Newbie question, how to get part to come to door?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    33

    Default Newbie question, how to get part to come to door?

    Hi, I have a VF3 and I'm a total newbie to programming. Im making a part and at the end of the program when the part is done
    the table stays where the last cut ended. How do I get it to go to the door so I don't have to manually jog it to change the part out? What should the line of code look like at the end? Here is the code from the last tool used.

    ( TOOL 10: 1.5 DIA. ROUND OVER )
    S7500M3
    G90G54G0X-.559Y-.0044
    G43Z1.H10M8
    Z.5
    G1Z-2.25F50.
    G42X-.6575Y.0127D10
    G2X-.7389Y.1284I.0171J.0985
    I.7389J-.1284F100.
    X-.6233Y.2098I.0985J-.0172
    G40G1X-.5248Y.1927
    G0Z.5
    G91G28Z0.M9
    G90X0.Y0.M5
    M30

  2. #2
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    42
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    29

    Default

    You've got a couple things going on here I'd edit, but they're mostly harmless. Just change that G90 line to G28 and take the X out.

    G28Y0.M5, Instead of G90X0.Y0.

    If that brings the part up but the table is way off somewhere in X, just add an X# to after your G0 Z.5 line

  3. #3
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    33

    Default

    Thank you, I will try it after this next part finishes.

  4. #4
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    33

    Default

    Worked perfect, thanks for taking the time to help.

  5. Likes kustomizer, BGL liked this post
  6. #5
    Join Date
    Aug 2007
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    1,504
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    482

    Default

    Thank you for taking the time to let us know it worked

  7. Likes Booze Daily, BGL liked this post
  8. #6
    Join Date
    Sep 2011
    Location
    North Plains, OR
    Posts
    124
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    33

    Default

    If you use Fusion 360, the post processor for the Haas VF2 automatically writes the code to place the part front and center after the job is complete.

  9. #7
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by Turbo442 View Post
    If you use Fusion 360, the post processor for the Haas VF2 automatically writes the code to place the part front and center after the job is complete.
    I use Inventor HSM (same cam) and was pleasantly surprised to see this added in the program. However if you have an array of parts in multiple vises or a fixture it will still center table for part #1. I have been manually adding to the X dimension to compensate. Would be a nice add-on to the post processor to select "table center", "part center" or "overall travel center" or a predetermined number.

    Haas has figured out a way to charge big money for a button for the pre-determined XYnumber (it's just a damn button, some wire and the technology to prevent you from using it unless you pay).

    Glad to see cam software begin to add smart features for dumb machines. As they should.

    Haas is living their worst nightmare. Which is the new life being breathed into their old machines thru new software.

  10. #8
    Join Date
    Aug 2007
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    1,504
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    482

    Default

    I use G129 to bring my tables out to change parts.

  11. #9
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,960
    Post Thanks / Like
    Likes (Given)
    352
    Likes (Received)
    1959

    Default

    Quote Originally Posted by Tryhard View Post
    I use Inventor HSM (same cam) and was pleasantly surprised to see this added in the program. However if you have an array of parts in multiple vises or a fixture it will still center table for part #1. I have been manually adding to the X dimension to compensate. Would be a nice add-on to the post processor to select "table center", "part center" or "overall travel center" or a predetermined number.

    Haas has figured out a way to charge big money for a button for the pre-determined XYnumber (it's just a damn button, some wire and the technology to prevent you from using it unless you pay).

    Glad to see cam software begin to add smart features for dumb machines. As they should.

    Haas is living their worst nightmare. Which is the new life being breathed into their old machines thru new software.
    Oh
    MY
    GOD!!!

    Just what the [email protected] are some of you people going on and on about!!!

    just a button, dumb machines, worst nightmare, new life into an old machine, new software....

    Just what kind of "New" magic technology do you think Fusion 360 is employing that puts the damn table to the front?
    How'bout some of you sit down and learn a little bit of G-code, learn a little bit of your control ( Haas, Fanuc or wotever ), and learn a little bit about modifying your post processor!


    In this case, look at this amazing and incredible capability provided to you by EVERY CAM program:
    Instead of using G28 in any capacity ( useless for anything other than sending an axis home ), employ G00 G53 to send the machine to wherever you want to!

    So, edit the post that at the end of the program it spits out this:

    M09
    M05
    G00 G49 G53 X(wherever) Y0 Z0
    M30

    Friggin' magic!!!
    If your CAM program allows variables, then use the (wherever) variable to tell it where EXACTLY you want the table to be at!
    Last edited by SeymourDumore; 03-16-2020 at 12:35 AM.

