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  1. #1
    Join Date
    Nov 2014
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    Question catia connex error

    Hello, i'm studying eletronic engineer on a university on brazil. i'm now using catia and i have low experience with programs of the same type. well, basically when i try to do a multi-section suface on, for example, two circles and two curves connecting them on those respectives edges, it appears the error:
    "The selected element is a non connex element, use another element or extract the non connex entity with NEAR operator"

    How do i solve this problem? i tried to use NEAR operator but i don't really know how to use it properly... if you could example i the most detailed all, i would be thankful because i am not a native english language speaker.

  2. #2
    Join Date
    Jul 2006
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    Pedro,

    Fitting a surface through 2 closed circles and 2 open curves doesn't make sense. That's probably why you are getting the "non connex" error. Could you attach a sketch of what you are trying to define.

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  3. #3
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    Nov 2014
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    Quote Originally Posted by MrCATIA View Post
    Pedro,

    Fitting a surface through 2 closed circles and 2 open curves doesn't make sense. That's probably why you are getting the "non connex" error. Could you attach a sketch of what you are trying to define.
    i'm trying to do the middle part of this watering can http://i.ytimg.com/vi/5bqOBeT4vAM/maxresdefault.jpg
    and i'm not being able to do it.

  4. #4
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    Nov 2014
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    i'm to do the middle part of this watering can http://i.ytimg.com/vi/5bqOBeT4vAM/maxresdefault.jpg , but i'm simply not being able to do it.

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  5. #5
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    Jul 2006
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    Thanks for the pictures - now I understand the assignment. The middle section of the watering can looks pretty straight forward. There is a curve (ellipse?) on the top and another on the bottom - these will be your section curves. There is also a curve in the front and one in the back - these will be your guide curves. It looks like the guide curves start and stop at the section curves, so everything should be all set to go.

    1. click on the Multi-Section Surface icon
    2. select the top ellipse to be section curve 1, and select the point at the top of the front guide curve (closing point 1)
    3. select the bottom ellipse to be section curve 2, and select the point at the bottom of the front guide curve (closing point 2)
    4. look closely for two red arrows showing the direction of the section curves. They should be pointing in the same direction (either clockwise, or counter-clockwise). If they are not the same, select one of the arrows to invert it. (this will avoid having a twisted surface)
    5. in the middle of the panel is the Guide Curve section. Click on the .... and select the front guide curve
    6. select the guide curve in the back (guide curve 2)
    7. click OK to make the surface
    Last edited by MrCATIA; November 11th, 2014 at 08:52 PM.

  6. #6
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    Still having the same problem... i don't know what to do anymore
    Attached Images Attached Images

  7. #7
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    The message says there's a problem with the sketch. So, let's try this:

    1. cancel the Multi-Section Surface command
    2. double-click on the first sketch to edit it. It should be one of the curves
    3. use the Tools + Sketch Analysis tool. It probably shows a short list of geometry, including the curve (circle/spline?). I'm guessing it also lists some points which are causing the problem.
    4. click on one of the points (blue highlight), and then click the first icon on the bottom to change the highlighted gometry to construction mode (it should dissappear from the list). Repeat changing the other geometry to "construction", except for the curve you want to use for the watering can.
    5. after you have removed everything except for the curve, close the Sketch Analysis window, and Exit the sketch.
    6. repeat steps 2 - 5 for all the other sketches.
    7. try the Multi-Section Surface command again.
    Last edited by MrCATIA; November 17th, 2014 at 05:01 PM.

  8. #8
    Join Date
    May 2016
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    Quote Originally Posted by Pedro13334 View Post
    Still having the same problem... i don't know what to do anymore
    Or try creating an extract. When you select multi-section surface, under guides, right click > create extract > select the guide curves individually(create 2 extracts). Now, the multiple extract should work.

    Good luck

  9. #9
    Join Date
    May 2016
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    Check this out:
    https://sahajpanchal.wordpress.com/2012/02/09/ use-non-connex-elements-from-sketch-in-3dcatia-v5

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