3dprintforums logo



Results 1 to 11 of 11

Thread: Troubl understanding G41 and G42 codes

  1. #1
    Registered StellasDad's Avatar
    Join Date
    Aug 2008
    Location
    Canada
    Posts
    5
    Downloads
    0
    Uploads
    0

    Troubl understanding G41 and G42 codes

    Ok... I'm a newbie. Now thats been said and out of the way, I'm having trouble understanding these codes.

    I do not understand how and when to incorporate these codes. I do understand that the G41 compensates to the left of the toolpath and the G42 to the right. How does one use these in a manual lathe program? What rules are there to follow?

    I would appreciate the help. Thanks in advance.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Feb 2008
    Location
    USA
    Posts
    509
    Downloads
    0
    Uploads
    0

    Smile Sorry...

    ...we may be a little confused. Your, on one hand, talking about CNC ( Computerized Numerical Control) "G" codes (G41 & G42 ect...automated machines) then on the other hand you change over to refering to a "manual lathe".??? Try again with more background info...
    Steve



  3. #3
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0
    I don't know if there is a big list of rules to know. A couple perhaps.

    First, pre-position the tool near the start of the profile to be cut, but not directly on the profile. When radius compensation is turned on, then the controller reckons that the path has now shifted from tool center to tool edge tangent. It may make an actual movement to adjust its position (by the tool radius amount), or, it may save that move and combine it with the next real positioning command.

    So if you begin with the tool on the profile, you'll probably get a little gouge mark.

    The lead off of the profile should follow a similar rule. Don't turn radius comp off (G40) while the tool is sitting on the part profile. Again, a gouge mark may result.

    So in real life, you need to add a short line onto and off of the actual profile that you want to machine.

    I think it is good practise to eliminate square internal corners from the path profile. The tool is not going to cut it anyways, so you might as well draw it the way it will actually look. Taking this step will help eliminate "cutter interference" alarms when the control cannot calculate the next move because the endpoint disappeared when the corner was trimmed. If you trim (fillet) the path first, then you won't have grief unless you call for a tool tip radius that is larger than your drawn fillet. You might or might not get an alarm, but the part will not be cut as drawn if the tool cannot fit into every corner of the path.

    There are typically 'directions' for tool comp. There may be a chart or table of some sort in the manual that tells you which number to assign to the tool, given the direction that it must approach and execute a path. I'm not really "up" on the details of this, so maybe someone else would care to elaborate.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #4
    Registered
    Join Date
    Feb 2008
    Location
    USA
    Posts
    509
    Downloads
    0
    Uploads
    0

    Ahhh..

    Did you mean lathe Manual??? How the cutter comp. is used is dependent on the the part rotation CW CCW , tool direction, and if it is an outside cut or a bore. I will post a formula later this week for slowing the feed rate as you make the turn that is based on the radius in the inside corner. I don't have it with me right now. Nice post HnFlungDung. Steve



  5. #5
    Registered StellasDad's Avatar
    Join Date
    Aug 2008
    Location
    Canada
    Posts
    5
    Downloads
    0
    Uploads
    0
    Ya... I meant manual programming for cnc lathes.

    Thanks for all the advice. You've been very helpful!



  6. #6
    Registered
    Join Date
    Jul 2007
    Location
    U.S.
    Posts
    25
    Downloads
    0
    Uploads
    0
    The general rules are
    G41 and G42 must be turned on in G1
    G41 and G42 are turn off by G40 in G1
    G41 outside of a part moves away from the chuck and towards center
    G41 inside a part towards the chuck and center
    G42 out side a part moves towards the chuck and away from center
    unless you are working on the back side of a part(chamfering before cutoff)
    G42 inside a part away from the chuck and center



  7. #7
    Registered StellasDad's Avatar
    Join Date
    Aug 2008
    Location
    Canada
    Posts
    5
    Downloads
    0
    Uploads
    0
    Thanks but that would all depend if you were climb or conventional milling. You just described comp if one were climb milling.


    Generally, G41 would be compensation to the left of tool path and G42 would be compensation to the left of toolpath. Right?



  8. #8
    Registered
    Join Date
    Sep 2008
    Location
    united kingdom
    Posts
    4
    Downloads
    0
    Uploads
    0

    G41/42

    hi Im not a lathe machinish myself i run a vertical miller but compensation is the same whatever your doing.
    the main rule for compensation is to activate it properly, to activate the compensation you MUST make a 90deg movement after the g41/42, if you dont do this sometimes compensation is not active properly and your component will be incorrect.

    Example:-
    N170 G21 G40 G96 G99 S300 T202 M14
    N180 G0 X24. Z0.
    N190 G1 X-1.6 F.23
    N200 G0 X24. Z3.
    N210 G42
    N220 G0 X14.5 -----90deg movement
    N230 Z1. ------90deg movement
    N240 G1 X20.0 Z-1.75 F.2---Profile
    N250 Z-25.25
    N260 X16.5 Z-27. F.05
    N270 Z-30. F.2
    N280 X46.
    N290 X48. Z-31.
    N300 Z-45.
    N310 G28 G40 U0. W0. M9
    N320 M1

    Hope this helps



  9. #9
    Registered
    Join Date
    Jul 2007
    Location
    U.S.
    Posts
    25
    Downloads
    0
    Uploads
    0
    No I just described bolth.G41 is always climbing G42 is always convetional.But it dosnt matter on a lathe,ecept to your canned roughing/finising cycles they HAVE to see motion towards the chuck and center



  10. #10
    Gold Member
    Join Date
    Oct 2005
    Location
    USA
    Posts
    672
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by StellasDad View Post
    Generally, G41 would be compensation to the left of tool path and G42 would be compensation to the left of toolpath. Right?

    This is exactly true. The control has no idea which side of the tool is in contact with the workpiece. It is only trying to follow the programmed path and move to the left (G41) or right (G42).

    Further, on many milling machines, you can use a negative value for the tool diameter which effectively puts the tool to the opposite side. In other words, running G41 with a negative tool diameter will put the tool to the right of the programmed path. Some people only use G41 (never G42) and simply use positive and negative diameters to control the side they comp to.



  11. #11
    Registered StellasDad's Avatar
    Join Date
    Aug 2008
    Location
    Canada
    Posts
    5
    Downloads
    0
    Uploads
    0
    I want to thank everyone or their valued input and I know understand compensation and feel comfy using it. Although I never thought of just using G41 and using a negative value, it makes sense to me.



Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed