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catia connex error

Pedro13334

New member
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.
 

MrCATIA

Super Moderator
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.
 

MrCATIA

Super Moderator
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:

MrCATIA

Super Moderator
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:

bhargav317

New member
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
 

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