Need Help! Stop 4th axis from going home, EC400


Page 1 of 2 12 LastLast
Results 1 to 20 of 32

Thread: Stop 4th axis from going home, EC400

  1. #1
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Question Stop 4th axis from going home, EC400

    I need to get the tombstone to turn 90' and then stay there till I can drill, countersink, and tap with it in that position.

    I managed to get the tombstone to turn with a A90, and drill. But when it gets through with that drill and goes to get the next tool the G28 makes it go back to 0.

    There has to be a way to get it to stay till I tell it A0.?

    Similar Threads:
    Dennis


  2. #2
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    Eliminate the A0. from the G28 line.

    Mike

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  3. #3
    Member
    Join Date
    May 2012
    Location
    Sweden
    Posts
    100
    Downloads
    0
    Uploads
    0

    Default

    Is it the tool change program that makes the G28 ?
    When you program M6 ?



  4. #4
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    Oh I forgot to mention, there is no A0 or any A codes in my post at all.

    I have to place the A codes in manually. This old Teksoft dont do it for me.

    So what I did was put the A90 in the line with the G57 and that was all.
    I assumed it would stay at that position till I put A0 and the end of my program.

    Dennis


  5. #5
    Registered
    Join Date
    Feb 2010
    Location
    USA
    Posts
    1184
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by 34ford View Post
    I need to get the tombstone to turn 90' and then stay there till I can drill, countersink, and tap with it in that position.

    I managed to get the tombstone to turn with a A90, and drill. But when it gets through with that drill and goes to get the next tool the G28 makes it go back to 0.

    There has to be a way to get it to stay till I tell it A0.?
    Do not use G28. There are other methods to position clearance in Z.

    Time to break out the manual; G28 sends all axis to the home position.



  6. #6
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by haastec View Post
    Do not use G28. There are other methods to position clearance in Z.

    Time to break out the manual; G28 sends all axis to the home position.
    When you use G28 as below, it only sends the listed axis's home.

    G00 G91 G28 Z0.;

    Per this example, only Z would return to home as in a tool change.

    Mike

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  7. #7
    Registered
    Join Date
    Feb 2010
    Location
    USA
    Posts
    1184
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Machineit View Post
    When you use G28 as below, it only sends the listed axis's home.

    G00 G91 G28 Z0.;

    Per this example, only Z would return to home as in a tool change.

    Mike
    I agree 100% but I suspect that he is using just G28 by itself. My intent was to encourage him to look up how to use G28 properly.

    Perhaps maybe he could post part of his code?



  8. #8
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by haastec View Post
    I agree 100% but I suspect that he is using just G28 by itself. My intent was to encourage him to look up how to use G28 properly.

    Perhaps maybe he could post part of his code?
    Dang, messed you up, want me to edit it?

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  9. #9
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by haastec View Post
    Do not use G28. There are other methods to position clearance in Z.

    Time to break out the manual; G28 sends all axis to the home position.
    Thats the way Teksoft does just before each tool change, which works, just not now that I wanna keep this axis to stay put.
    I will take the G28's out tomorrow and see how it works.

    Dennis


  10. #10
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by 34ford View Post
    Thats the way Teksoft does just before each tool change, which works, just not now that I wanna keep this axis to stay put.
    I will take the G28's out tomorrow and see how it works.
    Teksoft may be trying to clear everything out of the way for a tool change, so just make sure nothing is in the way for a tool change.

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  11. #11
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    Yea, I will definitely make sure the tombstone is back first.

    Oh something I just thought of too. Teksoft always puts a Z0 at the end of each op and boy that is a disaster on a EC400.

    Feeds the tombstone into the spindle!

    Dennis


  12. #12
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by 34ford View Post
    Yea, I will definitely make sure the tombstone is back first.

    Oh something I just thought of too. Teksoft always puts a Z0 at the end of each op and boy that is a disaster on a EC400.

    Feeds the tombstone into the spindle!
    Sounds like you should ask for a different post processor.

    Mike

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  13. #13
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    I am about halfway afraid to remove the G28 because at this point it is whats parking the tombstone before a tool change.

    Unless there is a code specific for parking it.

    Dennis


  14. #14
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    All you have to do is run it a 5% rapid and watch it with your hand on the emergency button.

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  15. #15
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default

    As haastec said, post some of your code here.

    Mike

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  16. #16
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Machineit View Post
    As haastec said, post some of your code here.

    Mike
    +1



  17. #17
    Registered
    Join Date
    Feb 2012
    Location
    USA
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by haastec View Post
    I agree 100% but I suspect that he is using just G28 by itself. My intent was to encourage him to look up how to use G28 properly.

    Perhaps maybe he could post part of his code?
    the omitting of problematic coding is out of control!!! it should be a required field...

    ..have you tried sending Z to second home or tool change home?

    G91 G30 Z0
    G90



  18. #18
    Member extanker59's Avatar
    Join Date
    Mar 2008
    Location
    USA
    Posts
    638
    Downloads
    0
    Uploads
    0

    Default

    I have always prefered G53 Z0. Or G53 X-15. Y0 Z0 for a vertical mill that puts it closest to the operator in Y, and centered in X, and Z home. You can very easily put it anywhere you like.



  19. #19
    Member 34ford's Avatar
    Join Date
    May 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

    Default

    Here is how my posts typically end before the next tool. And that Z0 you see in there sends the work into the spindle. So I always delete it. For some reason on this EC400 the Z0 is not send to home.

    N65 X15.902
    N70 X18.264
    N75 G80 G00 Z5.
    N80 G54 G90 X18.264 Y-.75
    N85 G49 G28 Z0 M09
    N90 M01

    N95 (90' C.SINK)
    N100 T09 M06
    N105 S800 M03

    Dennis


  20. #20
    Registered
    Join Date
    Feb 2010
    Location
    USA
    Posts
    1184
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by 34ford View Post
    N85 G49 G28 Z0 M09
    The reason is that G49 cancels the length offset but not the work offset, so it tries to drive the face of the spindle to your G54 Z0 position.

    Fix your post pronto, because this will bite you in the a$$ sooner or later and it will not be pretty.

    If you just replace your G49 with G91, that combination of code will send Z axis to the home position. The combination of code is key!

    I am not trying to insult you with this question, but what is your experience level with G-Code programming? I know you are using Tek Soft, but how well do you understand the code it is producing?



Page 1 of 2 12 LastLast

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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Stop 4th axis from going home, EC400

Stop 4th axis from going home, EC400