545,502 active members*
2,228 visitors online*
Register for free
Login
Results 1 to 6 of 6
  1. #1

    Haas - Get active radius offset possible?

    Hi, again. I was wondering if there is a simple way to access the active radius offset. I know there are the variables #2401- #2600 but this doesn't help me if I don't know which one is currently active. I guess I could add a D argument to the G65 macro and get the offset that way but I would rather not do that because then I would have to change a lot of programs. Also, the macro has a lot of arguments already so keeping it as simple as possible is a good idea, I think.
    So what do you think? Can it be done?

  2. #2
    Member
    Join Date
    Aug 2007
    Posts
    349

    Re: Haas - Get active radius offset possible?

    Hi,

    if the number of the spindle tool the number of the tool offset, you can read out the active spindle tool with #3026 and determine the actual tool diameter from it.
    #7=#[3200+#3026] alternatively #7=#[2400+#3026]+#[2600+#3026].

    Otherwise this should also be done using the last programmed D-parameter (#4107).
    It is important here that the D must have been called at least once before the macro call.
    #7=#[3200+#4107] alternatively #7=#[2400+#4107]+#[2600+#4107].

    I would map the D-parameter in the macro call as an optional parameter.
    G65 P.. X.. Y.. Z.. I.. [D..} {F..}

    ..
    N10 IF [#7 NE #0] GOTO12
    N11 #7=#3026
    N12…

    greetings eckitsch.

  3. #3

    Re: Haas - Get active radius offset possible?

    Hi, I think the vars #5041-##5042 do not have tool radius compensation,
    so by programming a simple linear move with active compensation at the begining you could compare the teoretical end position with the actual one and get the tool radius compensation.

    Lets say:

    G0 X0 Y0 Z0 (INITIAL POS)
    G1 X10 Y0 Z0 G41 (THE TEST MOVE END POS IS X=10,Y=0)
    #101=SQRT[[#5041-10]*[#5041-10]+[#5042-0]*[#5042-0]] (WE GET THE TOOL RADIUS COMP)

  4. #4

    Re: Haas - Get active radius offset possible?

    Right, that makes sense. I wonder tho how #3201-#3400 works in radius mode. The manual states specifically that it is the diameter of the tool where #2401-#2800 says diameter/radius. Maybe it's a typo?

    Either way =#[2400+#4107]+#[2600+#4107] should work in this case. If I understand it right it shouldn't matter if the D code came before or was used as an argument in g65, right?

    Thanks for the answer.

  5. #5

    Re: Haas - Get active radius offset possible?

    Humm. That sounds a bit sketchy, to be honest. And what happens if the radius is bigger than 10?

  6. #6

    Re: Haas - Get active radius offset possible?

    Quote Originally Posted by IsakAndersson View Post
    Humm. That sounds a bit sketchy, to be honest. And what happens if the radius is bigger than 10?
    it is sketchy XD

    even if the radius is bigger than 10 it "should" be in place at the end of the move.

Similar Threads

  1. Fanuc 3m radius offset confusion
    By EPS in forum Fanuc
    Replies: 1
    Last Post: 11-24-2016, 12:33 AM
  2. Fanuc OM Radius offset
    By pinguS in forum Fanuc
    Replies: 7
    Last Post: 04-06-2011, 02:33 PM
  3. Radius Offset and Length Offset
    By jim_stoll in forum Dolphin CAD/CAM
    Replies: 13
    Last Post: 10-15-2010, 01:47 AM
  4. TL25 Haas Lathe active tooling
    By alphamoose in forum Uncategorised MetalWorking Machines
    Replies: 1
    Last Post: 09-19-2008, 11:02 AM
  5. machinemate tool radius offset ???
    By jeffsnure in forum General CNC (Mill / Lathe) Control Software (NC)
    Replies: 0
    Last Post: 04-30-2008, 03:18 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •