Sketch has more than one open contour

I have a 2D sketch which has straight lines and splines - those
entities are together supposed to form a closed shape, but I suspect
there are gaps between the ends of the entities. When I attempt to
extrude the sketch, I get "sketch has more than one open contour",
which I suspect is because there are gaps in the sketch.
I can't figure out how to merge or join the individual entities into
one closed shape, and/or to eliminate the error in extruding. (I
to close the gaps the splines would have to adjust some).
Note I tried to use "repair sketch", but it didn't seem to do
anything ....
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Hi Gus,
Try Tools > Sketch Tools > Check sketch for feature... It might help..
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Or: RMB and select chain to identify gaps (where selection stops). If everything is selected, make one element temporarily construction geometry and you will be able to identify the last gap.
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OK, I tried that. Feature usage is "base extrude", Contour type is "multiple disjoint closed", and the resulting message is "sketch has more than one open contour". I'm assuming the problem is "gaps", but I don't really know what the error message means .....
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Check to see if you have any short lines dangling from any corners. This sometimes happens to me, and you have to zoom in to every intersection to find them. Brian
gus wrote:
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The error message means you have at least 2 sketch entities that are not joined together so you can't create an extrusion.
In order for you to create an extrusion from a sketch, it has to be fully closed with no gaps between the sketch entities. You will have to determine where the gaps are and close them by either creating new entities to fill the gaps or extend existing entities so that they join together in one continuous sketch. You can create a thin extrusion from one continuous sketch that is not a closed loop type sketch as long as there is only one continuous sketch without any gaps between the sketched entities.
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Duplicates can also cause the failure, as can very tiny objects, or accidental ones outside the normal viewing area.
Sometimes I draw a circle around suspected intersection problems and Extend those lines and then Trim to revalidate the intersection.
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As Bo mentioned, duplicate lines are sometimes inadvertently created using the symmetric tool. Other areas to look at are end points that are at the intersection of more than entity are sometimes coincident with the construction circle or construction line rather than the desired entity.
Good Luck
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In the 2D to 3D tools there is a sketch check tool that helps find duplicates and gaps.
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