End of Program Routine


Results 1 to 12 of 12

Thread: End of Program Routine

  1. #1
    Registered
    Join Date
    Mar 2011
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default End of Program Routine

    Hello,
    I'd like some input on a good end of program routine.

    I'm using a Fadal 88HS
    Format 2
    I use E1-Exx fixture offsets

    I set tool lengths and use a Z-xx.xx in the fixture offsets so I only have to set the tool length once for different fixtures. I set the Z0.0 to the top of the part and calculate that for the Z fixture offset.

    It's a 40x20 table and I'd like the table to move forward at the end of program.

    Here is what I am doing now:
    N65 G0 Z.1
    N66 M5 M9
    N67 G53 Z0.H0
    N68 G53 Y9.5
    N69 M30
    %

    After the program ends, the spindle moves down from its home position the distance of the tool length offset.

    I'd like to know why it does that and find a better way of doing it.

    Thanks for your help.
    Ken

    Similar Threads:


  2. #2
    Member chippslinger's Avatar
    Join Date
    Nov 2008
    Location
    USA
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default

    We have a 2000 Fadal3016 and we end all programs with G0G90E0X0Y0Z0



  3. #3
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    53
    Downloads
    0
    Uploads
    0

    Default

    Ken,
    Do you leave the Z zero set to the cold start position? I set all tool lengths from a probe but they could also be set from a common block from the machine table. That way you would have to only use the difference from the block height to the Z zero plane of your part in your fixture offset. My ending lines make a clean move to home. The only thing you have to watch for is that if your Z fixture offset amount is greater than 4.0 inches and you position X Y & E on one line then Z with H on the next the head will try to move in the plus direction greater than it's physical traval on the X,Y position line. I get around this by always positioning X, Y, Z, H, and E all on the first line after a tool change.

    M6T1
    M1
    M3S2600
    G0 G90 X1. Y-1.2 Z1. H1 E1
    Z.1 M8
    ~~~
    G0M5M9Z1.
    X0Y0Z0E0H0
    M2
    %

    I noticed that you had your Y axis move in a more comfortable part change position. I set machine home position to X0 Y9. Z0 from the cold start position.

    I hope this long winded explanation helps!
    Jim



  4. #4
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    G80
    M05M09
    G91G28Z.0
    G0G90E0X-10.Y9.9
    M19
    M30
    %

    www.integratedmechanical.ca


  5. #5
    Registered
    Join Date
    Mar 2011
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default

    Here is how I currently set up tools and fixtures.
    I don't change the XYZ home. It is still at Cold Start.

    I have touched the spindle face to a fixed object on the table and noted that Z value.
    When I place a new tool, I touch it to the same point.
    The difference in Z is the tool length. I enter that in the table as a positive number. (typically 3-7 inches depending on tool)

    I have a touch probe that I keep in the turret. I determined its length as per the other tools (for example 5.0").

    To determine the Z0.0 of the part, I touch the probe to the Z0.0 point, then note the Z reading with out any offsets (Z-15.0" for example). I increase this number by the length of the probe. The fixture Z offset is then 15.0+5.0=20.0. The spindle face is 20.0 from the top of the part. I enter this as a negative value in the Fixture table. ie:X5.0, Y4.0, Z-20.0.

    This system has worked for me. I don't have to set each tool for each new part. I do a lot of short run stuff and like to keep some basic tools in the turret and not have to reset them each time.

    I just need the best way to end the program without any extra movements.

    What would be the best way to park the Z given my set up?

    EDIT: After reviewing the manual and these responses, I think I am going to try using G28.

    Thanks for your input.
    Ken



  6. #6
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by HRWmfg View Post
    What would be the best way to park the Z given my set up?

    Ken

    G91G28Z.0

    www.integratedmechanical.ca


  7. #7
    Registered
    Join Date
    Mar 2011
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default

    Incremental Move?



  8. #8
    Registered
    Join Date
    May 2005
    Location
    usa
    Posts
    53
    Downloads
    0
    Uploads
    0

    Default

    Are you running the machine in format 2?
    G91G28Z0 is a tried and true way to send the Z axis home with a Fanuc control. I run our machine with format 1 and use a Z value in the fixture offset and a tool length offset similar to what you are doing.
    My ends shut off all offsets with no "extra" moves.
    As you are using a Z value in your fixture offset and a tool length offset you may want set your rapid overide to 25% and have your finger on the slide hold.

    G0 G90 Z1. M5 M9
    X0Y0Z0E0H0
    M2
    %

    I don't know if you could add a X and Y value in the last position line and have the machine park in a convient way to change parts.

    Last edited by Techman; 05-18-2011 at 12:57 PM. Reason: Grammer


  9. #9
    Monkeywrench Technician DareBee's Avatar
    Join Date
    Jan 2004
    Location
    Stratford, Ont. Canada
    Posts
    3154
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Techman View Post
    I don't know if you could add a X and Y value in the last position line and have the machine park in a convient way to change parts.
    Of course you can.

    See my first post.
    Every program I run (format 2) gets the end grouping I posted.
    Different fixtures get a different XY park position.

    G91 - yes - believe me, I thought it was weird to use incremental and I have experimented and I always get a Z over-run when not using G91G28Z0

    www.integratedmechanical.ca


  10. #10
    Registered
    Join Date
    Mar 2011
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default

    I'll try the G91G28Z0

    It did NOT like G28Z0H0

    Thanks for your input.
    Ken



  11. #11
    Registered carbidecraters's Avatar
    Join Date
    Apr 2005
    Location
    USA
    Posts
    1194
    Downloads
    0
    Uploads
    0

    Default

    How we have been doing it for almost 20 years


    Simple program end

    M5M9
    Z0H0G0
    M30

    Why G28? Z0 H0 is machine cold start zero anyways.

    We have had good luck with our Fadals milling mostly soft steel and aluminum up to 5 axis. We are always looking for spare parts :) If you have a broken down Fadal give a shout.


  12. #12
    Registered
    Join Date
    Oct 2010
    Location
    usa
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default

    Ken,
    We have a few older Fadals
    88HS format 2

    We have always set the tool length from the tip of the tool to the top of a reference surface (we use the top of the 4th axis on the machines.. its just convenient, and still there when changing dull tools later)
    the result is a negative tool length value in the offset

    Place the difference between reference surface, and the part zero, in the fixture offset.

    typical tool paragraph

    M6T2
    E1 G90 G0 X0 Y0 S1200 M3
    G43 H2 Z.15 M8
    .
    .
    .
    .
    G80 M9
    M6
    M1
    When finished using a tool we use M6...
    it shuts off the spindle, cancels tool offset, and returns the head back to the tool change position....

    At the end of program

    G80 M9
    M6
    E0 G90 G0 X0 Y10. ( change X and Y to any machine position for part change convenience, this Y move places the table closest to the operator )
    M30

    This works for us.



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

End of Program Routine

End of Program Routine