  12. Likes Dupa3872, g-coder05 liked this post
  13. #10
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    1,026
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    441

    Default

    its a Haas
    Just write your own G code and run it at the end of your program ,,, I have one for centering the table in X and parking it at the door ,,, I wrote one to load T23 ( my chip fan ) and spin it up to S2000 then up to S7000 and drop down to 12" off the table and blow the full table in a pattern ...

    And I have one I use a lot that well park the table in X and Y. and turn the chip conveyor on and off with a dwell with it on for 15sec and off for a min and it runs for 5 min like that ,,, ( works great for 4th axis parts that produce a top of chips )

    It took a little screwing around to get all the bugs worked out of the programs , but you only have to write them "ONCE" after that its just like calling up a M08 but rather than turning the coolant on it runs what ever program or M code you wrote to the G code you wrote.

    YouTube

    Above link should make it clear

  14. #11
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by SeymourDumore View Post
    Oh
    MY
    GOD!!!

    Just what the [email protected] are some of you people going on and on about!!!

    just a button, dumb machines, worst nightmare, new life into an old machine, new software....

    Just what kind of "New" magic technology do you think Fusion 360 is employing that puts the damn table to the front?
    How'bout some of you sit down and learn a little bit of G-code, learn a little bit of your control ( Haas, Fanuc or wotever ), and learn a little bit about modifying your post processor!


    In this case, look at this amazing and incredible capability provided to you by EVERY CAM program:
    Instead of using G28 in any capacity ( useless for anything other than sending an axis home ), employ G00 G53 to send the machine to wherever you want to!

    So, edit the post that at the end of the program it spits out this:

    M09
    M05
    G00 G49 G53 X(wherever) Y0 Z0
    M30

    Friggin' magic!!!
    If your CAM program allows variables, then use the (wherever) variable to tell it where EXACTLY you want the table to be at!

    Why even bother to raise your blood pressure by clicking on thread titles which you make clear are beneath your golden input?

  15. Likes kustomizer liked this post
  16. #12
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,960
    Post Thanks / Like
    Likes (Given)
    352
    Likes (Received)
    1959

    Default

    Quote Originally Posted by Tryhard View Post
    Why even bother to raise your blood pressure by clicking on thread titles which you make clear are beneath your golden input?
    Are you seriously that dense?

    Are you really trying to defend these comments?

    I use Inventor HSM (same cam) and was pleasantly surprised to see this added in the program.
    Haas has figured out a way to charge big money for a button for the pre-determined XYnumber
    Glad to see cam software begin to add smart features for dumb machines.
    Haas is living their worst nightmare.
    Which is the new life being breathed into their old machines thru new software.

  17. #13
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,429
    Post Thanks / Like
    Likes (Given)
    394
    Likes (Received)
    637

    Default

    Quote Originally Posted by Tryhard View Post
    Why even bother to raise your blood pressure by clicking on thread titles which you make clear are beneath your golden input?
    Seymour is right.

    I just make a template .nc file that looks like this:

    Oxxxx

    G28 G91 G00 Z0.
    G53 G90 X-12. Y0.
    M30

    Copy and paste it to start a new program. Change the X value to whatever you want.

    First, the spindle goes to Z home, then to Y home (all the way out) and to your specified X value.

    Simple, consistent, and no worries about getting an overtravel alarm.

  18. #14
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by ChipSplitter View Post
    Seymour is right.

    I just make a template .nc file that looks like this:

    Oxxxx

    G28 G91 G00 Z0.
    G53 G90 X-12. Y0.
    M30

    Copy and paste it to start a new program. Change the X value to whatever you want.

    First, the spindle goes to Z home, then to Y home (all the way out) and to your specified X value.

    Simple, consistent, and no worries about getting an overtravel alarm.

    Thank you. You are absolutely correct and that is useful information for the original poster. But I wasn't the OP.
    My problem was I was thinking out loud with my comments related to modifying the post processor for inputting the final X location to be useful when running an array but I inadvertently triggered a luddite sjw.

    Lesson learned.
    Cheers all.

  19. #15
    Join Date
    Jan 2011
    Location
    South Florida
    Posts
    670
    Post Thanks / Like
    Likes (Given)
    68
    Likes (Received)
    126

    Default

    Not intending to piss anyone off, but if you don't know how to add a little code at the end of the program to bring the table where you want it you need to stop studying your CAD-CAM program and open your Haas manual. You need to know what that code means and how to modify your programs to improve and or correct them.

    Practice writing programs by hand until you learn basic code.

