530,019 active members*
3,448 visitors online*
Register for free
Login
Results 1 to 7 of 7
  1. #1
    Registered
    Join Date
    Jan 2008
    Posts
    3

    Help! Intercon Arcs

    Hello All,

    New here, been lurking for a long long time. Anyways, Just brought home a new (to me) lathe with the centroid T-400 control and being a newbie at this cnc lathe stuff I am seeking help. When profiling in Intercon and using arcs, there are 4 different arc options and all of them are confusing me as to what to enter. The manual shows a couple of examples, but that's not helping. I figure one of you guys could hand sketch something and explain it in english a whole lot better than the manual. I'm LOST??? Thanks in advance.


    Amurf

  2. #2
    Registered
    Join Date
    Feb 2008
    Posts
    276
    In all cases, the arc move starts wherever the preceding move left off. You can't just program an arc as if it were a canned cycle. First you need a Rapid and/or Line move to bring the cutter to the starting point of the arc.

    Then you have four choices for how to specify the arc, depending on what information you know:

    EP&R = End point and radius. You know the coordinates of the end of the arc, and you know the arc radius. 95% of the time, this is what you want.

    CP&EP = Center point and end point. You know the coordinates of the arc center, and you know the coordinates of the end point.

    CP&A = Center point and angle. You know the coordinates of the arc center, and you know how many degrees you want to swing around that center.

    3 Point = Three point arc. You know the arc starting coordinates (the place your previous rapid or line went to); you know some point midway along the arc; and you know the end point coordinates.

    In each case, after you enter the information you know, Intercon calculates the remaining information. For example, if you enter an End Point and Radius arc, after you give the endpoint and radius, and choose CW or CCW, then Intercon calculates and fills in the center point and mid point coordinates, and the angle of swing.

    Two things can be confusing on a Lathe. First, all your X axis coordinates are diameter values, and so are twice the actual distance from centerline. Second, CW/CCW is always judged looking at the "back" or "top" side of the part, as if X+ was up, even if your lathe happens to be assembled with the tool post in front of centerline, and your X+ jog button therefore pointing down.

  3. #3
    Registered
    Join Date
    Jan 2008
    Posts
    3
    Marc,

    Thanks for your help (again) Does the last move (rapid or line) before the arc have to be an X move or does it matter?

    I haven't contacted dean yet as I've been fighting Pneumonia for the last few weeks but I'm feeling better and will get in touch with him. Thanks again, much appreciated!


    Murf

  4. #4
    Registered
    Join Date
    Feb 2008
    Posts
    276
    If you are programming a Profile cycle, then the first move in the Profile needs to be an X-only line or rapid.

    Since your arc is likely to start at the end of the part (or be further down the part), and you should always choose a Start Point for the Profile that is clear of the end of the part by at least twice the tool nose radius, this generally means that you need at least two moves in the Profile before the arc: one that just moves X down to your starting position, then one that moves Z in to the face of the part.

    More commonly you need three lines, to ensure that the entire arc gets cut. This is because, if you are using tool nose radius compensation, your first move needs to overshoot the beginning of the arc by at least the nose radius.

    For example, suppose you want to put a full radius on the end of a 2" bar, and your tool has a 0.032" nose radius.

    Your profile Start Point needs to be at or above X2.0, and out to at least Z0.064. I would add a bit more, so that I don't run into trouble if I have to adjust my tool nose radius offset by a few thousandths. So try X2.1 Z0.1 for a starting point.

    Your next move would be a Line or Rapid, staying at Z0.1, but moving X down past centerline, say to X-0.05.

    The next move would be a Line, staying at that X, but bringing Z in to Z0.

    Then a Line to X0 Z0 (the start of the arc)

    Then an Arc: say EP&R, with an end point of X2 Z-1 and a Radius of 1.

    The first three line moves make three sides of a box, approaching the start of the arc in a rather roundabout manner. This is necessary because you should be using cutter radius compensation (Comp Right in this case). If you picture a full circle, with the same radius as the tool nose, moving around the inside of that box, it fits with a little room to spare.

