New HAAS VF4 and canned cycles
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Sep 2019
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default New HAAS VF4 and canned cycles

    We have just recently taken ownership of a brand new VF4. Fantastic machine, but a few questions on basics. We have watched most of Mark and his tips of the day, but some things don't make sense to us. I know I could call haas and get these questions answered, but I figured I would try the collective on here and hopefully teach someone else a thing or two.

    1 - We purchased the option for a second home position. Is there a G or M code to utilize it at the end of the program? I could have the operator push the button on the HMI, but we would like to incorporate it into the program.

    2 - canned cycles and VPS - The VPS works great for us and can eliminate the constant need to use Mastercam to do simple hole patterns in our sheet metal parts. The issue we have is two fold. First, when the program starts, it goes directly to center then moves out to the first hole location, this issue dovetails into the second fold with this question. Clearance plane and feed plane. Maybe it is our mis-understanding of the "fill in the blank" parameters, but I cannot seem to find this out.Example below:

    Simple 6 hole pattern at 3 Inch diameter equal spaced. Spot drill first, the finish with a .050 Inch drill. Fixture holding with soft clamps holding the part to a chuck under it. some of the chucks have a "protruding center" in addition to the clamps.

    The wasted time that comes about with rapiding down to the clearance height then feeding at cutting feedrate until it finishes it drill then rapid back up to clearance height.

    In Mastercam, there are settings for clearance height and feed height. I set the clearance height to say 1 inch and the feed height to .010 Inch. It rapids down to .010 above the first hole (not center like the VF4 VPS is doing), drills, then rapids to the clearance height, moves to the next hole, rapids down to .010 Inch and drills. Rinse, lather repeat until finished.

    In The HAAS VF4 VPS, it would rapid down the the clearance, feed at the feedrate specified (say 10) through the whole inch, drill the hole, rapid back up to clearance and move to the second hole, then feed down at the feedrate.....wasted time!

    The canned cycle snippet generated gives me the following:

    S4000 M03
    G43 H02 Z0.5
    M08
    G82 G98 Z-0.01 F6. R0.5 P0. L0
    G70 I 2.06 J45. L8
    G80 Z0.5 M09
    G00 G90 G53 Z0 M05

    Where does the z value in G43 H02 Z0.5 come from. It seems to populate from the R value we input. Do we have to manually change this z value each time we program?

    Is there a way in the canned cycle to specify parameters for A) moving to the hole before rapid down to the feed plane to avoid hitting the center plug B) changing that z value.

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,416
    Post Thanks / Like
    Likes (Given)
    1473
    Likes (Received)
    1616

    Default

    Quote Originally Posted by CMSpinning View Post
    We have just recently taken ownership of a brand new VF4. Fantastic machine, but a few questions on basics. We have watched most of Mark and his tips of the day, but some things don't make sense to us. I know I could call haas and get these questions answered, but I figured I would try the collective on here and hopefully teach someone else a thing or two.

    1 - We purchased the option for a second home position. Is there a G or M code to utilize it at the end of the program? I could have the operator push the button on the HMI, but we would like to incorporate it into the program.

    Yes, there is a command for second home - G0G90G54P20(or your choosing)x0.y0.
    Not sure if there is a single command (other than the button on machine)
    see-
    https://www.haascnc.com/productivity/control/home.html

    also can use G54.xxx (look in your manuals)

    2 - canned cycles and VPS - The VPS works great for us and can eliminate the constant need to use Mastercam to do simple hole patterns in our sheet metal parts. The issue we have is two fold. First, when the program starts, it goes directly to center then moves out to the first hole location, this issue dovetails into the second fold with this question. Clearance plane and feed plane. Maybe it is our mis-understanding of the "fill in the blank" parameters, but I cannot seem to find this out.Example below:

    Simple 6 hole pattern at 3 Inch diameter equal spaced. Spot drill first, the finish with a .050 Inch drill. Fixture holding with soft clamps holding the part to a chuck under it. some of the chucks have a "protruding center" in addition to the clamps.

