549,879 active members*
1,652 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Haas Machines > Haas Mills > VF 1 Cutter Comp for tool diameter
Results 1 to 5 of 5
  1. #1
    Registered
    Join Date
    Jul 2011
    Posts
    3

    Question VF 1 Cutter Comp for tool diameter

    I have a Haas VF1 and just loaded a .5" SQEM that had a actual dia. was .5024. All my parts are coming out to small on the OD. I am not sure how I compensate for that over size. If there is a process I need to go through on my offset page or not. Looking for some direction. I have turned cutter comp on in my posted file using G41 but not sure if that is all I need to do.

    There are a few lines of the code for this tool



    G20 G40 G80 G90 M09
    G103 P0
    T02 M06
    M01
    S10000 M03
    G43 H02
    (msg,watchforair)
    M08
    M83
    G00 G90 X.135 Y-.9827
    Z.2631 M08
    G01 Z.0731 F30.
    G41 Z-.0269 F15. D00
    X.1352 Y-.6318
    X.1163 F30.
    G02 X-.0001 Y-.6177 I.0057 J.5328

    Not sure if the D00 is correct or not. I use a probe to set all my tools length and diameter.

    Any direction I can get would be greatly appreciated...

    Thanks

    Steve

  2. #2
    Flies Fast
    Join Date
    Dec 2008
    Posts
    2864

    Re: VF 1 Cutter Comp for tool diameter

    Ideally, most program using the tool number(Tx), matching the tool length offset number(Hx), matching the tool dia/radius offset number(Dx).
    If on some machines this is not possible, then the one that is dropped is the diameter offset number (which may be staged a constant number higher ie T1 H1 D31)
    D00 is a non editable offset that is permanently set to zero.
    This D(number) needs to be edited to another number, and then that number field can hold your tool adjustment.
    It looks as if you program tool centreline paths, if you do, then a +ive number makes the tool stay further away, -ive makes it pass closer
    Some machines a diameter input, some a radius value. Try inputting a value of +0.0024, if it cuts correct size, your machine takes a diameter value,... halve the value if your part is oversize.

  3. #3
    Member
    Join Date
    Jan 2005
    Posts
    13253

    Re: VF 1 Cutter Comp for tool diameter

    Quote Originally Posted by Steven E View Post
    I have a Haas VF1 and just loaded a .5" SQEM that had a actual dia. was .5024. All my parts are coming out to small on the OD. I am not sure how I compensate for that over size. If there is a process I need to go through on my offset page or not. Looking for some direction. I have turned cutter comp on in my posted file using G41 but not sure if that is all I need to do.

    There are a few lines of the code for this tool



    G20 G40 G80 G90 M09
    G103 P0
    T02 M06
    M01
    S10000 M03
    G43 H02
    (msg,watchforair)
    M08
    M83
    G00 G90 X.135 Y-.9827
    Z.2631 M08
    G01 Z.0731 F30.
    G41 Z-.0269 F15. D00
    X.1352 Y-.6318
    X.1163 F30.
    G02 X-.0001 Y-.6177 I.0057 J.5328

    Not sure if the D00 is correct or not. I use a probe to set all my tools length and diameter.

    Any direction I can get would be greatly appreciated...

    Thanks

    Steve
    D should be your tool number D2, normally you can't activate cutter comp with a Z axis move should be a X or Y move
    Attached Thumbnails Attached Thumbnails Cutter Comp.PNG  
    Mactec54

  4. #4
    Member
    Join Date
    Aug 2009
    Posts
    1154

    Re: VF 1 Cutter Comp for tool diameter

    ..."Part Contour" programmed path or Net example mactec posted above is the way to do it. Then, all Diameter Offset (Dxx) settings would be "+" and actual Tool size. The Part Contour can be a Subprogram and just by changing the D Offset call you can rough and finish with different Tools or same Tool (using variable D) and only write it once. (big time saver in the old days) There are some limits like using an Endmill bigger than the smallest Radius in Pocketing cuts.

  5. #5
    Registered
    Join Date
    Jun 2007
    Posts
    46

    Re: VF 1 Cutter Comp for tool diameter

    Steven: First thing I would recommend is to recalibrate your probe and toolsetter. .5024 diameter seems a little too far out of what should be nominal. Anytime our toolsetters (Renishaw) get beyond .001 on quality made tooling, we recalibrate.

Similar Threads

  1. tool wear/cutter comp
    By jbranting in forum Haas Mills
    Replies: 4
    Last Post: 12-19-2017, 10:30 PM
  2. Replies: 5
    Last Post: 11-27-2014, 08:28 PM
  3. Using tool diameter for cutter comp
    By intenths in forum Surfcam
    Replies: 2
    Last Post: 02-20-2014, 03:32 AM
  4. Replies: 2
    Last Post: 02-11-2014, 01:17 PM
  5. Can I adjust cutter comp diameter within a program?
    By davereagan in forum General CNC (Mill / Lathe) Control Software (NC)
    Replies: 2
    Last Post: 11-20-2007, 05:12 PM

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
  •