auto Z origin on lathe - Page 5


Page 5 of 5 FirstFirst ... 2345
Results 49 to 57 of 57

Thread: auto Z origin on lathe

  1. #49
    Registered
    Join Date
    Mar 2018
    Posts
    17
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    G00 X25 Z10
    G29 PZ=30
    G94 G22 PZ=25 Z-10 F200 D10
    G28
    G91
    G00 Z2.5
    G90

    This is ish how it looks. I'll get the specific one tomorrow.

    It is an OSP-P300S

    "
    G28
    G00 Z+2.5 G91
    G90
    NOEX VSZOZ = VSZOZ + VSIOZ - 2.5
    "
    Ill try this tomorrow




  2. #50
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2234
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    G00 X25 Z10
    G29 PZ=30
    G94 G22 PZ=25 Z-10 F200 D20 ( there is 20 from +10 to -10 )
    G28
    G00 Z2.5 G91
    G90
    NOEX VSZOZ = VSZOZ + VSIOZ - 2.5

    test it, and after that i will explain those variables; what means the "S" from osp300s ?


    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  3. #51
    Registered
    Join Date
    Mar 2018
    Posts
    17
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    ...
    G140 (-)
    G20 HP=1
    TD=108M323
    G50 S600
    G96 S250 M4
    G0 X400 Z5
    G29 PZ=30
    G95 G22 PZ=5 Z0 D5.0 L1.0 F0.1
    G28
    G91
    G0 Z5
    G90
    NOEX (VSZOZ)V1=VSZOZ+VSIOZ-5
    G20 HP=1
    M5
    M30
    ...
    I set it to 5% atm so I can "simulate" a hit with turning the feed up.On my V1 I get 726,617. This is the correct value if I were to change my zero point.If I only do V1=VSIOZ-5 I get the specific location on the start of my blank so I could put V1 as a cyclus start point!I think I got it man, thanks for the help!

    Last edited by Sammyen; 04-25-2018 at 04:11 AM.


  4. #52
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2234
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    hi

    i don't know if only 5% is enough; check the Z axis effort when cutting air, and use PZ=air+a_bit; if you have already done this, than is cool

    why do you use g50 s600 : is it a big machine ?

    so far i never used detection while cutting, but only when spindle was stationary, because the materials had a very tilted face after the bandsaw ; if you detect the face by cutting, than you should be sure that you always cut enough, so to get a straight face

    if you wish, pls check post 41 : it shows my code at work this is a way to begin cutting when there is no bar-feeder, and also the material is pulled to the turret instead of using a depth caliper : this is faster especially when the material is heavy and Z0 is pretty close to the chuck; if a depth caliber should be used, than the operator should sustain ( with one hand ) the entire mass of the bar which tends to fall, and with the 3rd hand it should keep the caliper into place ; using the turret makes it faster and requires less strength from the operator, especially for heavy materials; an operator which is less solicited should be more sharp about supervising the cnc; if he has worries that his muscles will atrophy, than he may bring a dumbbell to work

    once i have encoutered a pretty messy situation with a bar that should deliver 2 parts : the faces were so tilted, that i had to cut only a face at a time and check; otherwise it would be impossible to get 2 parts from the material : it happens when a low quality bandsaw is there

    about those system variables :
    ... VSZOZ : Z origin
    ... VSIOZ : comanded Z ( or target point if you wish ), not actual Z
    if you use
    N1 G00 Z0
    N2 G00 Z10
    N3 V1 = VSIOZ (V1 will show 10, while VSIOZ will be 10 since the moment of execution of line N2 )
    sometimes, things are not so straigth forward : during comp codes, VSIOZ may not be spot on : best practice is to test the code



    one more thing : "senseless gauging" is a reserved word, created by mr Wizard, so use it carefully, like G140 ( senseless gauging © mr Wizard ); from him i know this technique

    ok man

    Last edited by deadlykitten; 04-25-2018 at 08:56 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  5. #53
    Registered
    Join Date
    Mar 2018
    Posts
    17
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    Thanks for the info. Yes, its a big machine and the face is very often tilted.
    I will use this while the part is rotating to get the highest point.
    I'll call it something other than S. Gauging from now on!