    Suppose we had used X2 Z0 as the Profile Start; gone straight down to X0 Z0; then come up our arc. If you try to slide the cutter nose circle down the right side of the first line, then up the right side of the arc, it has to turn around long before it gets down to centerline. Much of your arc would be left uncut.

  5. #5
    Registered
    Join Date
    Jan 2008
    Posts
    3
    Marc,

    That helped alot. I can now picture the whys and hows in my head. I have a hard time understanding the manual sometimes, I don't know if it's just me or not but I definately understand the way you explain it. Thanks again for all your help.

    Sincerely,

    Murf

  6. #6

    Join Date
    Sep 2020
    Posts
    1

    Re: Help! Intercon Arcs

    Quote Originally Posted by cncsnw View Post
    If you are programming a Profile cycle, then the first move in the Profile needs to be an X-only line or rapid.

    Since your arc is likely to start at the end of the part (or be further down the part), and you should always choose a Start Point for the Profile that is clear of the end of the part by at least twice the tool nose radius, this generally means that you need at least two moves in the Profile before the arc: one that just moves X down to your starting position, then one that moves Z in to the face of the part.

    More commonly you need three lines, to ensure that the entire arc gets cut. This is because, if you are using tool nose radius compensation, your first move needs to overshoot the beginning of the arc by at least the nose radius.

    For example, suppose you want to put a full radius on the end of a 2" bar, and your tool has a 0.032" nose radius.

    Your profile Start Point needs to be at or above X2.0, and out to at least Z0.064. I would add a bit more, so that I don't run into trouble if I have to adjust my tool nose radius offset by a few thousandths. So try X2.1 Z0.1 for a starting point.

    Your next move would be a Line or Rapid, staying at Z0.1, but moving X down past centerline, say to X-0.05.

    The next move would be a Line, staying at that X, but bringing Z in to Z0.

    Then a Line to X0 Z0 (the start of the arc)

    Then an Arc: say EP&R, with an end point of X2 Z-1 and a Radius of 1.

    The first three line moves make three sides of a box, approaching the start of the arc in a rather roundabout manner. This is necessary because you should be using cutter radius compensation (Comp Right in this case). If you picture a full circle, with the same radius as the tool nose, moving around the inside of that box, it fits with a little room to spare.

    Suppose we had used X2 Z0 as the Profile Start; gone straight down to X0 Z0; then come up our arc. If you try to slide the cutter nose circle down the right side of the first line, then up the right side of the arc, it has to turn around long before it gets down to centerline. Much of your arc would be left uncut.
    Hi there, thanks for that really useful information. Do you have an example of starting a radius in the middle of the part? I will probably have to do the 1st part of the arc at the original position and then when I flip the part will have to do the remaining arc at that time. Starting in the middle means I probably won't have the luxury of starting below X=0 like you did when starting at the end.

  7. #7
    Registered
    Join Date
    Feb 2008
    Posts
    276

    Re: Help! Intercon Lathe Arcs

    You can use the Profile cycle without going to, or past, X0.

    The first move in the Profile still needs to move only X, but that could be as short as going from clearance to the stock OD. Then you could start whatever arc you want to do.

    I could not hazard a guess as to whether you can do what you want to do in one operation and one fixturing, or whether it requires two. You would have to post a drawing of what you have in mind.

Similar Threads

  1. Replies: 5
    Last Post: 12-10-2013, 03:02 PM
  2. Anyone proficient with Intercon?
    By Johns tool room in forum Centroid CNC Control Products
    Replies: 8
    Last Post: 09-25-2012, 03:04 PM
  3. Incremental arcs and Break arcs into lines
    By forhire in forum NCPlot G-Code editor / backplotter
    Replies: 10
    Last Post: 09-16-2010, 04:55 PM
  4. 3d arcs?
    By stevespo in forum BobCad-Cam
    Replies: 10
    Last Post: 09-01-2007, 02:02 AM
  5. Offline Centroid Intercon Problems
    By jime in forum General CNC (Mill / Lathe) Control Software (NC)
    Replies: 0
    Last Post: 11-05-2006, 11:20 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
  •