Haas ST30Y 4 axis simultaneous... is it possible with XYZ and C?
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default Haas ST30Y 4 axis simultaneous... is it possible with XYZ and C?

    Hey everyone,

    I have a unique part I'm working on and would like to not have to do a 2nd op in our 5x mill. Essentially, I need to do a swarf mill on a feature that is wrapped around the part. The walls are perpindicular to the turning axis(Z), but there are sections where the wall is inline with that axis and runs in that direction as well. So, if I mill around the wall, the tool will need to move off center in the Y axis, but also drive the C axis at the same time. Thus, all 4 axis will need to move to create this path.

    Is this even possible? I know my CAM system can output the path in the right spot with the tool in the proper orientation, but right now our post doesn't support this. I tried hacking together some code from a post that would work but get an Invalid Statement error anytime there are all 4 axes on a single line. What this tells me is that it is NOT possible. But I've heard from others that they've done such things, yada yada yada, but here I am stuck with nothing working.

    Any ideas or knowledge for this type of thing?

    Thanks!

    edit: added some photos of a generic shape with the same type of contour.
    mt1.jpgmt2.jpg

  2. #2
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    870
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    458

    Default

    Yes, entirely possible. I've milled and turned(very slowly) an eccentric feature on my 2014 ST-10Y. XYZC simultaneous with live radial tool and parting tool.

  3. #3
    Join Date
    Jan 2020
    Country
    NORWAY
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    21

    Default

    Yup, that's doable. I've got a 2020 ST30Y and use Inventor "ultimate" CAM package.

  4. #4
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default

    Could one of you post some sample code so I can see where mine is messed up? There is nothing in the manual regarding syntax and when I try to put some code that 'should' work, a 'statement error' alarm comes up. I can try again, but I had no luck before.

    Does it matter if C is driven by IPM or DPM? Any other settings that I need to worry about?

  5. #5
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    870
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    458

    Default

    As far as I know, unless they updated the NGC (haven't tried on my new ds30y yet) you can only use IPM. No dpm or inverse time on the lathes..
    Gotta use the 4th axis diameter setting for whatever diameter you're working with. Sucks when you have different diameters in the same program, you'll end up with different feedrates.

  6. #6
    Join Date
    Jan 2020
    Country
    NORWAY
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    21

    Default

    Quote Originally Posted by thesidetalker View Post
    As far as I know, unless they updated the NGC (haven't tried on my new ds30y yet) you can only use IPM. No dpm or inverse time on the lathes..
    Gotta use the 4th axis diameter setting for whatever diameter you're working with. Sucks when you have different diameters in the same program, you'll end up with different feedrates.
    I use simultaneous c-axis / radial or axial milling quite often. Can't say that I've noticed anything about set diameters etc. In the CAM I set the feedrates, etc. and that's about it. Once it is running you cannot override feed rate on the ops panel though. On regular, non-c axis milling stuff, it's no prob to override feed rates.

    Attached is a snippet of a typical engraving program along with a picture of the engraved feature.

    On a sidenote - I guess you just used it as an example, but I would prob have turned the part you showed and milled a slot for a bolt on key/guide. You'd reduce machining time by a lot in addition to material wastage. And the finish would be way better.

    EDIT: Looked more closely on the pictures you posted. Forget my proposal - you need to do what you planned:-)

    img_20210622_130816.jpg

    %
    O41003 (ENGRAVING - FROM FUSION)
    G98 G18
    G21
    G50 S3400
    G53 G0 Y0.
    G53 X0.
    G53 Z0.

    (2D Contour1)
    T1212
    (Code generated in Fusion)
    M154
    G98
    G97
    P4000 M133
    G54
    M8
    G19
    M15
    G0 C-93.032
    G0 Z-43.175
    X103. Y0.
    G1 C-93.032 F3.946
    X101. F16.
    X98.8
    C-91.717 F16.453
    Z-40.966 F64.
    Z-40.968 C-96.865 F16.453
    Z-40.973 C-96.973
    Z-40.981 C-97.08
    Z-40.992 C-97.187
    Z-41.006 C-97.294
    Z-41.023 C-97.4
    Z-41.043 C-97.505
    Z-41.067 C-97.61
    Z-41.093 C-97.714
    Z-41.123 C-97.816
    Z-41.155 C-97.917
    Z-41.191 C-98.017
    Z-41.229 C-98.116
    Z-41.27 C-98.213
    Z-41.314 C-98.308
    Z-41.361 C-98.401
    Z-41.41 C-98.493
    Z-41.462 C-98.582
    Z-41.517 C-98.67
    Z-41.574 C-98.755
    Z-41.634 C-98.838
    Z-41.696 C-98.918
    Z-41.76 C-98.996
    Z-41.826 C-99.071...................and so on,,,
    Last edited by Schjell; 06-22-2021 at 07:25 AM. Reason: wrong info

  7. #7
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    870
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    458

    Default

    On the lathe control it is setting 102 - C-axis diameter

  8. #8
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default

    @thesidetalker
    Yeah, I know the C axis diameter setting.

    @Schjell
    The engraving code you posted is just XZC. I'm looking for XYZC code.

