G75 facing feed - Page 3
Close
Login to Your Account
Page 3 of 3 FirstFirst 123
Results 41 to 45 of 45

Thread: G75 facing feed

  1. #41
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    259
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    34

    Default

    Hi Bill,

    Will try it out tomorrow.
    I think i do need N numbers before the New lines?

    I tried changing it by .8mm to get closer to the required dimension. I haven't used T10 so still needs dialing in.
    I double checked the Initial offset and it is fine. I just had a thought, i set the initial Offset for T10 from T2, Which has its offset initially set from T4. That could be the issue as T2 is 2 and a bit mm
    from T4.

    I will know for sure tomorrow!!!

    Cheers, Ken

  2. #42
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,899
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1574

    Default

    Quote Originally Posted by Kenre View Post
    Hi Bill,

    Will try it out tomorrow.
    I think i do need N numbers before the New lines?

    I tried changing it by .8mm to get closer to the required dimension. I haven't used T10 so still needs dialing in.
    I double checked the Initial offset and it is fine. I just had a thought, i set the initial Offset for T10 from T2, Which has its offset initially set from T4. That could be the issue as T2 is 2 and a bit mm
    from T4.

    I will know for sure tomorrow!!!

    Cheers, Ken
    Hello Ken,
    I only used T10 to make reference to the Tool Number during the discussion, I didn't mean that T10 should be used to call the Tool in the program; the trailing digits are required.

    If you're determining that the Offset is not being altered by Visual observation of an air gap between the Tool and Work (It is always about 3mm above diameter), you may nut be seeing the change by 0.8. Look at the Machine Coordinate System position display to see any variation in the positioning of the Tool when you alter the Offset.

    With regards to having Sequence Numbers, they are really only required on the Blocks that are referenced by P and Q in the Multi-repetitive Cycles and to Branch Destination Blocks using M99 P_ _

    where:
    _ _ = Sequence Number

    or, if your control is equipped with the User Macro Application, GOTO to Branch to a Sequence Number.

    Apart from the above, in my opinion, Sequence Numbers only consume memory.

    I suggest to clients to only use a Sequence Number at the Start of Each Tool Operation. I write a CNC program so that each Tool Operation is a Stand Alone Program and combined, make up the whole program.

    It would be a coincidence if all the tools used in a program were sequential, that is, T0101, T0202, T0303 etc. Because the Tool Numbers appear rather randomly in a program, its more intuitive, in my opinion, to know, or remember the Operation Sequence, rather than the Tool Number of each operation. Accordingly, I use Sequence Numbers at the start of each Tool Operation that relates to the Operation Sequence; N1, N2, N3, etc.

    When an operation needs to be rerun (to Dial in Size, Broken Insert, or for whatever reason), in Edit Mode, a search for the Operation Number is made and the operation run with confidence, knowing that each operation can run as a Stand Alone program. All that is difficult to do when each Block has a Sequence Number.

    When numbering the Start and End Blocks of the Profile Description used in the Multi-repetitive Cycles, I use numbers that have some relationship to the Sequence Number used that corresponds to the Operation Number for each Tool. For example, if the Sequence Number at the Start of the Tool Operation is N1 and a G71 Cycle is used in the Operation, I would use N111 and N112 for the Blocks that are at the Start and End, respectively, of the Profile Description. P and Q in the G71 Block would be P111 Q112. If the Tool Operation had a Sequence Number N2, then the P and Q Blocks would be P222 and Q223. And so it goes on; all other blocks in the Program would be without Sequence Numbers, as shown in the rehash of your program following.

    (80DEG. 0.8 RAD R/H T/TOOL)
    (ROUGH PROFILE)
    N1 G28 U0.0
    G28 W0.0
    T0100 G97 S2500
    G00 X-59.0 Z10.0 T0101 M08
    G01 Z1.0 F1000
    G71 U1.5 R2.0
    G71 P111 Q112 U-0.5 W0.15 F300 S2500
    N111 G00 X-28.0
    G01 Z-2.5 F200
    G01 X-55.0 R3.
    G01 Z-14.0
    N112 G01 X-59.0
    G00 Z10.0 M09
    G28 U0.0
    G28 W0.0
    M01
    (80DEG. 0.8 RAD R/H T/TOOL)
    (FINISH PROFILE)
    N2 G28 U0.0
    G28 W0.0
    T0200 G97 S2500
    G00 X-59.0 Z10.0 T0202 M08
    G01 Z1.0 F1000
    G70 P111 Q112
    G00 Z10.0 M09
    G28 U0.0 M05
    G28 W0.0
    M30

    Regards,

    Bill

  3. #43
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    259
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    34

    Default

    Bill,

    The radius worked a treat. Been stressing my brain to work out how to set it to R.5mm. The formulas i found are a bit beyond me atm. Is there a calculator that i can add the required dimensions to get a result?

    Cheers
    Ken

  4. #44
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,290
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    231

    Default

    ... and I thought it is a G75 thread

  5. #45
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    259
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    34

    Default

    G70,71,75.......

    All sorted!


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
  •