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?

 

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

 

Sorted. It seems I have a rogue point and an overlapping line.

Cheers!