CAM Programming: G60/G61 & G64 - and Why!
Close
Login to Your Account
Results 1 to 9 of 9
  1. #1
    Join Date
    Mar 2017
    Country
    CANADA
    State/Province
    Quebec
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    27

    Default CAM Programming: G60/G61 & G64 - and Why!

    How bothered are you programming for exact-stop and constant-velocity in your CAM part programs?

    I normally prog G61 for finishing passes and g64 for roughing but wonder if this makes any 'real' differences, considering the effort it takes to squeeze in these extra lines of gcode manually (lets' say in a 3D cam program).

    Why do YOU use them; time saving? reduce mechanical strains on MT? or to get some nice rounded corners perhaps? Any other scenarios?

    Thanks

  2. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7,745
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2061

    Default

    Quote Originally Posted by THCustoms View Post
    How bothered are you programming for exact-stop and constant-velocity in your CAM part programs?

    I normally prog G61 for finishing passes and g64 for roughing but wonder if this makes any 'real' differences, considering the effort it takes to squeeze in these extra lines of gcode manually (lets' say in a 3D cam program).

    Why do YOU use them; time saving? reduce mechanical strains on MT? or to get some nice rounded corners perhaps? Any other scenarios?

    Thanks
    .
    depends on tolerances of course. if you indicate parts needing to hold a .0002 or .0003 straightness and perpendicularity tolerance you do what ever needed. some use exact stop mode. others have parameters set if cnc is more than set amount out of position during movement it just stops with a error message that it exceeded the limit
    .
    usually i add G4 delay to wait for servos to stop moving (servo oscillation) when i change direction or even just stop moving in one direction. i also add G4 delay with spindle running to warm it up as it grows longer .0003 as it warms up
    .
    i also add cuts like +.0010, +.0005 and then .0000 if parts tend to distort after machining and extra cuts help remove it.
    .
    i also adjust feeds and speeds as surface oscillation from cutting vibration and built up edge forming and breaking off can cause .0004 waviness easily

  3. Likes THCustoms liked this post
  4. #3
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    3,926
    Post Thanks / Like
    Likes (Given)
    798
    Likes (Received)
    2565

    Default

    Quote Originally Posted by DMF_TomB View Post
    [I] also add cuts like +.0010, +.0005 and then .0000 if parts tend to distort after machining and extra cuts help remove it.
    Hi Tom,
    Being a bit of a pedant here, but when you talk about "extra cuts" of such small amounts when using carbide inserts meant for cast iron, isn't it more accurate to call them burnishing passes? The edge prep on those inserts doesn't allow for really small cuts.

    Or maybe it's closer to grinding...

  5. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7,745
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2061

    Default

    Quote Originally Posted by Milland View Post
    Hi Tom,
    Being a bit of a pedant here, but when you talk about "extra cuts" of such small amounts when using carbide inserts meant for cast iron, isn't it more accurate to call them burnishing passes? The edge prep on those inserts doesn't allow for really small cuts.

    Or maybe it's closer to grinding...
    .
    .
    i often mark up parts with a magic marker and cut .0005" at a time and when done dry the chips (dust) made is quite obvious. when marker mark becomes semi transparent usually cutting about .0001 or .0002
    .
    boring bars can be unstable opening bore less than .001 dia or .0005 radius. depends on length rigidity and feeds and speeds. some boring bars at higher rpm will cut .0001 bigger probably cause at higher rpm it wobbles to a bigger dia
    .
    usually extra cuts of .0005" amounts is cause machine may not repeat to .0000 and .0005 makes sure always some cutting pressure. extra cuts cutting tool deflection becomes less and less and surfaces edges become straighter and straighter.
    .
    there is some feeds and speeds where surface waviness is less. often higher sfpm is more shiny but waviness is more or unstable. i try to keep a .0003 TIR waviness tolerance
    Attached Thumbnails Attached Thumbnails warpageremoval.jpg   shinymilling.jpg  

  6. #5
    Join Date
    Mar 2017
    Country
    CANADA
    State/Province
    Quebec
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    27

    Default

    Had Siemens over tutor me on HSM recently,looking at my ctrl setings especially those G60 and G64 tols. To finally tell me that I have G64 G641/G642/G643/G644/G645 all with their respective function. All at 0.000 floats each which then gives me just about seventeen-trillion different ways to program a toolpath. No offense to anyone but I had to laugh!

    My question was about whether you (we) need to bother that much about all of that non-sense. As in can we just have one (two max) setting that envelop the "common" parts we can machine on CNC?! By common, I mean; free form, few helical/radius, filets and edges or chamfers. Unless we can do what additive or EDM can't with a CNC then... wow (/rant).

    Was just wondering if you guys are programming ALL this in exact-stop mode (e.g hassle-free) or ALL in constant-velocity mode. Whether you bother switching those modes between operations or perhaps even go as far as doing G09 on some specific blocks?

    You guys make your machines/toolpaths dance a little?!

    ps: I have 133 ops on the part I'm working on atm, and siemens is almost telling me to slow my feedrates if I can't use G60/64 properly... wtf)

    pps: Hard to be a "Machinist". Even harder to become a "Practical" one apparently LOL

  7. #6
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    102
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    24

    Default

    "ps: I have 133 ops on the part I'm working on atm, and siemens is almost telling me to slow my feedrates if I can't use G60/64 properly... wtf)"

    I'm sure that is what they told you.
    What they meant was that your CAM product needs to be properly configured to output the desired code absent your intervention.

    You don't actually have control/configuration issues.
    You have an issue with your posted output.

  8. #7
    Join Date
    Mar 2017
    Country
    CANADA
    State/Province
    Quebec
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    27

    Default

    Thanks for your input! Yea CAM system I'm using is not the best but can't say its the worst

    I'm customizing it now with User Defined Events that should include (inject?) the respective path-mode based on the tolerance it finds in the CAD data (as automated as it can be, hopefully). See if this can save me from re-writing the part program manually with silly G60 and G64 G602 ADIS=0.x" on some Ops/blocks ~ each and every time I have to re-post it from the CAM side :/

  9. #8
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    102
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    24

    Default

    That is exactly what I do.
    You might want to make a list of the behaviors first and the attributes you want associated with them.
    I always output G60 for drill cycles if it is supported at the machine, for example.
    My MAZAK posts always use their M825-M830 functionality. Which code depends on the stock I'm leaving.
    A little thought before running off with a bunch of changes can be useful.

  10. Likes THCustoms liked this post
  11. #9
    Join Date
    Mar 2017
    Country
    CANADA
    State/Province
    Quebec
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    27

    Default

    Quote Originally Posted by JCarroll View Post
    Which code depends on the stock I'm leaving.
    Man... ^ THIS ^

    Thanks for that tip, it works. Far better than using the TOL variable from CAD. Brilliant. Thank you! PP can also detect point-to-point toolpath (e.g drill) and that slams in the G60 automatically along with its jerk limitation setting (e.g.BRISK/SOFT).

    Almost done with this mess, thanks again for your tips!

    HSM is-not-for-girls I tell ya. Looks so much easier on TV lolll. Had to be sorted otherwise I swear my machine would have been destroyed by the time it reaches to the 5th part. Or the concrete cracked under... whichever comes first.


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
  •