    The wasted time that comes about with rapiding down to the clearance height then feeding at cutting feedrate until it finishes it drill then rapid back up to clearance height.

    In Mastercam, there are settings for clearance height and feed height. I set the clearance height to say 1 inch and the feed height to .010 Inch. It rapids down to .010 above the first hole (not center like the VF4 VPS is doing), drills, then rapids to the clearance height, moves to the next hole, rapids down to .010 Inch and drills. Rinse, lather repeat until finished.

    In The HAAS VF4 VPS, it would rapid down the the clearance, feed at the feedrate specified (say 10) through the whole inch, drill the hole, rapid back up to clearance and move to the second hole, then feed down at the feedrate.....wasted time!

    The canned cycle snippet generated gives me the following:

    S4000 M03
    G43 H02 Z0.5 (initial point, typically 1" or 2" IME = G43H02Z2.)
    M08
    G82 G98 Z-0.01 F6. R0.5 P0. L0 (R= retract plane, set to .1 commonly) (G98 specifies return to initial (in G43 line) G99 returns to r plane, set here in your code as .5 (I highly recommend using G98 until you are comfortable with programming)
    G70 I 2.06 J45. L8
    G80 Z0.5 M09
    G00 G90 G53 Z0 M05

    Where does the z value in G43 H02 Z0.5 come from. It seems to populate from the R value we input. Do we have to manually change this z value each time we program?

    Is there a way in the canned cycle to specify parameters for A) moving to the hole before rapid down to the feed plane to avoid hitting the center plug B) changing that z value.
    See above text

  3. #3
    Join Date
    Sep 2019
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the quick reply. Very helpful.

    Where do we set the initial point? Is that something we are missing in the VPS screens?

    We are putting the following at the end of the program:

    T1 M06
    G53 G00 G90 Y0. X-25.3

    and it seems to work. The thing in my mind is:

    The canned cycles seem to get you 90% of the way there and then you can effectively adjust for optimizing the program. Meaning, I can generate the program, but then I have to adjust the initial Z point in each line, then add the two lines above at the end.

    Unless there is somewhere to add these to automatically whenever you generate a program.

  4. #4
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,340
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    681

    Default

    My 2 cents on this is "86" that VQC for programming. The only time I use this is probing or a quick thread mill (And even then I may just use a macro). It just seems all the guys/girls in the factory start finger fiddling with the VQC and it takes longer to bang it out by hand or could have just cammed it out. If you are doing mostly hole patterns and don't want to cam I suggest you take an online Macro class. Especially if you are somewhat new as that it is the best time to learn.

    As for the second home position, Don't like that either. Haas gives you 10 user programmable G codes free (G200-G210). Use those, you can make 10 home positions. Mine look something like

    G200 =
    "M9
    G53 Z0 M5
    G53 X (Whatever absolute sets table center) Y (Whatever absolute is at door)
    G80 G90
    M30"

    Or if you are using a rotary use the same thing above with different X and label it G201

    One simple G2xx can eliminate so much work in MDI or even the main program.

    There are so many convenient ways to use this feature and most Haas users don't even know they are there.

  5. Likes Booze Daily, SeymourDumore liked this post
  6. #5
    Join Date
    Sep 2019
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    g-coder05,
    At first, I was the same way, "the visual Programming (or VQC) will not be for us." We were strictly using Mastercam to handle all of our milling needs because we had a VF0 with a third party conversion (Creative evolution CNC) and it was loosely dos based with absolutely no canned cycle programming. Mastercam would handle all of that. The Next Gen controller, even with these minor shortcomings, drastically improved the programming time. As Mark says in the tip of the day videos, "just answer the questions". Being as the machine is a LOT newer then the VF0, right off the bat it is faster in production altogether.

