Heidenhain 426
Close
Login to Your Account
Results 1 to 8 of 8

Thread: Heidenhain 426

  1. #1
    Join Date
    May 2012
    Location
    Almont, Mi, USA
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    3

    Default Heidenhain 426

    Trying to get a conversational post to work in either Fusion 360 or Inventor 2018 and have a question about using datum tables and cycle def 7 or 247.

    Here is the code it puts out.

    21 CYCL DEF 247 DATUM SETTING ~ I get an error 21 with no further explanation. I can't find a cycle 247. 7 yes but I get an incomplete cycl def if I change 247 to 7. I do want to use the datum table stored on the controller. This is as far as I was able to get on this one.
    Q339=1 ; DATUM NUMBER

    Thanks.

    Kevin V.

  2. #2
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    When my control throws that error the number is referring to the line number.

    Heres the start of the program im running right now, hopefully it will give you ideas.

    0 BEGIN PGM EYEBOLTS-ENDS INCH
    1 CYCL DEF 247 DATUM SETTING ~
    2 Q339= 3; DATUM NUMBER
    3 ; SET W0.0 OR GAUGE HEIGHT AND Z0.0
    4 Q1825 = 1;W OFFSET BACK

  3. #3
    Join Date
    Sep 2002
    Location
    gloucester ma
    Posts
    1,608
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    943

    Default

    personally I got a post working pretty well in Fusion and put all my datums etc in at the machine

    When editing the post you can make it say just about anything at the beginning of the program, so if you are always calling a datum table you can call that all as text.

    editing the posts is kind of something you really need to get your mind wrapped around. I guess it is Javascript

  4. #4
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,551
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    661

    Default

    What's the code look like at cycle 247? It should be something like:

    13 CYCL DEF 247 DATUM SETTING
    Q339 = 4



    That's the way it will look if you punch it in at the keyboard. Many post processors will put a line number or other punctuation somewhere in the cycle definition, in my experience that causes problems.

  5. #5
    Join Date
    May 2012
    Location
    Almont, Mi, USA
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    3

    Default

    Thanks all for your help and input. Didn't put too much thought into the conversational post, we have the ISO pot tweaked to our liking. Attached below. Use it at your own risk.heidenhainiso-mei_New .cps.zip

    Unzip and remove the .txt extension.

  6. #6
    Join Date
    Jul 2005
    Location
    San Francisco, CA
    Posts
    802
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    80

    Default

    Quote Originally Posted by KevinV_MEI View Post
    Trying to get a conversational post to work in either Fusion 360 or Inventor 2018 and have a question about using datum tables and cycle def 7 or 247.

    Here is the code it puts out.

    21 CYCL DEF 247 DATUM SETTING ~ I get an error 21 with no further explanation. I can't find a cycle 247. 7 yes but I get an incomplete cycl def if I change 247 to 7. I do want to use the datum table stored on the controller. This is as far as I was able to get on this one.
    Q339=1 ; DATUM NUMBER

    Thanks.

    Kevin V.
    Does G247 work in ISO?

    I'm guessing G247 or cycle 247 won't work on a TNC426. So you need to use Cycle 7 and in the machine parameters, MP7475 (use code number 123), set if the datum table is from machine zero or workpiece zero.

    If you have a newer TNC426 you maybe able to update the software to get cycle 247 working otherwise you need TNC530 or newer

    Also if you are using cycle 7 from a data table the format is

    10 CYCL DEF 7.0 DATUM SHIFT
    11 CYCL DEF 7.1 #1

    and you need to select the active datum table in PGM MGT

  7. #7
    Join Date
    May 2012
    Location
    Almont, Mi, USA
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    3

    Default

    No, In ISO you use a G53 P01 +1(+1 in place of G54) or 2, 3, etc. It assumes there is only one datum table, named Datum.d.

    I did change the MP7475 parameter from 0 to 1. Are you saying it should be 123?

    I did try to get an update from HH. They will only do it through Bridgeport, who for all intents and purposes here are defunct.

    I will try the proposed code above. I do like the ability to use conversational. It could be very productive on that controller. At which point do you use PGM MGT to select the active table?

  8. #8
    Join Date
    Jul 2005
    Location
    San Francisco, CA
    Posts
    802
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    80

    Default

    Quote Originally Posted by KevinV_MEI View Post
    No, In ISO you use a G53 P01 +1(+1 in place of G54) or 2, 3, etc. It assumes there is only one datum table, named Datum.d.

    I did change the MP7475 parameter from 0 to 1. Are you saying it should be 123?

    I did try to get an update from HH. They will only do it through Bridgeport, who for all intents and purposes here are defunct.

    I will try the proposed code above. I do like the ability to use conversational. It could be very productive on that controller. At which point do you use PGM MGT to select the active table?
    In ISO, G247 is the same as Cycle 247, if your control supports which yours doesn't, and G53 is the same as Cycle 7, when using datum tables.

    Not sure that it assumes there is only one datum table. Its probably you only have one and it was already selected. You can try it though... make a new datum table such as TEST.D, then hit the "program run" key, then "PGM MGT" key and then select TEST.D. If a M ends up behind it then that is the current active datum table.

    123 is the user code number (ie password) you should be using to enter into machine parameters.

    Let me know what your current NC software is and I will check what the newer version is.


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
  •