set to .4 second which is plenty in nearly all cases. You may need to shorten it in order to monitor such things as peck drilling or threading since the feed motion may not be longer than .4 second in some cases
    now i don't monitor threads, since the operator is near the lathe

    and drilling with circa 0.4 + LM is not common
    ... if tool is little, it can not be sensed
    ... if tool is big, and cutting is for 0.4 seconds, than is a rare situation
    ... if tool is normal, than is the case when you try to cut deeper, chips dont go out, etc ...

    ...in some cases
    about particular cases, i would like to tell you that i monitor cutting inserts ( generally width=3 ) with caution

    the cnc can not feel this insert, but it can feel if the insert is broken and the holder is making contact with the part

    thus a good limit may save your holder when the operator is not paying atention : well, is a bit hard to react, especially if material has a tough crust

    so far i saved the holder many times .... and i trashed many holders before

    so during a setup i always have a warning on the cnc scrren, because of the limits but it works

    all the best

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  6. #6
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    those distances may be even smaller in reality, if guys from Okuma have used safety coeficients when calculating the values for K

    when LM=100, you can still go ...

    LM is there for a reference, for safety, but those cncs can be pushed until tool stops inside the material, and i don't think that someone had such kind of problems

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  7. #7
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    I typically use 2mm clearance unless working with castings. As always some adjustments needed for conditions
    i just scanned my running programs ; generaly i use :
    ... 5mm when knife is in front of the part
    ... 2.5mm when live tool is in front of the part
    ... 2mm when tool is coming from above, thus feed direction is on X

    i never thougth to make all equal i was feeling comfortable ... thanks again for the sugestion

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  8. #8
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello there is a "thing" when using low clearances, and i am afraid not to begin cutting at an increased diff value ...

    pls consider that the part is at Z0, and there is a Z_clearance=2.5

    Code:
        NOEX LVOX = 24424.689 LVOZ = 15678.463 ( encoders origins )
    
        turret @ safe pos
        G00 X50 Z2.5
        M331 ( stops the buffer, so to avoid the case when V1 & V2 are calculated too soon )
        NOEX V1 = VAPAX - LVOX - VETFX         - 50  ( delivers actual_x - program_x )
        NOEX V2 = VAPAZ - LVOZ - VETFZ - VSZOZ - 2.5 ( idem for z )
        G01 Z-whatever   
    if " rapids are high " & " droop control is off ", V1 can be 7mm, and V2 can be 15mm

    when the feeding movement begins, will diff become 0 ( or close to it ) right at the moment when execution begins ( attached image "case 3" ), or somewhere along the way ( attached image "case 2" ) ?

    i need a way to be sure, or " cnc fail army " ... kindly



    V1 = 9.388 when M331 is not there
    V1 = 7.133 when M331 is used once
    V1 = 0.368 when M331x6
    V1 = 0.001 when M331x18; definetly rocket science

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  9. #9
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello when indexing the turret at low clearances, like <2.5mm, i was afraid that a collision may appear : if i run the code in step-by-step, then all seems ok, but if i run it continuous, things are moving too fast and i can no longer observe what is going on

    i needed to be sure that a colision does not occur, without increasing the clearance distance

    pls consider this example :
    ... turret rotation speed @ 100%
    ... rapids 100%
    ... turret is moving down ( towards X- ) at index position
    ... a long drill is indexing at X0 Z1.25mm and after that it is going in rapid inside the part ( after indexing, rapid is executed only on Z axis )

    in this conditions, will the tool interfere with the part ?





    to handle this case, thus to index with low clearances, and without being affraid of a collision, i started using droop control :

    Code:
        turret at safe position
        NOEX VINPX = 0.4
        NOEX VINPZ = 0.4
        NOEX G65
        T M66 S M08 G00 IP M63
        NOEX G64
        linear movement : rapid or feed
    this code delivers droop control only for a single joint-point; thus the "linear movement" is executed only after a droop control check

    if you replace NOEX G65 with G65, than downtime will appear, because also turret safe position will be subject to droop control check

    all is ok, as long as VINP* < clearance





    code shared in this post is a simple example of how to use this technique; real codes that i use, especially for long setups, are a bit more complex, but this is a story for another time