    Perhaps a little more info on what we actually use the machine for should be added. The parts we are running through the machine are generally spun metal components like oil seal shells and cups. Think of a small cup with a .036 - .080 wall thickness. These parts need a very simple pattern of holes around the bottom. Those holes are usually just drain holes or holes in which the rubber that gets vulcanized to the part "grabs". For these applications, having to layout the hole pattern in CAD format within Mastercam, then calling the holes and adding the spot drill to it, then repeating the process for the .050 drill. In the VPS, maybe a dozen questions answered and your off to the races. If I have to do some complicated contouring or a hole pattern of 50 holes with varying sizes and off positions, then mastercam would win hands down.

    Putting the "home position" into one of the available gcode slots would make sense and I will probably do just that.

    Like I mentioned above. the canned cycles seem to ge you about 90% of the way there and some minor tweaks to optomize the time cycle still works for us. My guys are pretty well versed in G-code. They mostly run the st20 lathes that we have and they program those long hand, but even then, we have about a dozen different processes that happen and keeping shell programs and changing a few dimensions makes their work sort of a poor mans VPS.

    The two things that I still need some clarifiaction on are 1 - where does the initial z point come from? and 2 - can we have the machine move to the first hole before rapid down when program start?

  7. #6
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    699
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    286

    Default

    G-coder
    Could you go more into depth on the G200-G210 programming

    Thanks

  8. #7
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    89
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    18

    Default

    from the mill manual -

    Second Home - Press to rapid all axes to the coordinates specified in
    G154 P20

    I suppose you could simply command:

    G0 G90 G154 P20 Z0;
    X0 Y0;

    just be sure to set the second home position in the settings -> user positions tab

    checking this just now, it doesn't seem that setting the second home position sets a value in G154P20. I'll hafta get back to you on what the manual's talking about.

    the hard way is using macro values.
    G0 G90 G53 Z#20270;
    X#20268 Y#20269;

    i checked this and it works as I expect.

  9. #8
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    694
    Post Thanks / Like
    Likes (Given)
    103
    Likes (Received)
    361

    Default

    Quote Originally Posted by D.D.Machine View Post
    G-coder
    Could you go more into depth on the G200-G210 programming

    Thanks
    Aliased G (and M) codes.

    There's a tip of the day about it too. Here

  10. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,416
    Post Thanks / Like
    Likes (Given)
    1473
    Likes (Received)
    1616

    Default

    To the OP, you will find alot of good help here for Haas machines, but the fastest way to get what you want is to just google "Haas how to xxxxxxxxx" or go to youtube and type in the same query. Haas has a video for just about anything you can imagine, from how to set tool offsets and program to changing coolant....

  11. #10
    Join Date
    Sep 2009
    Location
    barcelona, spain
    Posts
    2,365
    Post Thanks / Like
    Likes (Given)
    525
    Likes (Received)
    1421

    Default

    Em..

    Hand code the absolutely most efficient program of say 6 holes on a diameter.

    Then check the total time vs a typical program time cam or vqc.
    Then vs a typical cam/vq program with the biggest timesaver corrected.

    Then value of the time saved vs production per day.
    Risks in terms of tools and crashes on hand-entered values.

    It is possible to hand code extremely fast and efficient programs.
    These can be easily built from macros.

    There is no "right" A. imho.
    Your volume, value-add, wip cost, are all critical path drivers with potential unforeseen exponential costs and risks.

    If You are doing 100/day and try to do 150, that is one thing.
    1000/d to 2000/d that is another.

    Clever programming is easy to do, but near impossible to maintain without lots of docs and operational experience.

  12. #11
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,340
    Post Thanks / Like
    Likes (Given)
    463
    Likes (Received)
    681

    Default

    Quote Originally Posted by D.D.Machine View Post
    G-coder
    Could you go more into depth on the G200-G210 programming

    Thanks
    Here's a post that goes a little more in depth.


    Aliasing G codes

  13. #12
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    89
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    18

    Default

    Quote Originally Posted by coyoinu View Post
    ...
    G0 G90 G154 P20 Z0;
    X0 Y0;

    checking this just now, it doesn't seem that setting the second home position sets a value in G154P20. I'll hafta get back to you on what the manual's talking about.
    it looks like G154 P20 has been deprecated in favor of settings 268-270.


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
  •