  6. #54
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2234
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    hi / just a few more things :

    - you used s250*f0.1=25mm/min feed during G22; real feed will be at 1/5 ratio, thus only 5mm/min; G22 reduces the feed in this way, by default; i like to program the feed at 100*5 G94, so the real feed to be 100mm/min during contact; there is a maximal feed that is allowed during G22 ( 500mm/min or 2500mm/min; i dont remember exactly, but generally you won't reach that value ); so my advice, if you wish for 0.1mm/rot, simply use G95 G22 PZ=5 Z0 D5.0 L1.0 F0.1*5; i use higher feed because spindle is stationary in my case ( i have in idea how to boost you code, but i will share it later )

    - about the D : you begin at Z5 and target Z0 : this requires D5; how you also used L1.0, this may require D6 ? i don't know, so :
    ... pls check how the D is altered by L<>0, or
    ... use
    G95 G22 PZ=5 Z0 D5.0 (L1.0) F0.1*5

    - about the decimal points : the okuma controller may treat 5.0 the same as 5, so using
    G95 G22 PZ=5 Z0 D5 F0.1*5 should be just fine

    - about the feed position : i like to keep it at the end; the okuma controller should not treat differently "
    G95 G22 PZ=5 Z0 D5 F0.1*5 " and " G22 PZ=5 Z0 D5 F0.1*5 G95 ", so if you puted G95 right at the begining , considering that it must precced the G22, than you shoud not worry; better test this, to be sure ( some controlers<>okuma care about feed position )

    - about travel from Z5 to Z0 L1, thus from Z5 to Z-1 : this window may be to small : during it, the Z axis has to accelerate and avoid initial effort peek, and also decelerate near the end; this may create problems with higher feeds, because real zone where the effort will be stabilized will be -1<zone<5; the "zone" reduces as the feed increases, so i recomend you "
    G22 PZ=5 Z-10 D15 F0.1*5 G95 " in this way, you should be sure that during contact, you are away from the acceleration/deceleration zone; pls be aware that there are warnings about a " minimal 2.5mm clearance " to be used when load monitoring is involved, and more precise, " 5mm clearance is recomended"; so the contact should occure after at least 5mm from the position where G22 begins, and also, G22 should have at least 2.5mm after the contact point; so if you consider that the material will be anywhere between Z-2 and Z+3, use "G00 Z+3+5"+"G22 Z-2-2.5... "is it ok ? did i explained it well ?


    i hope you find these usefull kindly !


    Last edited by deadlykitten; 04-26-2018 at 02:39 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  7. #55
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2234
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    Quote Originally Posted by deadlykitten View Post
    i have in idea how to boost you code, but i will share it later
    to use G22 with higher feed, like 100mm/min, and keep the spindle stationary, than pls consider touching not with the "cutting edge", but with the "turret frontal"

    i guess your turret frontal is big enough to handle the X400 coordinate

    particular case example : if your material is X500 and turret can only reach X350, than simply shift your detected Z with a bit more; between X350detected and X500material, should be a little difference=d caused by the tilted bandsaw, so modify the Zorigin delivered by G22 with d

    idea behind all these is to have a G22 travel as minimal as possbile, executed as fast as possible

    if you just started using G22, than also try to implement this; trials will lead to a bit of downtime, but for the future, the code will remain unchanged

    if your material is very tilted, than 1st few face cuts should not stop at X0, but at X200, so not to cut air

    i have seen over the internet an example with a big lathe with live tools, that was getting the face done by circular milling : i guess this is faster than turning, and less air cut is there

    i hope you find it usefull and i hope i explain things well / kindly !

    Last edited by deadlykitten; 04-26-2018 at 03:25 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  8. #56
    Registered
    Join Date
    Mar 2018
    Posts
    17
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    Im using the cutting edge because I will put something like this under a G-code with inc. values so I can locate the part and set my cycle start points. I want to use the relevant tool and use as little time as possible. So if I want to turn a D400 part I will go to X395 Z10 and then have G206 to locate my part and set V1 as starting Z for face. (Spindle will not be stationary, but it will have the same "cutting data" as the operation it sets the start points for)
    Most of these are a few millimeters slant, but the big ones I have milled

    "G95 G22 PZ=5 Z0 D5.0 (L1.0) F0.1*5" - As long as there is more or equal distance from your starting point to the set Z value (Z0 in this case) it will not cause an alarm. The L can be as big as you want.At least that's what I got from it while trying. D=Distance from starting point to end point. (Not included L-length)

    Alarm:
    G0 X400 Z4.99
    G95 G22 PZ=5 Z0 D5.0 L1.0 F0.1*5

    No alarm:
    G0 X400 Z5
    G95 G22 PZ=5 Z0 D5.0 L10.0 F0.1*5

    Last edited by Sammyen; 04-27-2018 at 05:57 AM.


  9. #57
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2234
    Downloads
    0
    Uploads
    0

    Default Re: auto Z origin on lathe

    hello guys & girls an update will be soon shared in this thread, about facing & zeroing ( without G22 )

    fast & smooth, few keystrokes, versatile : easy adaptable to different diameters and bar lengths

    something like " not know what hit you " , or " what happened " / so smooth you don't know is there

    all-inclusive / kindly


    ps : i have to prepare the video ...

    if you wish to be famous, first you have to succeed
    ... where is Sid ?



Page 5 of 5 FirstFirst ... 2345

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

auto Z origin on lathe

auto Z origin on lathe