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  10. #10
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello mr Wizard

    ... sometimes the safe position is reached, and the turret is still unclamping
    ... sometimes there is no need to rapid back to the part
    ... clearances are pretty low
    ... there are time charts, so to analyze the amount of time gain
    + others





    i have a folder, called " hollywood ", inside which i have 3 short movies, with setups that are using dynamic indexing

    next update should handle " middle index function " and " combi holders "

    in that moment, i will share the videos, because only the code, is not interesting the video is more communicative, more self-explanatory

    i don't rush, i need to be sure, or i will crash the machine





    i helped a guy with some parts; i put the dynamic indexing ( because setup would last a couple of days ), and i left from his shop without worries / kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  11. #11
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    Quote Originally Posted by deadlykitten View Post
    V1 = 9.388 when M331 is not there
    V1 = 7.133 when M331 is used once
    V1 = 0.368 when M331x6
    V1 = 0.001 when M331x18; definetly rocket science
    hello past self of my self : it seems a bit weird to obtain different values for V1, but actually is not

    in this code :

    Code:
        N1 G00 safe position
        N2 G00 X200 Z+2.5
      ( nothing, M331 once, or M331 many times )
        N3 NOEX V01=something with VAPAX V02=something with VAPAZ
    N3 will be executed only after previous line has confirmed it's execution

    normally this happens after "|axis_position-progam_position|<droop"; in other words, when N3 is executed, movement from N2 did not finish

    if you put 1 or more M331 codes, you simply delay the execution of N3, and during this delay, movement from N2 continues even futher

    if you put many M331 codes, the delay will allow the axis to reach the coordinates from the program, and, like this, ipw becames 0

    i needed to be sure that a colision does not occur, without increasing the clearance distance
    well, now i know the answer

    in this code :

    Code:
        N1 G00 safe position
        N2 G00 X200 Z+2.5
        N3 G01 Z-50 feed
    if rapids are high, when feed begins, X axis won't be at 200, but maybe at 210 ?!

    if feed is low enough to allow X droop to minimize ( thus to move from 210 to 200 ) until cutting edge reaches the part, then you won't crash the cnc

    otherwise, you will crash it

    for example, this code, where a drill is going in rapid inside a part, will crash, because clearance is low, is executed fast, thus there is no time to minimize the droop

    Code:
        N1 G00 safe position
        N2 G00 X200 Z+1
        N3 G00 Z-50
    in other words, when low clearances are used among an axis, it is required to be sure that the clearance is still long enough to allow the droop of the other axis to minimize

    another example : if threading ( among Z ) is done without a thread relief, and X clearance is low, and rapids are high, then the insert may cut during repositioning ( check attached )

    kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  12. #12
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello mr Wizard, i just wanna announce you that my latest dynamic indexing code is completed

    you are right : i really believe that only i will ever understand it

    i heared that there are at least 20 apprentices / day, all fighting about auto set fix r, oslow and ofast ...

    there is a thing about high-end particular macros, a thing that i am not going to talk about, but i am really sure that you know what i mean

    does it really matter if some machines are moving pretty optimized ? a root beer price is not affected by such sh** / kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  13. #13
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    Quote Originally Posted by OkumaWiz View Post
    You waste more time....

    Consider that it takes 3/4 of a second to unclamp the turret. I that same time you can rapid away from the part so you have now worries about indexing.

    It takes another 3/ of a second to clamp so you can rapid back to the part while it clamps.

    You need no goofy code that only you understand and you save NO time by going through all the extra steps.
    hello mr wizard since the moment i read your reply, i tried to convince you that there is a time gain; and it was hanging there, in my mind, on my 2dolist, but i did not know how to deal with it

    all this time i was reading and re-reading your arguments, and your reply always made sense, cristal clear, but 2 days ago, i had a revelation : i tried to check if the turret really unclamps in 3/4seconds, and if it clamps back in 3/, as you said, and i discovered that i can detect only the unclamp time, but i can not detect the clamping time

    and in that moment, voila, something kicked me : i don't have to formulate my answer based on your reply, thus i was looking in the wrong direction