  20. Likes chiphook68, Tryhard, BGL liked this post
  21. #16
    Join Date
    Sep 2011
    Location
    Southern Indiana USA
    Posts
    167
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    79

    Default

    Here is the ending blocks of code I put in almost all my mill programs

    (Reset for next piece)
    G28 G91 Z0.
    G28 G91 Y0.
    G90
    M30

    If I want it to be somewhere beside the current X coordinate I use this code

    (Reset for next piece)
    G28 G91 Z0.
    G90 G0 G54 Xn.nnn (where G54 is whatever home you want to reference and Xn.nnn is whatever coordinate puts the table where tyou want it in the X)
    G28 G91 Y0.
    G90
    M30

    Lots of ways to skin this cat, but knowing how to write/edit G&M code is a good skill to acquire.

  22. Likes BGL, Tryhard liked this post
  23. #17
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,299
    Post Thanks / Like
    Likes (Given)
    860
    Likes (Received)
    1300

    Default

    I do the same, only I use them as subprograms. O9000 and O9001 specifically.
    Each machine has these subprograms in memory and they are specific to each machine.
    ie: 4 axis machine may have G91 G28 A0, 3 axis machine would not.

    The nice thing about this is the main program can be run on any mill with no editing.
    No need to do anything fancy, just edit your post to output M98 P9000/P9001 where appropriate.

  24. #18
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,670
    Post Thanks / Like
    Likes (Given)
    691
    Likes (Received)
    1042

    Default

    Are you seriously that dense?

    Are you really trying to defend these comments?
    I busted out on that one. I was trying to stay out of this but the fact my 15 year old Chinese female students understand this clearly and a programmer doesn't just solidifies my point of today's CNC programmers are really behind. (Nothing personal)

    All that useless rambling about Haas and home buttons made me dizzy. Haas makes it so simple, Perhaps read the manual on G code Aliasing?!? Create one single code (G200 for example).

    G200=
    G0 G90 G53 Z0 M8
    X (Absolute center of table) Y0 M5
    M30

    I absolutely detest the use of G28 and G91. No reason on newer controls (Including Fanuc) to put in incremental mode just to put it back in absolute. Ive seen a lot of nasty things when people are finger camming and miss a preparatory command at the beginning of a program or segment.

  25. Likes SeymourDumore liked this post
  26. #19
    Join Date
    Oct 2019
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    202
    Post Thanks / Like
    Likes (Given)
    21
    Likes (Received)
    26

    Default

    Quote Originally Posted by g-coder05 View Post
    I busted out on that one. I was trying to stay out of this but the fact my 15 year old Chinese female students understand this clearly and a programmer doesn't just solidifies my point of today's CNC programmers are really behind. (Nothing personal)

    All that useless rambling about Haas and home buttons made me dizzy. Haas makes it so simple, Perhaps read the manual on G code Aliasing?!? Create one single code (G200 for example).

    G200=
    G0 G90 G53 Z0 M8
    X (Absolute center of table) Y0 M5
    M30

    I absolutely detest the use of G28 and G91. No reason on newer controls (Including Fanuc) to put in incremental mode just to put it back in absolute. Ive seen a lot of nasty things when people are finger camming and miss a preparatory command at the beginning of a program or segment.
    You guys are confusing yourselves. The original poster was struggling with the program. I commented on my post processor not knowing the center of an array. Sure the button rant was semi off topic, but no reason to spew venom. ...at me or the original poster. Put it to rest geez.
    Cheers

  27. #20
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,429
    Post Thanks / Like
    Likes (Given)
    394
    Likes (Received)
    637

    Default

    Quote Originally Posted by g-coder05 View Post
    I busted out on that one. I was trying to stay out of this but the fact my 15 year old Chinese female students understand this clearly and a programmer doesn't just solidifies my point of today's CNC programmers are really behind. (Nothing personal)

    All that useless rambling about Haas and home buttons made me dizzy. Haas makes it so simple, Perhaps read the manual on G code Aliasing?!? Create one single code (G200 for example).

    G200=
    G0 G90 G53 Z0 M8
    X (Absolute center of table) Y0 M5
    M30

    I absolutely detest the use of G28 and G91. No reason on newer controls (Including Fanuc) to put in incremental mode just to put it back in absolute. Ive seen a lot of nasty things when people are finger camming and miss a preparatory command at the beginning of a program or segment.
    You're missing the point...

    I keep a .nc file with the code I posted above. To start a new program, I just copy and paste the file and start typing. It doesn't matter if the end of program code blocks are a foot long. You only type it once.

    Second, a lot of parts we run need to have the table positioned at different X locations for ease of load/unload. So if the operator complains and wants it moved 6 inches, just jump to the end of the program and edit the X value. Done.


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
  •