How do I find the dangling things that solidworks says this has?
Edit the sketch that created the feature, and you'll see that some of the sketch entity relations have will have turned that sickly yellow-brown color, which means they've lost their reference (that's what's "Wong"; sorry I couldn't resist). Delete these relations and add new ones to fully define the sketch.
An alternate to Glenn's input you can...
RMB when in the sketch and select Display Sketch Relations. There are two points that have lost their references. Delete the relations and redefine.
The others are correct. Attached is the fixed file also.
Your sketch looks small, which makes it easy to find those yellowish relations. However, in a much larger sketch full of relations, this is not as easy to visually locate. Use the "Display / Delete Relations" button in Sketch ribbon. In the D/DR feature manager, select in the drop-down under Relations to change from the default "All in this sketch" to "Dangling". These dangling relations should all be yellow colored. You can delete them directly from this feature manager interface. Afterward, click OK to return to your sketch. Add relations or dimensions to items which are now undefined (assuming it was fully defined to begin with and you wish to redefine it fully).
This is a more robust method to find and remove dangling relations in sketches of any size.
I use a similar method when taking a virtual part, defined in context, and strip it of its External relations to replace with dimensions so that I can save it independently as a file outside of context. This is useful when creating a new copy of an assembly which contains virtual parts, as once you begin editing them, they complain a lot about not being able to add new relations to this because it has relations in an outside context. I remove those offending contexts, so that I can re-relate it in its new context or keep it independent.
I just learned something. I mean, I know about the D/DR function, just never actually used it.
I'd be lost without it ....
You can suppress/unsuppress sketch relations to and these can be controlled for configurations.
Thanks Tom Gagnon, Nice tip!
Thanks everyone for the tips.
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