    so i decided to share a real example : 1st time, when i started messing with all these, i was running a drilling setup

    a few minutes ago, i just rewrite the code for 2 drills, and i run it on the machine :
    ... image 1 : code 1 is a "normal" okuma code : no broken vector + ctr + $noex local&system variables
    ... image 2 : code 2 = code 1 + dynamic indexing
    * near the bottom, are the times for executing with reduced rapid speed ( slow ), or with full rapid speed ( fast )

    it can be seen that :
    ... "code-2 on slow" performs almost as fast as "code-1 on fast"
    ... "code-2 on fast " is quicker : 0.25-0.30seconds/index


    my dear mr Wizard, and all of you, a while ago, i started writing custom programs for reducing cycle times; one benefit was that those programs, runned at slow rapid, would perform almost as fast as a normal program with full rapids


    back then it was a big problem when using dynamic indexing @ full rapid speed : some tools crashed, sometimes the machine was indexing agressively ... but now those are fixed, code developed, more time is gained / kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  14. #14
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    you waste more time
    hello please check below video, from an okuma dealer

    instead of losing time in order to find the optimal indexing position and which ctr codes to execute and manually re-adjust at each setup change, such behaviour can be coded inside a *.ssb in order to execute automatically, taking into consideration tooling offsets, toolholder size, how many posts will the turret rotate between indexes, turret rotation sense, restart flags, colission bounding, swiching between machining states ( turning, y axis on, m110, etc ), and so on

    even if such a code works, it requires an amount of definitions way larger than normal, so, to shorthen the definitions time, use an app that allows fast definitions, gets offset data from machine, and scans the g-code, replacing "G00 home" with "If & call' functions

    once definition time has shorten, it's much easier to apply it with confidence also on shorter setups, and that's easy to say, requiring time to achieve

    for some gang lathes, and some mills with atc & spindle moving togheter, such procedures are factory default

    code processing speed, some confirmations, consistency, ratio between turret index time & rapid travel, etc, changes with osp generation; an older osp generation can't run such a code ( some system variables not yet available), or can't keep up with it thus whatever possible time gain during machining, is loosed, more ore less, during code parsing/execution

    but, once it works, tolerate :
    ... tool corections within ± tolerance_A
    ... clearances within ± tolerance_B
    ... rapid travel length to home position within ± tolerance_C
    * and avoid a crash by tolerance_A < tolerance_B < tolerance_C, and you may have the surprise to see that tolerance_C can be less than cas interference tolerance

    next video uses real close indexing positions in front of the part, and things can be pushed even futher, like real close above the part, or other scenarios / kindly



    Last edited by deadlykitten; 07-10-2021 at 07:16 AM.
    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  15. #15
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hello this thread is about minimal z clearances, as not to cause an interference

    it was a long journey to figure some things out, and i started looking into it as to achieve shorter cycle times when using m66/on-fly-index, which is a demanding safety code, but applications range is much more wider

    so i stepped toward the unpredictibility of okuma's ctr codes and variable index positions

    clearances have to be increased as :
    ... speeds go up
    ... direction change angles are close to 90*, like near a corner, but to generlize, as direction change angles are more an more far away from 180*

    using droop control is a method to ensure accuracy, but :
    ... feed2feed motions have different treatment than feed2rapid or other combinations, and for lathe, there is droop and rapid droop control, while mills are different, not like the motion control is different, but from the point of parameters and system variables
    ... N1 index position, N2 G00 X0 Z2.5 G65 may apply droop control also at the point where the axis are located before executing N2, and accurate index position is not a must, so downtime is created; to fix this, one may use this :
    ...... N1 index position, N2 rapid, N3 G65 N4 G64, N5 feed
    ......... or
    ...... N1 index position, N2 rapid, N3 G65 N4 feed G64
    *those codes should apply droop only at the clearance position, but there are disatvantages :
    ... G65 is used between 2 linear movements, so it will break the continuity of the motion, because it requires computational time, thus it's effect has a cost; this cost can be avoided by using noex
    ... G64 is used to disable G65, and it will add computation time for the next block, and under some scenarios, it will add downtime
    so another solution is N1 index position, N2 rapid, N3 NOEX G65 N4 NOEX G64, N5 feed
    ... p200 behaves different than p300, and also differernt than an updated p300, and those differencies include computation cost for noex blocks

    there are some trials behind this, some codes being tested over long term setups, or alone-intensive ipotethical scenarios, than those results have been used to boost up other codes



    as for droop control alternative with minimal cost, i present you this :

