584,866 active members*
5,189 visitors online*
Register for free
Login
Results 1 to 10 of 10
  1. #1
    Join Date
    Apr 2011
    Posts
    720

    Proper cut start methods

    Hi,

    I have some more pretty basic questions about G gode techniques for beginners.
    I am practicing trying to write my own code for simple things and today I decided to do circle cuts. I wrote the clip below to try to cut a simple circle and it works but I know its not very good and probably terribly inefficient, but I'm just trying things out a little at a time.

    My question is that, while this works, it just plunges the cutter at the begining, and I know that's not best practice. But reading my Tormach manual, the Peter Smid CNC Programming Techniques book, and going thru the G code tutorial at the CNC Cookbook site, haven't shown me the best approach to this problem.

    I think I want to ramp into the cut on each pass, but don't know where to learn how to do it? One thought was maybe helical interpolation was the approach, but that's really just a guess.

    Any suggestions on where to learn this would be appreciated.

    Thanks Terry


    G0 G49 G40 G17
    G90
    G20 (Inch)
    M3 S4000
    G04 P2
    M9
    G00 X0.0 Y0.0
    Z0.4
    F10
    G01 X1.0 Y1.0
    Z-.03
    G02 X1.0 Y1.0 I-.51 J0
    G01

  2. #2
    Join Date
    Feb 2006
    Posts
    7063
    If you do this:

    G01 X1.0 Y1.0
    G00 Z0.02
    G02 X1.0 Y1.0 Z-.03 I-.51 J0
    G01 Z0.4

    This will do a helical interpolation. Straight plunges are kinda hard on the tool. Much better to do some kind of more gentle approach that ramps down to depth at a reduced feedrate, typically 1/3-1/2 the traverse feedrate. So, if your full-depth feedrate is 12 IPM, use 4-6 IPM for the plunge, then speed up to 12 once at depth. When side-cutting, it's also best to ease into the cut, with either a tangential or arc move that ends on the final path.

    Regards,
    Ray L.

  3. #3
    Join Date
    Apr 2011
    Posts
    720
    Ray,

    Thanks a lot for the reply! That works, but I'm not sure why????
    Is the interpolation caused be moving the Z-.03 until after the G02, or by the addition of the G00 Z0.02 before the G02, or the combination of both steps?

    Since this leaves a ramped cut, I assume in a real job, if it's not a thru hole, I would add a pass without the interpolation to flatten the bottom?

    Do you know a text or web location that covers the theory of this procedure?
    Thanks again
    Terry

  4. #4
    Join Date
    Feb 2006
    Posts
    7063
    Terry,

    G01, G02 and G03 can move any, or all, axes at one time. The velocity of each axis will be set such that all axes reach the destination position at the same time. So, adding the Z-0.03 to the G02 causes the tool to move in a circular arc in X/Y, while simultaneously moving downward in Z - hence a helical move.

    Your first post indicated you have the Smid book - that explains ALL the standard G-codes. Best way to learn them is by doing a lot of "air cuts" using MDI, to understand what each does.

    If you want a flat bottom, then, yes, you would have to do one more G02 without a Z move to clean up the bottom.

    Regards,
    Ray L.

  5. #5
    Join Date
    Apr 2006
    Posts
    439
    Hi Terry

    I think the single most valuable tool that helped me learn G-Code was a program called NCPlot. It is a backplotter. It gives a graphical representation of your code. You write your code on the left and it is shown on the right. There is also a forum here on the zone for it. I am pretty sure there is a free version ( Lite ) and a 15 day on the full version. I can't live without it. It has saved my butt so many times it's not funny. And usually for really dumb mistakes like an omitted decimal point or - sign. When you see that wacky line in the viewport it is pretty obvious. You can sit at your desk and write all kinds of code and not have to go to the machine to see what it will do. You can step through it line by line and see what everything does. Here is your code in the screen shot. And the website. NCPlot.com - Tools for CNC Programmers



    Scott ( Not the same Scott who sells NCPlot )
    Attached Thumbnails Attached Thumbnails NCPlot.jpg  
    www.sdmfabricating.com

  6. #6
    Join Date
    Apr 2011
    Posts
    720
    Ray,

    Your explanation helped a ton, thank you, after what you told me I able to find the appropriate place in the Smid book, so I am studing away LOL.

    Scott thank you for the preview and link to NCplot, it looks really neat and does even more stuff than I thought it might. I intend to check it out right away.

    Terry

  7. #7
    Join Date
    Dec 2003
    Posts
    673
    another really handy tool is the free version of HSMWorks.. it includes a great G-code editor which visualizes the cut, and color codes the g-code to help you keep track of the types of cuts.

    Easy rule of thumb is, if you want to ramp axis together, put them on the same line x y z.
    If you want to position independently (sequentially) put them on different lines
    x
    y
    z

  8. #8
    Join Date
    May 2005
    Posts
    2502
    Terry, there's a bunch of considerations to solve the circle cutting problem in general. For example, you do want to helix in, but only helix up to 2x the diameter and then spiral out from there if the overall circle is larger than the diameter. There are cleanup issues too. Certainly a finish pass is in order. Many consider that they get greater accuracy if they run the finish pass twice--once in each (climb vs conventional) direction.

    You can see code for all this in the G-Wizard Conversational CNC add-on. It offers a Wizard for interpolating holes. Just get GW Editor and click the "Wizards" button on the Toolbar.

    CNC Conversational Programming Software from G-Wizard

    The Wizard will generate code which you can then look at to see how it was done.

    Cheers,

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  9. #9
    Join Date
    Apr 2011
    Posts
    720
    Spinnette,

    Thanks for the suggestion on HSMWorks, but when I googled it, the link I found seems to say it only works with Solidworks? Did I miss something?

    Bob,

    I appreciate your advise, and I have been using my GWizard Editor as I've been trying to learn. I did find it helped to do a final pass without the helix in play and it did help to cleanup the bottom of the cut. I haven't tried going both ways yet, but will definetly do that. In my trial cuts, I'm cutting a 1.25" circle in .1875" 6061, so I think I'm OK with your 2x the diameter idea?

    One question though, when I look at the wizards, I only see the canned drilling cycles available, nothing yet for arcs and circles? Am I missing something here also?

    Thanks
    Terry

  10. #10
    Join Date
    May 2005
    Posts
    2502
    Terry, you're correct, so far only the Hole Wizard. More to come.

    RE 2x the Diameter, I mean 2X the cutter diameter. This is so as not to cut a ring that could potentially jam and break the cutter. You want to turn that helical cut center plug into chips.

    Cheers,

    BW
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

Similar Threads

  1. ACME rods - normal start and multi-start
    By shaffin in forum Canadian Club House
    Replies: 0
    Last Post: 12-20-2010, 02:19 PM
  2. Replies: 4
    Last Post: 01-06-2009, 05:20 PM
  3. Test methods
    By guhl in forum Fanuc
    Replies: 0
    Last Post: 12-08-2007, 10:21 AM
  4. Replies: 12
    Last Post: 01-09-2007, 07:42 PM

Posting Permissions

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