TNC 151 Whole program doesn't download from TNC Server
Close
Login to Your Account
Likes Likes:  0
Results 1 to 10 of 10
  1. #1
    Join Date
    Mar 2017
    Country
    UNITED KINGDOM
    Posts
    35
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    6

    Default TNC 151 Whole program doesn't download from TNC Server

    Hello All,

    I am using fusion 360 and trying to load a program from a laptop via serial cable. It loads the first 3 lines then says stopped on TNC Server status a 2 bytes have been transmitted. It then just sits there.

    I am using a fusion 360 TNC155 Post and wonder if that is the issue?

    Here is code it generates:

    0 BEGIN PGM 1001 MM
    1 BLK FORM 0.1 Z X-51 Y-26 Z-26
    2 BLK FORM 0.2 X+51 Y+26 Z+0
    3 TOOL DEF 1 L0 R+5
    4 L Z+0 R0 F9998 M91
    5 M5
    6 TOOL CALL 1 Z S5000
    7 M3
    8 L X+56.5 Y-22.375 R0 F9998
    9 L Z+15 R0 F9998
    10 M8
    11 L Z+5 F9998
    12 L Z+0 F1000
    13 CC X+55.5 Z+0
    14 C X+55.5 Z-1 DR+
    15 L X+50
    16 L X-50
    17 CC X-50 Y-18.61
    18 C Y-14.845 DR-
    19 L X+50
    20 CC X+50 Z+0
    21 C X+51 Z+0 DR-
    22 L Z+5 F9998
    23 L X+56.5 Y+12.625 F9998
    24 L Z+0 F1000
    25 CC X+55.5 Z+0
    26 C X+55.5 Z-1 DR+
    27 L X+50
    28 L X-50
    29 CC X-50 Y+16.39
    30 C Y+20.155 DR-
    31 L X+50
    32 CC X+50 Z+0
    33 C X+51 Z+0 DR-
    34 L Z+15 F9998
    35 M9
    36 M5
    37 L Z+0 R0 F9998 M91
    38 M2
    39 END PGM 1001 MM

    I can't recall seeing BLK Form parameters in the heidenhain conversational before but then I am very new to programming.

    Any help much appreciated.

    I am running TNC server in FE mode as it transmits more code than ME mode. I have tried my serial port with different settings but no joy.

  2. #2
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    7,484
    Post Thanks / Like
    Likes (Given)
    709
    Likes (Received)
    3537

    Default

    What brand and generation of controller are you loading the program into? My Fanucs would have stopped on line 1. A letter O that is not in parenthesis is read as a new program number.

  3. #3
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,358
    Post Thanks / Like
    Likes (Given)
    281
    Likes (Received)
    2198

    Default

    Open the program in notepad and delete the block form blocks and see if it goes in there
    I will find my post that I deleted that from

  4. #4
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,358
    Post Thanks / Like
    Likes (Given)
    281
    Likes (Received)
    2198

    Default

    '
    there might be a post titled 'minimal heidenhain minimal' included in Fusion

    *caution* it contains M91 at the beginning and end which may crash your machine

    I will look for mine which I deleted them but it is at work

  5. #5
    Join Date
    Mar 2017
    Country
    LATVIA
    Posts
    371
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    189

    Default

    which mode exactly are you using to upload the code? perhaps you're trying to drip feed it?

    there are some parameters that define end characters for lines, port setting etc on the machine side, so maybe it is just coincidence that it stopped on line 4, the control may simply have ran out of buffer space for a single line when not understanding the end of line char put there by the F360 post processor

  6. #6
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    492
    Post Thanks / Like
    Likes (Given)
    1015
    Likes (Received)
    172

    Default

    I have TNC server set in FE mode as well and drip feed without issue. I would delete any "TOOL DEF" line (or turn off tool comments in the post dialog options inside Fusion). My TNC 355 control will fail to upload if any tool comments are in the program.

    Were you able to try the post that I attached to the other thread you started?

  7. #7
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,042
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    693

    Default

    Code looks fine,

    Set the controls mode from FE to EXT and try that if you are using a non heidenhain program to upload , also start control uploading before sending from the PC

    Also try using the heidenhain TNC server program (you'll have to set the mode back to FE for that)

    Boris

    PS M91 in TNC terms is use the machine datum as a reference for the move rather than the set datum. has no effect on the program

    PPS <<been away for a while

  8. #8
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,358
    Post Thanks / Like
    Likes (Given)
    281
    Likes (Received)
    2198

    Default

    code is not fine
    151 will not accept block form

  9. #9
    Join Date
    Dec 2012
    Location
    ny usa
    Posts
    522
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    272

    Default

    ^^^^Correct^^^^. I believe that's for the graphics on the 155.

  10. #10
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    492
    Post Thanks / Like
    Likes (Given)
    1015
    Likes (Received)
    172

    Default

    How are you coming along with this issue Colin?


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
  •