Renishaw Probing Routines and Work Offsets
Close
Login to Your Account
Results 1 to 6 of 6
  1. #1
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Renishaw Probing Routines and Work Offsets

    I am trying to understand how the Renishaw macros deal with work offsets.

    Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

    Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

    Something like this:

    G65 P9832
    G65 P9811 Z-.5 S1.
    (Maybe Something here to get make the protected move in G54)
    G65 P9810 Z1.25 F150.


    I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

    If it matters this is a Haas NGC with WIPS.

    Thank you!

  2. #2
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    335
    Likes (Received)
    330

    Default

    Quote Originally Posted by swinthrope View Post
    I am trying to understand how the Renishaw macros deal with work offsets.

    Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

    Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

    Something like this:

    G65 P9832
    G65 P9811 Z-.5 S1.
    (Maybe Something here to get make the protected move in G54)
    G65 P9810 Z1.25 F150.


    I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

    If it matters this is a Haas NGC with WIPS.

    Thank you!
    Many ways to do this, here is one. The protected move does need a work offset, so can't be used at the beginning of a sequence. But generally, the first P9811 (single position measure) should start .500" (10MM) above the surface.

    G65 P9832
    G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
    G00 G54 Z2.0 (Maybe Something here to get make the protected move in G54) (If you are comfortable, you do not need a protected move here.)
    G65 P9810 Z1.25 F150.

    Paul

  3. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    818
    Post Thanks / Like
    Likes (Given)
    464
    Likes (Received)
    790

    Default

    Quote Originally Posted by LockNut View Post

    G65 P9832
    G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
    G00 G54 Z2.0 (Maybe Something here to get make the protected move in G54) (If you are comfortable, you do not need a protected move here.)
    G65 P9810 Z1.25 F150.

    Paul

    I'm thinking something like this


    G65 P9832
    G65 P9811 Z-.5 S1. (You have just set a Z work offset here using G54)
    G00 G54
    G43 H25 Z1.25 (use probe tool offset no.)

    G65 P9810 Z1.25 F150.

  4. Likes LockNut liked this post
  5. #4
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    821
    Post Thanks / Like
    Likes (Given)
    978
    Likes (Received)
    529

    Default

    Quote Originally Posted by swinthrope View Post
    I am trying to understand how the Renishaw macros deal with work offsets.

    Generally, I would like to understand how the macros such as G65 P9810 deal with work offsets and if there is a way to alter their default behavior. They appear to operate in their own pseudo offset plane where X0,Y0,Z0 are the position of the spindle when the macros are run. I would like to find a way to get them to work from some offset - G53, G54, etc.

    Specifically I would like to jog the machine over a fixture, probe G54 Z off of a fixture, then do a protected move up to 1.25" off of the newly found Z0.

    Something like this:

    G65 P9832
    G65 P9811 Z-.5 S1.
    (Maybe Something here to get make the protected move in G54)
    G65 P9810 Z1.25 F150.


    I am also open to any other options to end up with the same result, but whatever solution must provide a Z at a very specific height relative to the fixture for further probing moves otherwise I will miss surfaces.

    If it matters this is a Haas NGC with WIPS.

    Thank you!
    Here you go. This is a bit of code we use for the same thing, modified for your purpose.

    T24 M06
    T2
    G00 G90 G54 X0 Y0
    G43 H24
    G00 Z1.25
    G65 P9832
    G65 P9810 Z0. F50.
    G65 P9811 S2. Z0
    G65 P9810 Z1.25 F50.
    G65 P9833
    G28 G91 Z0
    M01

  6. #5
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    584
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    295

    Default

    Lot of bad examples up in here.

    It sounds like he wants to jog above the fixture, then set the offset similar to how you use WIPS.

    If there is no existing workoffset, you wont be using 9811. P9811 assumes the offset is already set and needs updating.

    You should know how far you want to go to set your offset, not just blindly use P9811 Z0 and see how far it goes, up or down. Sloppy.

    Set your offset first, then update it. Like how WIPS works, tell it how far to go to reach the expected surface.


    How far above are you starting?
    #1= 0.5

    #5223= #5023-#[2000+#3026]-#1
    G43H#3026
    G65 P9832
    G65 P9811 Z0 S1.
    G65 P9810 Z1.25
    G65 P9833
    M30

  7. #6
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    504
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    85

    Default

    Few general remarks:
    1. Any of Inspection Plus commands will generate alarm, when no active tool length offset compensation is set in the machine (G43H ***). It does not distinct which offset is set (probe or any other tool), so be sure that probe offset is active.
    2. The routines UPDATE rather then SET the WCS. While measuring the bore for example, the actual WCS coordinates are updated by the X Y distances between starting point and measured center point. If one wishes to set X0 Y0 at this point, the X0 Y0 must be set prior to measurement at starting point.


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
  •  
2