584,861 active members*
4,923 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Okuma > Programming for Eccentric Turning...
Results 1 to 14 of 14
  1. #1
    Join Date
    Nov 2012
    Posts
    0

    Programming for Eccentric Turning...

    Hello folks, new member here.

    I've got a question about the possibility of eccentric turning. Without CAM software... The manual has been consulted. YouTube has been watched. The internet has been googled many times... So I've ended up here. This is on a Captain L470M with OSP100L control by the way.

    I was thinking about using creating a macro of sorts, timing the X-axis to the C-axis by means of using a sine or cosine function. Something like...

    G1 G91 X=SIN[ "C-AXIS POSITION" ] Z-.1mm C360. M15/M16 F2500mm

    ...or a variation thereof. My thinking being, that as the C-axis rotates, from C0*/SIN 0*) the X-axis should mimick an actual Sine-wave (incrementally that is, from it's starting point,) and interpolate positive up until C90*/SIN 90*, then negative to C270* / SIN 270*, then positive again back to C0* /SIN 0*.

    I've played around with this at the machine, but there's a few things I'm not sure of. I could get the control to accept a "G91 X=SIN[90]" command and actually get it to feed. (So, I know that you can program using a Sine, Cosine, Tangent function.) I tried writing a small loop macro where X=V30+1 and C=V30+1 would count up by 1-degree of rotation, up to 360, then reset V30=0, then repeat. But I could not get it to mimick an actual sine-wave. I'd like to replace 90 with the c-axis position if possible.
    [Edit: After some thinking, I realize that I was creating a spiral helix with this portion of code... It may be possible to disregard.]

    Clear as mud, right?

    One question I have- is there a read-only system variable for the C-Axis position? I tried "VAPAC", mirroring the VAPAX and VAPAZ variables listed in the manual. -No Dice. At least the control would not accept "X=SIN[VAPAC]" - it kept giving a "Syntax-2" alarm. Replacing the above VAPAC with a real number would work. Should I be using VSIOC (C-Axis command target point {program coordinate system} ) instead? Or is there another not listed in the manual.

    Second question - If there is such a system variable, (there has to be, right?) can I control one axis by a function of another axis' current position? Such as, "G1 X=[2 times the Z-axis' current position] Z10" or perhaps, "G1 X=[2*VAPAZ]" ?

    I know this sort of thing doesn't get asked a whole lot. I appreciate any help or advice you guys may have (Besides, "Get a CAM system, loser! " )

    Many thanks,
    -Justin

  2. #2
    Join Date
    Apr 2009
    Posts
    1262
    What you are trying to do should be possible. Your syntax error is just a typo I believe. Try adding another pair of brackets to your statement or if that doesn't work, try to set V1=VAPAC & then use V1 in your statement. What you will not be able to do is have one axis follow "live" with the C axis since when you look at the VAPAC it is basically a snapshot of what is currently in the register.

    Just going from memory I think the variable name is correct.

    I have done elliptical shapes on the Okuma, although it was using XZ moves, so it's possible, and accuracy depends on calculation increments, ie; it is really short line segments from calculated point to point, but the control will knock out thousands of blocks of code by itself with relative ease. (my ellipse had over 3500 blocks from about 4 lines of code)

    What I'm not sure of is if you are trying to mill the elliptical shape or turn it like you stated. If you want to turn it, you may want to use the G88 threading cycle to sync your axis with spindle rotations and still spin the spindle.

    Let me know which way you are going before we dig any deeper into this.

    Best regards,

  3. #3
    Join Date
    Nov 2012
    Posts
    0
    Wiz,

    I'm planning to turn the eccentricity. I currently don't have any live tools setup on the machine. Plus, the goal for this is to use the turning method as a future platform for rope threading, or basically any irregular eccentric turning.

    The Syntax alarm only showed up with the statement X=SIN[VAPAC] . When I changed the statement to X=SIN[90] the control accepted and processed the block. I thought I had a typo too (based on the alarm and previous experience,) and tried every possible way to word the statement using the VAPAC. Using an real number worked, so I'm pretty positive the VAPAC was causing the trouble.

    I'll try using a V1=VAPAC statement like you mentioned. I'll mess around with it and see if the value @ V1 on the parameter page changes with chuck rotation - but I suspect you're right, that it would only work as a snapshot, and only displayed accurately after immediate execution of the V1=VAPAC statement.

    Just another thought - On the "Actual Position" display, page 2/3, the "CD" shows in real-time the actual orientation of the spindle "C" axis. I'm guessing this would be said VAPAC that we are speaking of, correct?

    I don't have any experience using the G88 cycle you mentioned. I saw where you posted this in another thread, and checked it out in the programming manual. I understand how it sync's the axes together, but I'm not sure how that would be helpful in creating an eccentric. Are you suggesting that I adjust the lead, and use phased multiple leads to "multi-pass" the eccentric diameter in, so to speak?

    Going further, if that indeed is what you are suggesting, would it be possible to use the same approach for a rope thread? Perhaps using a macro to adjust the thread starting poing by a Sine/Cosine amount, and then call a single G88 or G33 pass, and repeat? Am I thinking in the right direction here?

