Open profile

I have just drawn a complicated 2D sketch and then try to extrude it.
The error message comes up about open/closed profile.
Is there any way of finding out where the open contour is without going
along the drawing profile with the zoom/pan command?
Reply to
J Parr
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Go to Tools/Sketch Tools/Check Sketch for Feature and in Feature usage: check Base Extrude. Failing sketch entities should be highlighted.
// Krister L
Reply to
Howdy -
1) Use RMB, select chain to see where the gap is - the chain will highlight and you will see the extents of the sketch.
2) Turn on your Tools->Options->Sketch->Display Entinty Points In part/assy sketch - these are really helpful.
3) When the error occurs, it usually highlights the "bad" area or at least the first one it finds - this can show the area that is bad.
4) Turn 1/2 the geometry into reference geometry, close the loop with a temporary line you can quickly home in on a problem this way - once debugged, go back to construction geometry.
5) Tools-> Sketch Tools -> Repair Sketch might be useful
6) Check Sketch for Feature
Reply to
Sean-Michael Adams
Sorted. It seems I have a rogue point and an overlapping line.
Reply to
J Parr

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