G112 breakdown - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 29 of 29

Thread: G112 breakdown

  1. #21
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,723
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1467

    Default

    Quote Originally Posted by rainman View Post
    Well, that may well be, but I've had very unreliable results if I don't position to C0 prior to entering polar mode. Maybe it's just our machine, but the only way to get predictable results is to start at C0, then enter polar mode.
    Hello rainman,
    Your experience is not typical. Following is also an extract directly from a Fanuc manual:

    "The virtual axis is at coordinate 0 immediately after G12.1 is specified.
    Polar interpolation is started assuming the angle of 0 for the position of
    the tool when G12.1 is specified."

    Its because of this that the warning to move to C0 before entering Polar Mode is made, but there is absolutely no requirement to always start at actual C0.

    This aspect can be used to advantage when there is a repeat of a feature around the part. As C0 is always assumed when initiating Polar Mode, Polar Mode can be exited at the completion of the feature, rapid the C axis to the next start position and the same code that uses Polar Mode for the feature executed again. I have a few clients that use Polar Mode in this manner quite seamlessly.

    Your HAAS example in your last Post is just that, an example. Sure, you can change the C0.0 position by using a Workshift Offset, but that is not what your HAAS example does in the following extract.

    M154 (ENGAGE C AXIS)
    G28 H0 (HOME C AXIS)

    In this example, C Axis Machine Zero is being used and not all job are going to lend themselves to starting the feature being machined in Polar Mode at C Axis Machine Zero. If you dig down, you will find that you can start at any C axis coordinate; its just that when you enter Polar Mode, C0.0 position is assumed, as put by the extract from the Fanuc Manual above.


    Regards,

    Bill

  2. #22
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    1

    Default

    you guys are awesome. never disappoint!! i ended up creating a hex in gibbs, putting the radius on the corners, and am now trying to pick apart the code and figure out exactly how it works, the one without rads will be huge for me so thank you Bill. your a wizard. again thank you all for the insight.

  3. #23
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    361
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    94

    Default

    Quote Originally Posted by angelw View Post
    In this example, C Axis Machine Zero is being used and not all job are going to lend themselves to starting the feature being machined in Polar Mode at C Axis Machine Zero. If you dig down, you will find that you can start at any C axis coordinate; its just that when you enter Polar Mode, C0.0 position is assumed, as put by the extract from the Fanuc Manual above.

    Bill
    That's fine if you're only doing one polar tool path, not needed to be oriented to anything else. But what happens if you need to maintain orientation to other milled or drilled features? If C0 is assumed at start point, won't the polar feature be mis-oriented to the rest of the part?

  4. #24
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,723
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1467

    Default

    Quote Originally Posted by rainman View Post
    That's fine if you're only doing one polar tool path, not needed to be oriented to anything else. But what happens if you need to maintain orientation to other milled or drilled features? If C0 is assumed at start point, won't the polar feature be mis-oriented to the rest of the part?
    Quite the opposite. If another feature, drilled hole etc., is at C0.0 and the feature using Polar Mode is at, say, C30.0, one would simply rapid to C30.0 before initiating Polar Mode. When Polar Mode is invoked, C0.0 is assumed, irrespective of where the C axis may be, and the Polar Mode program code starts at C0.0. You want another different Polar Mode feature at another location, say starting at C73.5? Simply rapid to C73.5 with Polar Mode cancelled, initiate the new Polar Mode Program that again starts at C0.0. Fairly simple really.

  5. #25
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    361
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    94

    Default

    OK, so I assume you're correct about this, but I've never had to do it. Hard to make CAM do that anyway. What I've always done is rapid to X0Y0C0, clear of the part in Z. Then invoke G112, then feed at a high feed rate to the starting point (say, G1X1.12C.25F150.). Then feed down and proceed with tool path. It's always worked, and maintained orientation to other features. And in CAM, I need not worry about where I'm starting in C.

  6. #26
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    1

    Default

    so to check in, i was able to cut a .5 hex into some 6061 after turning it down, so success!!! my next projects will be learning to cut to flats on a bar, and cutting squares. which im sure ill be in here asking more questions. your discussion on C location prior to G112 is interesting. wouldn't if doing any work where you need a c axis to time certain features, would it not be best to always just start out at C0.? and just keep whatever feature you cut as a reference for everything else? so say i broach a keyway, than want to drill and tap into said keyway than cut a hex or some other feature my key is now virtually C0. and my drill/tap will also be positioned at C0., than if needed when going into G112 i can orient the spindle any way by doing math of how i want hex to start?

  7. #27
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,723
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1467

    Default

    Quote Originally Posted by rainman View Post
    OK, so I assume you're correct about this, but I've never had to do it. Hard to make CAM do that anyway. What I've always done is rapid to X0Y0C0, clear of the part in Z. Then invoke G112, then feed at a high feed rate to the starting point (say, G1X1.12C.25F150.). Then feed down and proceed with tool path. It's always worked, and maintained orientation to other features. And in CAM, I need not worry about where I'm starting in C.
    How in the World is it going to be hard to make a CAM system do it the way I've suggested it can be done? When Polar Mode is invoked, C0.0 is assumed, period. Accordingly, all of your Polar Mode features are going to start at C0.0, period (programmatically speaking). So the CAM system will create the feature starting at C0.0 irrespective of how you want to get to the actual start angle in C. Simply rapid to the C Start Angle with Polar Mode cancelled, then initiate Polar Mode and the program starts at C0.0, end of story; simple.

  8. #28
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Haas X in Polar

    Quote Originally Posted by rainman View Post
    I am 99% sure that Haas uses radius for X axis in polar.
    Yes, Haas does use radius for X axis in polar.

  9. #29
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    714
    Post Thanks / Like
    Likes (Given)
    105
    Likes (Received)
    377

    Default

    Our Tsugamis were set up to use radius in Polar mode as well - must be a FANUC parameter. Both 0i and 32i controllers.


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
  •