    Many thanks Wiz!
    -Justin

  4. #4
    Join Date
    Apr 2009
    Posts
    1262
    If you want to turn you need to use the G88 cycle. With this cycle you can use both X and Z coordinates and you can time it with your revolutions to generate eccentric shapes. Like stated in my other post the RPM will make a difference on the amount of sharpness of axis reversal. This will probably require some playing with to accomplish your desired shape.

    Rope threads are turned this way by shifting your start point and following the rope form. Is this what you are trying to do?

    If not, To accomplish the eccentric you want, use both x and z coordinates and a federate to time the lobes with your spindle revs. You will need to go at a rather slow RPM probably under 500 or so depending on sine form desired.

    Best regards,

  5. #5
    Join Date
    Nov 2012
    Posts
    0
    I'll save the rope threads for later. I'll work on the eccentricity for now. Baby steps.

    I'll try messing around with the G88 cycle. I appreciate all the help. It may be a few days, but I'll try to post back with some results.

    Thanks again.
    -J

  6. #6
    Join Date
    Aug 2011
    Posts
    2517
    I've done a lot of rope threads in the past.
    it's just a thread with a special profile.I'm not aware of any software that can generate a special thread profile automatically (using G92/G33 etc)
    you can cut them by setting a start point then cutting a single thread with one small cut. then you shift the start a small amount then take another thread cut.
    shift start position
    take a thread cut
    shift start position
    take a thread cut
    etc etc etc

    most rope thread programs are several hundred lines of code

  7. #7
    Join Date
    Jun 2015
    Posts
    4131

    Re: Programming for Eccentric Turning...

    Quote Originally Posted by OkumaWiz View Post
    I have done elliptical shapes on the Okuma, although it was using XZ moves, so it's possible, and accuracy depends on calculation increments, ie; it is really short line segments from calculated point to point, but the control will knock out thousands of blocks of code by itself with relative ease. (my ellipse had over 3500 blocks from about 4 lines of code)

    What I'm not sure of is if you are trying to mill the elliptical shape or turn it like you stated. If you want to turn it, you may want to use the G88 threading cycle to sync your axis with spindle rotations and still spin the spindle
    hello mr Wizard i just started messing my head with rope threads ( seems i have too much free time ), and i found this discussion

    onestly, i did not know about the G88; to make it deliver a rope thread, then G112/G113 is required

    there is also the "circular threading" option for osp300

    it may be possible that "circular threading" is not the same thing as "G112/G113", just like how "G34/G35" is not the same thing as "G33/G31":
    ... one delivers a single thread
    ... the other one permits linking several threads, one right after the other

    about the ellipse ( 3500blocks from 4 lines of code ), i suppose that you have used an "if goto"


    i wish to thank you for sharing this G88, and in return, i will share my ellipse approach or do you wish for beer ? kindly !

    https://www.youtube.com/watch?v=O3twPF4b850
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  8. #8
    Join Date
    Jun 2015
    Posts
    4131

    Re: Programming for Eccentric Turning...

    hello mr Wizard i have been thinking about G88

    in image 1 is the example from the manual : at each spindle revolution, the machine moves only on Z with a constant increment ( eq among secvention 22 ) , or on both Z&X with constant increments ( secvention 23 ); so far, so good

    in image 2 is a single arch thread : depending on how the pitch is computed, at each spindle revo, machine moves with variable increments for X and Z, but the math for computing those increments is not complicated

    so far, in image 1 & 2, there is more than one pitch among a line segment, or among an arch



    in image 3 are special threads ( left low is a sin wave, just like Jashley was describing in #1 ); each toolpath represents a pitch : in this case, during one spindle revolution, we don't talk about an increment for X & Z axis, but about a complex geometry


    i will repeat my self :
    ... image 1+2 : many pitches among a simple geometry ( case a )
    ... image 3 : a complex geometry, within 1 pitch ( case b )



    G88 delivers "case a" without doubts, but do you know if it can deliver also "case b" ? have you delivered such a complex shape only by using G88 ?

    for example : is it possible to move the cnc among an ellipse toolpath, by using G88 + a single spindle revolution ?

    if this would be possible, than Okuma rocks


    so far i never tried G88, i don't even know if i have this function installed, so i thougth to ask / kindly
    Attached Thumbnails Attached Thumbnails 01.png   02.png   03.png  
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  9. #9
    Join Date
    Oct 2006
    Posts
    14

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    Hi Deadlykitten & Mr. OkumaWiz,
    I am trying to put a thread on a 2.5" convex conveyor Roller having 250" radius it is 10.5" long I think this G88 would be the ticket. Have you tried it yet? I did some awesome face knurling using G74 cycle (see pic) started at X2.6 in previous line G74 X.2 Z-.03 H.03 D.015 U.005 F.5 Q30 M74 M33. The Rollers are made from 304 Stainless so knurling is not my preferred method. I figured I would use a multi-start Arc Thread and I think that's the G88? Thanks for any input you or others might have on this.

