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?
Go to Tools/Sketch Tools/Check Sketch for Feature and in Feature usage:
check Base Extrude. Failing sketch entities should be highlighted.
// Krister L
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
Later,
SMA
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