Find leak in sketch geometry

[Helmi74]

Hi,

i did a relatively simple sketch geometry with some parametric values. I've been quite careful, used constraints as much as possible but still end up having a geometry which somehow isn't closed in the eyes of fusion. It doesn't show my geometry as closed and i can't do push pull and other things you would expect.

After inspecting visually i can't find anything problematic. What would be the right steps to follow to get rid of this problem?

Unfortunately i can't publish this document at the moment.

Thanks for helping

[TheCADWhisperer]

White dots = missing coincident constraints.

Blue lines = unconstrained geometry.

When in doubt - click and drag white dots.

What do you observe?

Why sketch extra lines?  Get lazy!  Only sketch that which is needed.

[j9lemmon]

Click and drag white dots is great advice. Thanks @TheCADWhisperer

[etfrench]

About 15 seconds to find the problem.  10 seconds were used to extend the lines where the white dots show non-coincident endpoints and 5 seconds to window select the geometry above the crossing line, right mouse click, then selecting Move to Sketch Plane from the context menu.

[j9lemmon]

Thanks @etfrench - very useful details. 

[j9lemmon]

I figured out how to use Sketch Checker to highlight leaks in sketches (very simple). 

⦁ do Edit Sketch for the Sketch that's leaking
⦁ at Top, choose Inspect - Sketch Checker
⦁ white dots that turn gray might cause the leak

The link to download Sketch Checker is above in this discussion.

[j9lemmon]

Using the advice above, especially from @etfrench and @TheCADWhisperer , I spent 30 minutes experimenting with adding constraints and other fixes for a leaky sketch. Here's what I observed:

⦁ Goal 1: eliminate white dots that show without being selected.
⦁ Goal 2: on mouse rollover, the sketch should turn black [ if Show Profile is checked in Sketch Palette]

⦁ After applying a constraint, press ESC key to exit that tool
⦁ Any white dot is a likely source of a leak. Move the dot around with mouse & observe; this gives clues about how much the segments adjoining that dot are constrained.

To apply a constraint to multiple segments:
⦁ do Edit Sketch
⦁ at Top, select a Constraint
⦁ click on a segment, then a second segment. EG select Parallel Constraint, click a segment, then a 2nd segment, and the Parallel constraint will appear.
⦁ If two adjoining lines are NOT connected to each other, try to Extend one of the lines. Do Edit Sketch - at Top choose Modify - Extend, then click a segment to extend it past the offending white dot, then do Modify - Trim to Trim what's over-extended.

These tips and my terminology, so I'd love improvements from those with more experience.

Thanks again for the help.