    Bill

    I've done so much with so little for so long I think I can do almost anything with nothing

    Attachment 397654

  10. #10
    Join Date
    Jun 2015
    Posts
    4131

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    hi smwmachine so far i have not used the G88; that's definetly a task for mr Wizard ( i guess he delivered not only revolution parts, but also excentrics, by timing the feed with rpm and stuff )

    G88 seems to be kind of a G85, that begins at same spindle phase ( attached pdf ); i would begin with a G85 code, and change it to G88, to see what happens ?!?!

    I figured I would use a multi-start Arc Thread
    if you don't have an option ( like arc-threading, etc ), talk with kurmay

    I did some awesome face knurling ...
    please, how did you achieved the knurl-shape ? did you re-run the code at another Q value ? M03 ans M04 ? or was the tool cutting also when going towards X+ ? thx

    I've done so much with so little for so long I think I can do almost anything with nothing
    what about a big-bang ? kindly
    Attached Thumbnails Attached Thumbnails 01.PNG   02.PNG  
    Attached Files Attached Files
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  11. #11
    Join Date
    Oct 2006
    Posts
    14

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    Hello Deadly,
    Your correct about the Face thread & I used G72 not G74 that was a different program. I ran at .6 pitch with Q multi start 14 plcs. all in M4 spindle rotation the 1st per below ran in X+ then I changed the code to go X-. I use G71 for O.D. Threads and G72 for face threads. I put the wrong code in my last posting here is the actual code. Below is going X+.

    G0G97S200M4
    Z1. T0808 M87
    X0
    M8
    Z.02
    (T8 FACE THREADING)
    G72 X2.7 Z-.015 H.015 D.004 W.002 F.6 Q14 M74 M33

    What I want to do is the same knurling, but in G71 for O.D. for knurling a 2.25" X 10.5 long conveyor roller that has a crown for a flat belt of 200". The ideal option would be to just have to tell it in the G71 code an "L" or the "I" and "K". Then run it Z- then Z+.

    Thanks for the quick reply.
    Bill

  12. #12
    Join Date
    Jun 2015
    Posts
    4131

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    hello bill

    pls provide a clear drawing and the desired pitch

    i would try to run some G88 trials on your part, but i am busy, and those trials require some time

    i can't promise to do it soon; please, how long can you wait ? can you deliver your part somehow, and wait for a while ?



    if you are in a rush, i may give you a code that requires CXZ; only problem is that this kind of code, for your part, has a chance to be executed really slow, because it requires small segments, that may lead to cnc succumb :
    ... bad news : cycle time will be long, speed will not be constant, and tool may break
    ... good news : toolpath will be ok
    * the succumb phenomen appears as the pitch becomes smaller; when the pitch is greater, succumb phenomen may still be present, but with less effects



    also, because that thread is among a radius, is not possible to use the classical " shift Z&X + cut among Z + shift Z&X + cut among Z"



    your only solutions are "G88" or "the arc-thread-cutting-function ( optional )" or " a normal knurling tool + multus "

    at this moment i don't know if there are other alternatives / kindly




    check this out : about face knurling

    https://www.youtube.com/watch?v=OjDOSzIssBo
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  13. #13
    Join Date
    Oct 2006
    Posts
    14

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    Hi Deadly,
    I have to deliver part Monday. My machine does have the Profile generation and Plane conversion options. I think the "G112/G113" as well? I attached one of my machines Data Cards & a couple better pics of the face knurling the red primer part is the customer's sample it was knurled. I've attached another favorite part for this same customer a set of spools I made by pinch turning. The spools are 1.9" at the biggest dia. and .8" at the smallest.

    Attachment 397752
    Attachment 397750

  14. #14
    Join Date
    Jun 2015
    Posts
    4131

    Re: Programming Arc in Threads on OKUMA 5020L with G88?

    hello again / if you have G112 and 113, than you have the function installed ( check attached pdf )

    by "profile generation", do you mean G101 102 103 and,or 132 133 ? however, each one of them handles only 2 coordinates, and knurling for your part requires 3 coordinates, and computing all those coordinates at a small distance may lead to cnc succumb; the only function that can handle 3 coordinates as default is G01; even so, milling is slower then turning, and succumb milling is slower then milling

    i don't know what you mean by "plane conversion"; G17 18 119 ?

    monday ? check if you can run G112/113, and pls let me know ... kindly

    ps : those pinch turn parts look nice
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

Similar Threads

  1. How much eccentric it is ?
    By Ashish B in forum Hobby Discussion
    Replies: 2
    Last Post: 04-30-2012, 09:24 AM
  2. eccentric
    By hongjianming in forum CNC Swiss Screw Machines
    Replies: 1
    Last Post: 01-05-2011, 06:37 PM
  3. turning Intiutive programming off/on
    By riverracer in forum Haas Mills
    Replies: 2
    Last Post: 04-27-2010, 11:13 PM
  4. Eccentric Turning on LB 300
    By jimmyjolly in forum Okuma
    Replies: 4
    Last Post: 03-17-2010, 05:40 PM
  5. Best education for turning center programming?
    By protrxrptr17 in forum Community Club House
    Replies: 0
    Last Post: 05-08-2005, 12:24 AM

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
  •