creating a point at the center of an area

Discussion in 'SolidWorks' started by Randle.Domico, Dec 8, 2005.

  1. I can use the properties to locate the center of area, but how do I
    creat a point in that location.
    For example: create a point in the center of area of a triangle.
    Thank you
     
    Randle.Domico, Dec 8, 2005
    #1
  2. Randle.Domico

    Dan S. Guest

    I use the section data to locate the point. Take a section, write down
    the coordinates, and then create a sketch using thoses coordinates.
    This will work until you change the geometry and the center moves. I'd
    love another way, and maybe there is one.

    Also, my company often asks for section modulii which solidworks
    doesn't compute (I have to use ProE to calculate this, and I hear about
    it from the ProE guys). I'd love to have this integrated also.

    Dan Sommerfeld
    Industrial Designer
    ITW Dahti Technologies
     
    Dan S., Dec 8, 2005
    #2
  3. Aren't you guys sort of missing the point? The OP said that he could read
    the coordinates by using the Tools/Section Properties tool. But then how
    does he put a point there? Manually typing those numbers into a 3D sketch
    is a way that would work. But, I would think that those numbers would be
    available to the API, so I think what he wants is a macro just like the one
    we have for putting a 3D point at the CG. There are 2 macros that do that -
    one that puts a new point every time you run it, and the other that updates
    the one existing point. Both are static in that they don't automatically
    update. So, someone with some time could take the CG macro and rewrite it
    to a Center of Area macro. I don't have the time right now - any takers up
    to the challenge?

    WT
     
    Wayne Tiffany, Dec 9, 2005
    #3
  4. Randle.Domico

    George Guest

    You can add a "Reference Point" to the "Center of Face" on any shape
    surface...

    Insert/Reference Geometry/Point

    This is the same tool used for inserting a plane or an axis. See
    Reference Geometry.

    This is not to be confused with...

    Tools/Sketch Entities/Point
     
    George, Dec 9, 2005
    #4
  5. Ahhh, touche. I don't believe I have ever used that one, but I think it
    hits the nail in the head here as the best solution without a macro. If you
    add the point and then modify the shape of the face, then the point will not
    move on its own. However, if you then edit the definition of that reference
    point, it will update properly. You can use that point to attach lines,
    etc. (Don't forget to turn on the viewing of points.)

    That's why I like this group - thanks.

    WT
     
    Wayne Tiffany, Dec 9, 2005
    #5
  6. Randle.Domico

    Jeff Guest

    if you are looking for a way to generate a point at the center of mass,
    which is what it kinda sounds like, there was a post about a week ago
    that had a macro that would generate a point at the center... hope
    that helps...

    Jeff
     
    Jeff, Dec 9, 2005
    #6
  7. Randle.Domico

    George Guest

    FYI - I sketched a triangle and extruded it. I then inserted the
    reference point. Click on the point and record the coordinates. If you
    then go back to the triangle sketch and drag one of the vertexes and
    leave the sketch the reference point has moved to the new centroid of
    the area. (SW2006SP2)
    ~G
     
    George, Dec 9, 2005
    #7
  8. Now that is interesting. The way I tested it was by changing the shape by
    double-clicking to show a dimension, change the dim, then rebuild. The
    model and the face updated, but the point did not. But if you go into the
    sketch to make the change, the point will update when you come out. You
    don't have to rebuild to come out, just close the sketch. So, two different
    methods - I wonder if SW knows about this??

    WT
     
    Wayne Tiffany, Dec 9, 2005
    #8
  9. Randle.Domico

    George Guest

    Wayne, I tried your method too and all updated, even the point. It is
    now in a different location. Strange ... it works both ways for me and
    I cannot recreate your scenerio.

    I contribute this to Bermuda Triangle Surface rather than Boolean
    Triangle Surface.... goof luck!!

    Its snowing like crazy here so I think I am going to cut out.

    Have a nice weekend.

    ~G
     
    George, Dec 9, 2005
    #9
  10. Randle.Domico

    chub Guest

    Thank you all for he helpful information.

    The "Tools/Sketch Entities/Point" command work great for faces.

    What I have been trying to find is a way to creat a point in the COG of
    a chained 2d object witout going into DWG editor. It would be nice to
    be able to create the point while in sketch mode but the above command
    will work for what I need.

    I use this to determine the center of effort in relation to the center
    of lateral resistence in sailboat design.

    Thanks,
    Randle
     
    chub, Dec 10, 2005
    #10
  11. Randle.Domico

    chub Guest

    I have yet to find a way to create a point at COB in drawing mode.
    If I do the "Tools/Sketch Entities/Point" command in PART mode the
    point it works good, but will not show in DRAWING mode.
    hmm......
    any ideas???
     
    chub, Dec 10, 2005
    #11
  12. Randle.Domico

    George Guest

    Chub,

    To get this point to show in drawing mode ...

    In part mode right click on the point in the design tree and select
    Show.
    Then in drawing mode View\Points

    ~G
     
    George, Dec 12, 2005
    #12
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