    Here is a screenshot of what happens when the wall that runs along the center axis and is also perpendicular to it, hence the need for Y movements along with XZC.
    mt3.jpg

  9. #9
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default

    Here is some code I hacked together that alarms out at N18:

    (-CONTOUR MILL1-)
    (MAIN SPINDLE, X-AXIS ROTARY TOOL)
    N5 G00 G53 Y0.
    N10 G53 X0.
    N15 G53 Z0.
    N20 G20 G40 G80
    N25 T1919 (0.2500 X 0.750L 4FL CRB EM)
    N30 G18
    N35 G98 M154
    N40 G54
    N45 G00 G28 H0
    N50 G97 P3500 M133
    N55 M08
    N7 G00 X1.9348 Y.2532 Z-.7301 C60.
    N8 X1.2431 Y.1627
    N9 X1.0431
    N10 G01 X.8431 F4.26
    N11 Y.1584 Z-.7328
    N12 Y.1489 Z-.7404
    N13 Y.1407 Z-.7495
    N14 Y.1341 Z-.7598
    N15 X.843 Y.1292 Z-.771
    N16 Y.1262 Z-.7829
    N17 Y.125 Z-.7951
    N18 X.8429 Y.1248 Z-.9489 F5.68 C60.0347 (<-- 386 Invalid Address Format)
    N19 X.843 Y.1244 Z-.9526 C60.1386
    N20 X.8429 Y.1236 Z-.9564 C60.3112
    ...

  10. #10
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    870
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    458

    Default

    Might be the 4 decimal places on your C letters. Try with 3.

  11. Likes Ox liked this post
  12. #11
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default

    I think it might also have to do with the G18. Might not have time to test today, but maybe after i get these things out the door.

  13. #12
    Join Date
    Jan 2020
    Country
    NORWAY
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    21

    Default

    Quote Originally Posted by BluishInventor View Post
    @thesidetalker
    Yeah, I know the C axis diameter setting.

    @Schjell
    The engraving code you posted is just XZC. I'm looking for XYZC code.

    Here is a screenshot of what happens when the wall that runs along the center axis and is also perpendicular to it, hence the need for Y movements along with XZC.
    mt3.jpg
    You're right, sorry about that. Pretty sure I've done it though, I recall a few jobs that I'll dig up the code for tomorrow and check. See attached picture, I am pretty sure it slid along the Y when doing this.

    What I haven't been able to do though is to mill along an angled plane or drill. I bought an adjustable live tool holder, but so far I have only been able to use it as an Axial or a radial holder, machine does not accept live tooling programs at an angle. Hence the hack shown on the picture. screenshot_20210622_194721_com.huawei.himovie.overseas.jpgscreenshot_20210622_194721_com.huawei.himovie.overseas.jpgscreenshot_20210622_194721_com.huawei.himovie.overseas.jpg

  14. #13
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    870
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    458

    Default

    Quote Originally Posted by BluishInventor View Post
    @thesidetalker
    Yeah, I know the C axis diameter setting.

    @Schjell
    The engraving code you posted is just XZC. I'm looking for XYZC code.

    Here is a screenshot of what happens when the wall that runs along the center axis and is also perpendicular to it, hence the need for Y movements along with XZC.
    mt3.jpg
    Here's a snippet from an old program. (M154 called @ previous tool)

    Code:
    G98 G97 G80 G40 G0 G19 
    G0 G53 X-.1 Y0
    G53 Z0
    M1 
    T707 
    M133 P6000 
    G0 Z-0.5043 C244.479 /M8 
    X1.7676 Y0.6961 
    G0 X1.4934 
    Y0.5881 
    X1.3934 
    G1 X1.0934 F20. 
    Z-0.5069 Y0.2985 X1.2499 F35. 
    G1 Z-0.5071 Y0.2985 X1.2426 C242.742
    Z-0.507 Y0.2984 X1.2364 C241.004 
    Z-0.507 Y0.296 X1.2301 C239.48 
    Z-0.5071 Y0.2935 X1.225 C237.956 
    Z-0.5071 Y0.2908 X1.2189 C236.448 
    Z-0.5071 Y0.288 X1.214 C234.94 
    Z-0.507 Y0.2874 X1.2073 C233.211 
    Z-0.5072 Y0.2867 X1.2019 C231.483 
    Z-0.507 Y0.2838 X1.1937 C229.325 
    Z-0.507 Y0.2808 X1.1876 C227.167 
    Z-0.507 Y0.2776 X1.1799 C225.007
    etc

  15. Likes BluishInventor liked this post
  16. #14
    Join Date
    Jul 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    12

    Default

    Ok, it looks like my G18 is probably the culprit. I will test and report back when I get a chance.

    Thanks, everyone!

  17. #15
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,664
    Post Thanks / Like
    Likes (Given)
    8004
    Likes (Received)
    9745

    Default

    Quote Originally Posted by BluishInventor View Post
    Ok, it looks like my G18 is probably the culprit. I will test and report back when I get a chance.

    Thanks, everyone!

    That was my first guess when reading the original post, but your code says that you are in G1, so ref plane is moot.


    I too would try backing down the C to 3 digits.
    And I'm guessing that your feedrate there will be WAY slow.
    I don't run Haas, but I ass_u_me that your feedrate in that line will be in degrees/min.



    ----------------

    Think Snow Eh!
    Ox


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •