Haas -- FANUC Macro compatibility?
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,397
    Post Thanks / Like
    Likes (Given)
    384
    Likes (Received)
    626

    Default Haas -- FANUC Macro compatibility?

    I'm hoping to improve myself by learning macro programming. If I learn a little more, I'll know just enough to be dangerous....

    My question is, how cross-compatible is a FANUC macro manual with a Haas machine? I understand some of the variables might(?) do different things, but the structure is the same, right?



    This is the book I was thinking about getting. https://www.amazon.com/Fanuc-Custom-...a-458001799679

  2. #2
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,423
    Post Thanks / Like
    Likes (Given)
    11691
    Likes (Received)
    3921

    Default

    Get the Smid Book, 100%.

  3. Likes ChipSplitter liked this post
  4. #3
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,511
    Post Thanks / Like
    Likes (Given)
    1730
    Likes (Received)
    2162

    Default

    I think before I spent $60 I would go to the Renishaw site and download their inspection plus pdf docs. If that is not enough, then maybe buy the book...

  5. #4
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,633
    Post Thanks / Like
    Likes (Given)
    1208
    Likes (Received)
    672

    Default

    I know that I carry on about it but I have this one https://www.amazon.com/S-K-Sinha/dp/...N7Y3GVH915CMXA

    It was pricey for me but really helped and still helps. Even in the Authors foreword he says that it is meant to be read textbook style... So to run from basics to more advanced macros. I still use it to back track every now and again.
    The author even sent me extra variables that were not in my edition once I purchased it and I just stuck them in the back.

  6. Likes gregormarwick liked this post
  7. #5
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,290
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    231

    Default

    Quote Originally Posted by NAST555 View Post
    I know that I carry on about it but I have this one CNC Programming using Fanuc Custom Macro B: Sinha, S.K: 9780071713320: Amazon.com: Books

    It was pricey for me but really helped and still helps. Even in the Authors foreword he says that it is meant to be read textbook style... So to run from basics to more advanced macros. I still use it to back track every now and again.
    The author even sent me extra variables that were not in my edition once I purchased it and I just stuck them in the back.
    Thank you NAST555 for your nice words about the book.

    In the new reprint of the book, several appendices have been added, including one for macro variables. It is really helpful to have a complete list at one place, with reference page numbers for their description. Some typos also have been corrected.

    If you are purchasing the book, look for appendices C, D and E at the back. If not found, ask for the newer version, or PM me to mail you the extra material.

    Smid's book is good, but, for i-series controls, mine is better. Ask somebody who has seen both the books,

  8. Likes NAST555 liked this post
  9. #6
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,397
    Post Thanks / Like
    Likes (Given)
    384
    Likes (Received)
    626

    Default

    Bump, bump, bump.

    Thanks for the book recommendations.....

    But I still don't know the answer to my original question.

    Pinging Wheelie, litlerob1, Mike1974, TMP, or anyone else that knows Haas macros.

  10. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,889
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1565

    Default

    Quote Originally Posted by ChipSplitter View Post
    Bump, bump, bump.

    Thanks for the book recommendations.....

    But I still don't know the answer to my original question.

    Pinging Wheelie, litlerob1, Mike1974, TMP, or anyone else that knows Haas macros.
    Hello ChipSplitter,
    For the most part, the Fanuc and Haas User Macro language can be considered the same. Local, Common Volatile and Common Nonvolatile Variables are the same. Many of the System Variables considered to be standard are the same.

    There are a lot of Fanuc System Variables available that are not listed in the Fanuc Manual. The reason for this is that Fanuc supply their controls to many different MTBs and its the responsibility of the MTB as to whether additional System Variables are supplied or not. As Haas is both the supplier of the Software and the MTB, many additional System Variables are available.

    One major difference between the Fanuc and Haas System is that Haas supply a "G" Code to set, or limit the number of Look Ahead Blocks. By specifying G103 with a P address in the range of 1 to 15, the number of Look Ahead Blocks is limited to the number specified by the P address. If P0 is specified, or G103 is included in a Block with the P address omitted, then Look Ahead Limiting will be disabled. The Fanuc System doesn't have this feature and a Work Around must be employed when the Look Ahead must be stopped.

    Being able to stop the Look Ahead Block is very important in some circumstances. For example, if you needed to get the Current Machine Position at the end of a move, then you may think that the following would suffice:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    #1=#5023
    ------
    ------
    ------
    ------

    If in the above example the Workshift for Z in G54 is -210.123 and the Tool Length Offset registered for H01 is 85.60, then the Machine Position in Z at the Absolute Z10.0 position will be -114.523. Accordingly, one may expect that #1 will take on this value when it reads the System Variable #5023. Not so. In fact, the result of the above code is likely to be a value of circa -0.10 being registered in Local Variable #1. To get the desired result, the above code would have to be rewritten as follows:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    G53 (or G31)
    #1=#5023

    The above code will stop the Look Ahead before #1=#5023 is executed and ensures that the G43 Z10.0 H01 is completed before #5023 is read.

    Regards,

    Bill

  11. Likes ChipSplitter liked this post
  12. #8
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,397
    Post Thanks / Like
    Likes (Given)
    384
    Likes (Received)
    626

    Default

    Quote Originally Posted by angelw View Post
    Hello ChipSplitter,
    For the most part, the Fanuc and Haas User Macro language can be considered the same. Local, Common Volatile and Common Nonvolatile Variables are the same. Many of the System Variables considered to be standard are the same.

    There are a lot of Fanuc System Variables available that are not listed in the Fanuc Manual. The reason for this is that Fanuc supply their controls to many different MTBs and its the responsibility of the MTB as to whether additional System Variables are supplied or not. As Haas is both the supplier of the Software and the MTB, many additional System Variables are available.

    One major difference between the Fanuc and Haas System is that Haas supply a "G" Code to set, or limit the number of Look Ahead Blocks. By specifying G103 with a P address in the range of 1 to 15, the number of Look Ahead Blocks is limited to the number specified by the P address. If P0 is specified, or G103 is included in a Block with the P address omitted, then Look Ahead Limiting will be disabled. The Fanuc System doesn't have this feature and a Work Around must be employed when the Look Ahead must be stopped.

    Being able to stop the Look Ahead Block is very important in some circumstances. For example, if you needed to get the Current Machine Position at the end of a move, then you may think that the following would suffice:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    #1=#5023
    ------
    ------
    ------
    ------

    If in the above example the Workshift for Z in G54 is -210.123 and the Tool Length Offset registered for H01 is 85.60, then the Machine Position in Z at the Absolute Z10.0 position will be -124.523. Accordingly, one may expect that #1 will take on this value when it reads the System Variable #5023. Not so. In fact, the result of the above code is likely to be a value of circa -0.10 being registered in Local Variable #1. To get the desired result, the above code would have to be rewritten as follows:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    G53 (or G31)
    #1=#5023

    The above code will stop the Look Ahead before #1=#5023 is executed and ensures that the G43 Z10.0 H01 is completed before #5023 is read.

    Regards,

    Bill

    Thank you Bill. That makes sense.

  13. #9
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,889
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1565

    Default

    Quote Originally Posted by ChipSplitter View Post
    Thank you Bill. That makes sense.
    Hello ChipSplitter,
    A correction to my previous Post is required.
    "at the Absolute Z10.0 position will be -124.523", should be "at the Absolute Z10.0 position will be -114.523"; I omitted to take into account the Z10.0, the machine Position would be -124.523 if the Absolute Coordinate were to be Z0.0

    Regards,

    Bill

  14. #10
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,290
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    231

    Default

    Quote Originally Posted by angelw View Post
    Hello ChipSplitter,
    For the most part, the Fanuc and Haas User Macro language can be considered the same. Local, Common Volatile and Common Nonvolatile Variables are the same. Many of the System Variables considered to be standard are the same.

    There are a lot of Fanuc System Variables available that are not listed in the Fanuc Manual. The reason for this is that Fanuc supply their controls to many different MTBs and its the responsibility of the MTB as to whether additional System Variables are supplied or not. As Haas is both the supplier of the Software and the MTB, many additional System Variables are available.

    One major difference between the Fanuc and Haas System is that Haas supply a "G" Code to set, or limit the number of Look Ahead Blocks. By specifying G103 with a P address in the range of 1 to 15, the number of Look Ahead Blocks is limited to the number specified by the P address. If P0 is specified, or G103 is included in a Block with the P address omitted, then Look Ahead Limiting will be disabled. The Fanuc System doesn't have this feature and a Work Around must be employed when the Look Ahead must be stopped.

    Being able to stop the Look Ahead Block is very important in some circumstances. For example, if you needed to get the Current Machine Position at the end of a move, then you may think that the following would suffice:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    #1=#5023
    ------
    ------
    ------
    ------

    If in the above example the Workshift for Z in G54 is -210.123 and the Tool Length Offset registered for H01 is 85.60, then the Machine Position in Z at the Absolute Z10.0 position will be -114.523. Accordingly, one may expect that #1 will take on this value when it reads the System Variable #5023. Not so. In fact, the result of the above code is likely to be a value of circa -0.10 being registered in Local Variable #1. To get the desired result, the above code would have to be rewritten as follows:

    G90 G54 X0.0 Y0.0
    G43 Z10.0 H01
    G53 (or G31)
    #1=#5023

    The above code will stop the Look Ahead before #1=#5023 is executed and ensures that the G43 Z10.0 H01 is completed before #5023 is read.

    Regards,

    Bill
    Nowhere in the Fanuc manuals it is mentioned that G31 will stop look ahead.
    It is the finding of Bill. Such a simple solution.
    He has been generous enough to share such a useful information with all of us.
    We all are grateful to him.


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
  •