    Code:
        NLOOP IF [ ABS [ VAPA* - LV* - VSIO* ] LE 0.15 ] NDONE
            GOTO NLOOP
        NDONE NOEX
    
    or
    
        NLOOP IF [ ABS [ VAPA* - LV* - VSIO* ] LE 0.15 ] THEN NLOOP
    requires local variable definition LV* = VETF*+VBZO*+VZSH*+VSZO*, and unlike g65 that targets all axis in-position, it can be triggered only for that axis that may lead to an interference

    i like that code, because is simple, looks clean

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  16. #16
    Member arie kabaalstra's Avatar
    Join Date
    Jan 2007
    Location
    Netherlands
    Posts
    352
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    that all depends on the machine..I used 2 mm on the Bridgeport VMC 800, 1000, 600, 610, Interact, Oerlikon Vector, Schies & Froriep, Kiheung, Basically every Heidenhain Operated Machine i ever worked on, but i also used the same 2 mm on Elora controled machines, and on Cincinnatti and Fadal Controls..
    These were like 600mm or bigger tables (the Schiess & Froriep had a table of 6000 x 6000 and a 3500 mm Z-axis.. that thing was bigger than my Current workshop.

    On my own Beagle VMC 2814 (built it myself) i generally use 1 mm,

    On lathes, generaly 1 mm as well..

    it has to do with how much you trust yourself in Setting up the machine in the first place..
    I once ran the Bridgeport VMC 800 with a clearance of only 0.1 mm to show my chef the importance of calibrating the machine every now and then.. since it had a 600 mm Z-axis travel, Temperature differences could be up to 0.1 mm.. so.. if your machine isn't adjusted for temperature change in the workshop.. it's a Hit or Miss kinda thing..

    i ran to Z+0.1 in Rapid, to show how important it was.. hit the startbutton and turned away, knowing the machine would stop 0.1 mm above the workpiece.. i had a stop programmed after that,so i could open the door, and slide a 0.1 mm shim between the tool and the work.. and i told my chef to NEVER attempt anyhting similar on any other machine in the shop.. before i had finished my sentence there was a loud bang from one of the lathes.. turned out to be , indeed a Calibration fault.. as someone had moved a boring bar forward in the holder, and changed the workpiece offset.. WRONG!.. you should CALIBRATE!..

    What i Always do, and that as become sort of my "Signature" I move to an Initial Clearance, and then start the spindle, and if needed the Coolant as well, then move to clearance plane.. Like so:
    Code:
    T2M6
    S3200
    G00 X20 Y30 Z20 M3 (First Clearance, Spindle start)
    G00 Z2 (Real Clearance)
    After that i also move back up to Z20, and Turn spindle and Coolant off.. that way, your machine isn't sprayed with Coolant all the way up, if you have a toolchanger, or use G28 or G30 to move the spindle out of the way after the program.. to facillitate changing parts..

    I use G28 for that, it positions the table forward, in the middle with the spindle 10mm shy of the highes postion.. (this is also done with a future Toolchanger in mind, but the Z position has to be 5 mm lower to allow for Toolchange (HSK 25)
    G30 is the Home position, i always "park"the machine there, before shutting down, for a quick start the next time.



  17. #17
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    i ran to Z+0.1 in Rapid, to show how important it was
    hy arie such small clearances work when there is no deflection, thus rigid setups, and aproach is from a far position, as to not involve droop control for example :
    ... a boring bar can bend a 0.1 ... 0.5
    ... an antivibration bar may bend 1-2
    ... finishing a big diameter part at high hrc, will raise up the turret more 0.1 .. 0.3
    ... facing a hard material with a big endmill, may raise the spindle, especialy when using those inserts that tend to push the stock down

    imagine drilling at z-150, then g00 z01 folowed by g00 x100 g91 ... such a code will hit the drill in the stock, unless accuracy positioning codes are used

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  18. #18
    Member arie kabaalstra's Avatar
    Join Date
    Jan 2007
    Location
    Netherlands
    Posts
    352
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    hy arie such small clearances work when there is no deflection, thus rigid setups
    if your setup isn't rigid.. don't bother hitting the green button i always say...

    if your machine isn't rigid and repeatable, get a forklift, and throw the thing in a Dumpster..

    I've been working on Fairground and Amusmentpark rides.. and these are BIG (now you can imagine what we needed a 6 x 6 x 3.5 meters Mill for..)

    2 mm was stil my standard clearance before "entering"the work.. when transferring from 1 end to the other, i moved to 20 mm to take any deformation into account (since most parts were welded sub assemblies that needed milling/drilling afterwards.. first weld, then mill..

    I ran series of these parts.. making a "Jig" on the machine by means of clamps, and blocks of steel.. so i could just "Slot" my work in.. Program the lot, Hit start, get of the Operator Console, down the ladder, get part number 2 close to where part 1 is being machined in the mean time, so i could get part 1 out when done, get part 2 in, hit start, and move part 1 out of the way, making room for part 3.. Juggling with parts that would weigh up to 7 metric tonnes.. all in a days work..



  19. #19
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    indeed arie, anyone wishes for rigidity, but sometimes there may be a weak fixture, or overhang on tool , or whatever

    lately some o350 x 550 parts needed external turning with 0.02mm tolerance, after deposition of a hard layer, that simply distroys carbide inserts after 30-50mm, while better diamond tipped inserts would last a few complete passes, but with wear corections among the way

    for example, final radial docs are like 0.3 0.2 0.1 0.07 0.05 0.02, while offset corections are aplied, and, to achieve the last 0.02, the tool offset is raised with 0.2mm, or something, thus, in orider to go deeper, the tool is raised there is no linearity between offset and real doc, as the normal aproach was initialy grinding, which is much more stable and finess

    as passes are relativley long duration, is easy to loose track of corections, so a log is being kept

    this is just a particular example, as, in general, every setup has an elastic and plastic behaviour; and rigidity occurs when elastic behaviour does not affect the tolerance but of course it drives me crazy, i wanna throw the thing in the dumpster, like you said .... but i just have to get it done, what choice do i have ?

    .I used 2 mm on the Bridgeport VMC 800, 1000, 600, 610, Interact, Oerlikon Vector, Schies & Froriep, Kiheung, Basically every Heidenhain Operated Machine i ever worked on, but i also used the same 2 mm on Elora controled machines, and on Cincinnatti and Fadal Controls..
    the background of the clearances that i discused here, is in conjucton with okuma's codes; is a result of long term homework about cycles times shortening technique, trigering seconds, tens of a second, or even less, each time scale having different aproaches

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  20. #20
    Member arie kabaalstra's Avatar
    Join Date
    Jan 2007
    Location
    Netherlands
    Posts
    352
    Downloads
    0
    Uploads
    0

    Default Re: optimal clearance ?

    In my book.. Such discrepancies between offset and dimension, call for a more Rigid setup, or even hardturning..but that requires a way different machine..


    but, if Ceramics wear out that quicly, what kind of hardness are we talking about?.. I have done my fair share of Hardturning on a "regular CNC" with Kennametal MC2 Ceramics up to 63 HRc..without a hickup..

    if they wear out that fast.. Cutting Speed is too high.. rather take some more time to Finish a part than to stop and measure every single part 4-5 times..

    Like i always do: Rough out a part, until there is like 0.1 mm left.. then take the Finishing tool, and Remove the rest.. that should do the trick.

    At the moment, i'm running lots of TItanium parts, and i use a roughing tool for most operations, except Grooving, I Drill the inside to a "Comfortable dimension, and only have to Bore out mere tenths.. every part comes out like it should.. and when the upper border of a Tolerance field comes in sight, appliying a little bit offset does the trick.. be one step ahead of the game!.. at all times. Compensate for wear before you're out of Tolerance..



Page 1 of 2 12 LastLast

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

optimal clearance ?

optimal clearance ?